Discussion:
HEIDENHAIN iTNC 530 Tap Cycle Help Conversational Format
(too old to reply)
b***@gmail.com
2009-08-28 10:21:29 UTC
Permalink
Raw Message
Hi,

Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.

Regards
cncmillgil
2009-08-28 11:29:22 UTC
Permalink
Raw Message
Hi,
 Will someone post or email some programming example of a tap cycle.
 Specifically  CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
 I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
 CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
 Regards
We do have a Heidenhain 426 at work, but not equipped with tap
capabilities, so I'm told. I have only just begun figuring out
Heid'ies programing language & machine tool functions. I do have
manuals if they are similar to your 530 control?
Would appreciate if you figure it out, to post the code showing that.
Thx

======================================================
______
/_____/\ Best Regards,
/____ \\ \ Gil
/_____\ \\ / HOLDZEM©®
/_____/ \/ / / Made in USA
/_____/ / \//\ By an
\_____\//\ / / American Toolmaker
\_____/ / /\ / West Chicago, IL
\_____/ \\ \ USA
\_____\ \\
\_____\/
======================================================
Jerry
2009-08-28 16:24:18 UTC
Permalink
Raw Message
I've been working on 530 for last two and a half years and 420 before that.
I'm at home so if you can post or email me a blank code I will fill it in
for you.
Jerry
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
cncmillgil
2009-09-02 11:58:55 UTC
Permalink
Raw Message
Post by Jerry
I've been working on 530 for last two and a half years and 420 before that.
I'm at home so if you can post or email me a blank code I will fill it in
for you.
Jerry
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically  CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Jerry, sounds like your the Heidi guy?
If you have second, could you post the code to sweep a like a 1"rad
across X using Y-Z with say a 1/4"ball EM?- Any example will do, can't
be that hard. I'm close.
I've put in the example in the book, but it does not seem to be
working properly with my dim's input.
I'm a newbee to Heidi's conversational. Aint like no other I've run
across. Kinda funuc macro/type hybrid- in a "league of its own".
Actually really nice. They were way ahead of there time, considering
its a mid 90's setup. I think it can blow away Hurco at certian
things?
If I can figure out how to hook the laptop up to it, one of these
days, I'll pull out some of the prog's to play with.
The other opition I have with this beast, is using ISO. Any experience
with that?
Any help would be appreciated.
FYI this machine was never really used to its full capabilities, by
what I'm seeing. Only been at this place for 8mo now - still
learning<g>

--


\|||/
(o o)
______.oOO-(_)-OOo.____________________
~ Gil ~
the HOLDZEM©® king
Jerry
2009-09-02 21:03:50 UTC
Permalink
Raw Message
I will try to make that program tomorrow if I have few minutes. I don't
program in ISO as Heidenhain is way nicer.
Jerry
Post by Jerry
I've been working on 530 for last two and a half years and 420 before that.
I'm at home so if you can post or email me a blank code I will fill it in
for you.
Jerry
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Jerry, sounds like your the Heidi guy?
If you have second, could you post the code to sweep a like a 1"rad
across X using Y-Z with say a 1/4"ball EM?- Any example will do, can't
be that hard. I'm close.
I've put in the example in the book, but it does not seem to be
working properly with my dim's input.
I'm a newbee to Heidi's conversational. Aint like no other I've run
across. Kinda funuc macro/type hybrid- in a "league of its own".
Actually really nice. They were way ahead of there time, considering
its a mid 90's setup. I think it can blow away Hurco at certian
things?
If I can figure out how to hook the laptop up to it, one of these
days, I'll pull out some of the prog's to play with.
The other opition I have with this beast, is using ISO. Any experience
with that?
Any help would be appreciated.
FYI this machine was never really used to its full capabilities, by
what I'm seeing. Only been at this place for 8mo now - still
learning<g>

--


\|||/
(o o)
______.oOO-(_)-OOo.____________________
~ Gil ~
the HOLDZEM©® king
Jerry
2009-09-03 21:39:59 UTC
Permalink
Raw Message
Below are two simplest examples to do rad. One milling in X and other
milling along the rad.
Jerry


0 BEGIN PGM rad1 INCH
1 BLK FORM 0.1 Z X+0 Y+0 Z-2
2 BLK FORM 0.2 X+3 Y+3 Z+0
3 TOOL CALL 18 Z S5000
4 * - 0.25" ballnose
5 * - 0.5" rad
6 * - machining along X axis
7 CYCL DEF 247 DATUM SETTING ~
Q339=+0 ;DATUM NUMBER
8 L X-0.2 Y-0.125 R0 FMAX M3
9 L Z+0 R0 FMAX M8
10 CC Y+0.5 Z-0.625
11 L Z-0.625 R0 F500
12 LBL 1
13 LP IPA-5 R0
14 L X+3.2
15 LP IPA-5
16 L X-0.2
17 LBL 0
18 CALL LBL 1 REP8
19 L Z+6 R0 FMAX M9 M5
20 L Z-0.1 Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad1 INCH


0 BEGIN PGM rad2 INCH
1 BLK FORM 0.1 Z X+0 Y+0 Z-2
2 BLK FORM 0.2 X+3 Y+3 Z+0
3 TOOL CALL 18 Z S5000
4 * - 0.25" ballnose
5 * - 0.5" rad
6 * - machining along radius
7 CYCL DEF 247 DATUM SETTING ~
Q339=+0 ;DATUM NUMBER
8 L X-0.2 Y-0.125 R0 FMAX M3
9 L Z+0 R0 FMAX M8
10 CC Y+0.5 Z-0.625
11 L Z-0.625 R0 F500
12 LBL 1
13 L IX+0.01
14 CP IPA-90 DR-
15 L IX+0.01
16 CP IPA+90 DR+
17 LBL 0
18 CALL LBL 1 REP160
19 L Z+6 R0 FMAX M9 M5
20 L Z-0.1 Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad2 INCH
Post by Jerry
I've been working on 530 for last two and a half years and 420 before that.
I'm at home so if you can post or email me a blank code I will fill it in
for you.
Jerry
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Jerry, sounds like your the Heidi guy?
If you have second, could you post the code to sweep a like a 1"rad
across X using Y-Z with say a 1/4"ball EM?- Any example will do, can't
be that hard. I'm close.
I've put in the example in the book, but it does not seem to be
working properly with my dim's input.
I'm a newbee to Heidi's conversational. Aint like no other I've run
across. Kinda funuc macro/type hybrid- in a "league of its own".
Actually really nice. They were way ahead of there time, considering
its a mid 90's setup. I think it can blow away Hurco at certian
things?
If I can figure out how to hook the laptop up to it, one of these
days, I'll pull out some of the prog's to play with.
The other opition I have with this beast, is using ISO. Any experience
with that?
Any help would be appreciated.
FYI this machine was never really used to its full capabilities, by
what I'm seeing. Only been at this place for 8mo now - still
learning<g>

--


\|||/
(o o)
______.oOO-(_)-OOo.____________________
~ Gil ~
the HOLDZEM©® king
Jerry
2009-09-02 21:05:59 UTC
Permalink
Raw Message
This is a simple program to tap 1/2-13 hole with two different cycles. Your
machine zero may be different.
Jerry

0 BEGIN PGM tap INCH
1 * - 1/2-13 tap, M3 not needed because spindle has to stop anyway to
orient
2 * - examples of 2 taping cycles
3 BLK FORM 0.1 Z X-5 Y-5 Z-2
4 BLK FORM 0.2 X+5 Y+5 Z+0
5 TOOL CALL 1 Z S1000
6 CYCL DEF 247 DATUM SETTING ~
Q339=+1 ;DATUM NUMBER
7 L X+0 Y+0 R0 FMAX
8 L Z+0.2 R0 FMAX M8
9 CYCL DEF 207 RIGID TAPPING NEW ~
Q200=+0.2 ;SET-UP CLEARANCE ~
Q201=-0.7 ;DEPTH OF THREAD ~
Q239=+0.07692 ;THREAD PITCH ~
Q203=+0 ;SURFACE COORDINATE ~
Q204=+0.2 ;2ND SET-UP CLEARANCE
10 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=+0.2 ;SET-UP CLEARANCE ~
Q201=-0.7 ;DEPTH OF THREAD ~
Q239=+0.07692 ;THREAD PITCH ~
Q203=+0 ;SURFACE COORDINATE ~
Q204=+0.2 ;2ND SET-UP CLEARANCE ~
Q257=+0.35 ;DEPTH FOR CHIP BRKNG ~
Q256=+0.03 ;DIST FOR CHIP BRKNG ~
Q336=+0 ;ANGLE OF SPINDLE
11 CYCL CALL
12 L Z+5 R0 FMAX M9 M5
13 L Z-0.1 Y-0.1 R0 FMAX M91
14 M30
15 END PGM tap INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
cncmillgil
2009-09-03 00:02:54 UTC
Permalink
Raw Message
This is  a simple program to tap 1/2-13 hole with two different cycles. Your
machine zero may be different.
Jerry
0  BEGIN PGM tap INCH
1  * - 1/2-13 tap, M3 not needed because spindle has to stop anyway to
orient
2  * - examples of 2 taping cycles
3  BLK FORM 0.1 Z  X-5  Y-5  Z-2
4  BLK FORM 0.2  X+5  Y+5  Z+0
5  TOOL CALL 1 Z S1000
6  CYCL DEF 247 DATUM SETTING ~
    Q339=+1    ;DATUM NUMBER
7  L  X+0  Y+0 R0 FMAX
8  L  Z+0.2 R0 FMAX M8
9  CYCL DEF 207 RIGID TAPPING NEW ~
    Q200=+0.2  ;SET-UP CLEARANCE ~
    Q201=-0.7  ;DEPTH OF THREAD ~
    Q239=+0.07692 ;THREAD PITCH ~
    Q203=+0    ;SURFACE COORDINATE ~
    Q204=+0.2  ;2ND SET-UP CLEARANCE
10 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
    Q200=+0.2  ;SET-UP CLEARANCE ~
    Q201=-0.7  ;DEPTH OF THREAD ~
    Q239=+0.07692 ;THREAD PITCH ~
    Q203=+0    ;SURFACE COORDINATE ~
    Q204=+0.2  ;2ND SET-UP CLEARANCE ~
    Q257=+0.35 ;DEPTH FOR CHIP BRKNG ~
    Q256=+0.03 ;DIST FOR CHIP BRKNG ~
    Q336=+0    ;ANGLE OF SPINDLE
11 CYCL CALL
12 L  Z+5 R0 FMAX M9 M5
13 L  Z-0.1  Y-0.1 R0 FMAX M91
14 M30
15 END PGM tap INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically  CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Jerry, Thx. The guys in the shop I'm at say that they could never get
the machine to tap. Saying it has to be equipped from the mfg. for
taping? & also use a floating tap holder? Both are also mentioned in
the manual.
Hell I've never seen a CNC that could not G84 tap?, with or without a
nice ext./comp.-slip clutch tap holder. Well I'm learn'in sumpin
new????
Like I stated previously Heidi's way is different.
We don't do alot of taping, plus we work with Titanium- real bear to
tap.
IMO Its not worth the chance on breaking a tap on, because usually 1
or 2 pcs in the order. TI is $$$ & so is EDM tap removal.
My main concern is, an easy way to sweep simple Y/Z or X/Z contours
across the block. The prog. manual has examples, but me not being
familiar with all the commands, like CT CC ect. makes it confusing to
apply to my work.
Shit today I just figured out repeat label with an incremental Z (IZ)
- the old loop tape method., only the repeat command counts how deep
to go the the incremantal Z. Sweet! sit back,relax & let the machine
do the work.
This thing is like play time for me. Being on a weirdo ANAYAK & no
toolchanger! I took a 3"wide 5mm dp. cut in TI the other day, the
whole machine osilated & howled! Never hear nothing like that before.
Nothing happend to the carbides on the face mill (positive 3/4"round
inserts), it was just as it entered on the part. After it was in the
cut no probelem. Sure did turn some heads. hehehehe. It has to be the
way the machine tool is designed. The Y travels the Z column with it,
not like most bed type mills where the Z is stationary & X/Y travel on
the bed. Must have been like the way covers, kinda tiny tattle sound??
thanks again for your help. If time permits & the opertunity comes up,
I would like to try your taping prog., even if its just to cut some
air :-)

--

Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterday's technology
building
Tomorrows Dreams
Jerry
2009-09-03 00:20:52 UTC
Permalink
Raw Message
I have never seen a CNC machine that could not tap. You may not be able to
rigid tap but with a floating holder you should have no problem.
As for CC it means circle center and you need it for C (circular) and CP (
circular polar). CR only needs end position of circle and radius.
The biggest fun on this control is to use variables (Qs). You can use it for
simple stuff like changing depth of cut , cutter compensation and such but
if you get really good with it you can actually use it for quite complex
surfacing.
Is your control 426 or 530?
Jerry
This is a simple program to tap 1/2-13 hole with two different cycles.
Your
machine zero may be different.
Jerry
0 BEGIN PGM tap INCH
1 * - 1/2-13 tap, M3 not needed because spindle has to stop anyway to
orient
2 * - examples of 2 taping cycles
3 BLK FORM 0.1 Z X-5 Y-5 Z-2
4 BLK FORM 0.2 X+5 Y+5 Z+0
5 TOOL CALL 1 Z S1000
6 CYCL DEF 247 DATUM SETTING ~
Q339=+1 ;DATUM NUMBER
7 L X+0 Y+0 R0 FMAX
8 L Z+0.2 R0 FMAX M8
9 CYCL DEF 207 RIGID TAPPING NEW ~
Q200=+0.2 ;SET-UP CLEARANCE ~
Q201=-0.7 ;DEPTH OF THREAD ~
Q239=+0.07692 ;THREAD PITCH ~
Q203=+0 ;SURFACE COORDINATE ~
Q204=+0.2 ;2ND SET-UP CLEARANCE
10 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=+0.2 ;SET-UP CLEARANCE ~
Q201=-0.7 ;DEPTH OF THREAD ~
Q239=+0.07692 ;THREAD PITCH ~
Q203=+0 ;SURFACE COORDINATE ~
Q204=+0.2 ;2ND SET-UP CLEARANCE ~
Q257=+0.35 ;DEPTH FOR CHIP BRKNG ~
Q256=+0.03 ;DIST FOR CHIP BRKNG ~
Q336=+0 ;ANGLE OF SPINDLE
11 CYCL CALL
12 L Z+5 R0 FMAX M9 M5
13 L Z-0.1 Y-0.1 R0 FMAX M91
14 M30
15 END PGM tap INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Jerry, Thx. The guys in the shop I'm at say that they could never get
the machine to tap. Saying it has to be equipped from the mfg. for
taping? & also use a floating tap holder? Both are also mentioned in
the manual.
Hell I've never seen a CNC that could not G84 tap?, with or without a
nice ext./comp.-slip clutch tap holder. Well I'm learn'in sumpin
new????
Like I stated previously Heidi's way is different.
We don't do alot of taping, plus we work with Titanium- real bear to
tap.
IMO Its not worth the chance on breaking a tap on, because usually 1
or 2 pcs in the order. TI is $$$ & so is EDM tap removal.
My main concern is, an easy way to sweep simple Y/Z or X/Z contours
across the block. The prog. manual has examples, but me not being
familiar with all the commands, like CT CC ect. makes it confusing to
apply to my work.
Shit today I just figured out repeat label with an incremental Z (IZ)
- the old loop tape method., only the repeat command counts how deep
to go the the incremantal Z. Sweet! sit back,relax & let the machine
do the work.
This thing is like play time for me. Being on a weirdo ANAYAK & no
toolchanger! I took a 3"wide 5mm dp. cut in TI the other day, the
whole machine osilated & howled! Never hear nothing like that before.
Nothing happend to the carbides on the face mill (positive 3/4"round
inserts), it was just as it entered on the part. After it was in the
cut no probelem. Sure did turn some heads. hehehehe. It has to be the
way the machine tool is designed. The Y travels the Z column with it,
not like most bed type mills where the Z is stationary & X/Y travel on
the bed. Must have been like the way covers, kinda tiny tattle sound??
thanks again for your help. If time permits & the opertunity comes up,
I would like to try your taping prog., even if its just to cut some
air :-)

--

Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterday's technology
building
Tomorrows Dreams
cncmillgil
2009-09-03 00:43:51 UTC
Permalink
Raw Message
Post by Jerry
I have never seen a CNC machine that could not tap. You may not be able to
rigid tap but with a floating holder you should have no problem.
As for CC it means circle center and you need it for C (circular) and CP (
circular polar). CR only needs end position of circle and radius.
The biggest fun on this control is to use variables (Qs). You can use it for
simple stuff like changing depth of cut , cutter compensation and such but
if you get really good with it you can actually use it for quite complex
surfacing.
Is your control 426 or 530?
Jerry
This is a simple program to tap 1/2-13 hole with two different cycles.
Your
machine zero may be different.
Jerry
0 BEGIN PGM tap INCH
1 * - 1/2-13 tap, M3 not needed because spindle has to stop anyway to
orient
2 * - examples of 2 taping cycles
3 BLK FORM 0.1 Z X-5 Y-5 Z-2
4 BLK FORM 0.2 X+5 Y+5 Z+0
5 TOOL CALL 1 Z S1000
6 CYCL DEF 247 DATUM SETTING ~
Q339=+1 ;DATUM NUMBER
7 L X+0 Y+0 R0 FMAX
8 L Z+0.2 R0 FMAX M8
9 CYCL DEF 207 RIGID TAPPING NEW ~
Q200=+0.2 ;SET-UP CLEARANCE ~
Q201=-0.7 ;DEPTH OF THREAD ~
Q239=+0.07692 ;THREAD PITCH ~
Q203=+0 ;SURFACE COORDINATE ~
Q204=+0.2 ;2ND SET-UP CLEARANCE
10 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=+0.2 ;SET-UP CLEARANCE ~
Q201=-0.7 ;DEPTH OF THREAD ~
Q239=+0.07692 ;THREAD PITCH ~
Q203=+0 ;SURFACE COORDINATE ~
Q204=+0.2 ;2ND SET-UP CLEARANCE ~
Q257=+0.35 ;DEPTH FOR CHIP BRKNG ~
Q256=+0.03 ;DIST FOR CHIP BRKNG ~
Q336=+0 ;ANGLE OF SPINDLE
11 CYCL CALL
12 L Z+5 R0 FMAX M9 M5
13 L Z-0.1 Y-0.1 R0 FMAX M91
14 M30
15 END PGM tap INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Jerry, Thx. The guys in the shop I'm at say that they could never get
the machine to tap. Saying it has to be equipped from the mfg. for
taping? & also use a floating tap holder? Both are also mentioned in
the manual.
Hell I've never seen a CNC that could not G84 tap?, with or without a
nice ext./comp.-slip clutch tap holder. Well I'm learn'in sumpin
new????
Like I stated previously Heidi's way is different.
We don't do alot of taping, plus we work with Titanium- real bear to
tap.
IMO Its not worth the chance on breaking a tap on, because usually 1
or 2 pcs in the order. TI is $$$ & so is EDM tap removal.
My main concern is, an easy way to sweep simple Y/Z or X/Z contours
across the block. The prog. manual has examples, but me not being
familiar with all the commands, like CT CC ect. makes it confusing to
apply to my work.
Shit today I just figured out repeat label with an incremental Z (IZ)
- the old loop tape method., only the repeat command counts how deep
to go the the incremantal Z. Sweet! sit back,relax & let the machine
do the work.
This thing is like play time for me. Being on a weirdo ANAYAK & no
toolchanger! I took a 3"wide 5mm dp. cut in TI the other day, the
whole machine osilated & howled! Never hear nothing like that before.
Nothing happend to the carbides on the face mill (positive 3/4"round
inserts), it was just as it entered on the part. After it was in the
cut no probelem. Sure did turn some heads. hehehehe. It has to be the
way the machine tool is designed. The Y travels the Z column with it,
not like most bed type mills where the Z is stationary & X/Y travel on
the bed. Must have been like the way covers, kinda tiny tattle sound??
thanks again for your help. If time permits & the opertunity comes up,
I would like to try your taping prog., even if its just to cut some
air :-)
--
        Gil©
      Member of
 ==American Toolmakers==
 using the "old world" ways
with yesterday's technology
       building
    Tomorrows Dreams
Ya your right CNC's all tap - I've put 1/2 * 3/8 taps in drill chucks
& taped. After a few holes the tap pushes up(always), just feed hold,
rejust & go!

Heidi's converational looks very powerfull for easy 3D shapes. It's
just nobody ever dove in to it to make it work to its full extents
previously at my place. Plus the boss like's Hurco's & so do I. Too
bad, not much effort is going to be spent on the ol Heidi/Anayak. The
table is huge, they could realy use a 4axis with a center/tailstock to
cut round pcs to rectangle on the ends. Could even be a cheaper 4pos
indexer? & the head swivels & looks like the control can be reset on
that plane angle for axis travels?
They are looking down the road of CNC lathe with live tooling.

--

___ ___
/ \ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------------ \ \/\/
\ _\/ \__\/

Gil©
Cliff
2009-09-03 20:59:45 UTC
Permalink
Raw Message
Post by cncmillgil
I took a 3"wide 5mm dp. cut in TI the other day, the
whole machine osilated & howled! Never hear nothing like that before.
Nothing happend to the carbides on the face mill (positive 3/4"round
inserts), it was just as it entered on the part. After it was in the
cut no probelem. Sure did turn some heads. hehehehe. It has to be the
way the machine tool is designed. The Y travels the Z column with it,
not like most bed type mills where the Z is stationary & X/Y travel on
the bed. Must have been like the way covers, kinda tiny tattle sound??
Slop in the ways or a screw/nut?
Use indicator & 2X4 to pry & see what moves.
--
Cliff
cncmillgil
2009-09-04 03:17:16 UTC
Permalink
Raw Message
Post by cncmillgil
I took a 3"wide 5mm dp. cut in TI the other day, the
whole machine osilated & howled! Never hear nothing like that before.
Nothing happend to the carbides on the face mill (positive 3/4"round
inserts), it was just as it entered on the part. After it was in the
cut no probelem. Sure did turn some heads. hehehehe. It has to be the
way the machine tool is designed. The Y travels the Z column with it,
not like most bed type mills where the Z is stationary & X/Y travel on
the bed. Must have been like the way covers, kinda tiny tattle sound??
  Slop in the ways or a screw/nut?
  Use indicator & 2X4 to pry & see what moves.
--
Cliff
Could be.. but I dont think so. Just by standard indicator use, you
can kinda tell how much approx back lash is in the screw/nut just by
reversing a jog increment like .001. How many clicks to get the
indicator ro move?= approx back lash? Usually a half ass indication of
how many time's she been crashed <g>... But............... this pig
has Heidenhien glass $scales$ on the all 3 axis table travels unlike
standard CNC resolver or feedback from the drive moter/screw rotation-
iregardless to actual table position. So what does that mean? All back
lash & end thrust is compensated by the controler auto-magicly? maybe.
Any hoot, I looked for the Q209 taping cycle today, it aint got it.
Is the 530 control newer than the 426? dumb question. never mind.
Looks like I'll have to play with what I know: ISO-G-CODE for taping.
Whole thing is, most who have Heidi's dont use ISO.
I have to say, again, this is the wierdest damn CNC machine I've ever
run across. I've seen a few in my trip around the mold shop block.
Not only the control, but the machine tool itself! No shit, this
morning, just for shits& giggles, I timed myself from flip power
switch on to cutter in steel cutting. Any guess's?
30 sec max! No shit......... well a few things have to be in place the
day before. Like Z almost to upper limit, setup/prog/block the same.
So its turn on & continue cutting. But 30 sec? hell the Hurco takes
5min before you can open the network drive up & begin to start looking
for a file, let alone login-P/W machine/toolchanger calibration. The
Roders some times took an hour before it would go. Freekin old
Fadels...... shit, look out you could be miss-aligned instead of
aligned. So the majority of CNC's must be calibrated/aligened by
traveling the XYZ to extents-hitting the overtavel limit switch, then
screw rotation for align at a slooooooowwwwww feedrate of course. The
the tool changer has to go around the world a few times, hopfully not
asking which tool is in the spindle, because I plain ass forgot from
yesterday. SOB if i tell it the wrong tool, guess what? (I will not
crash the tool changer, I will not crash the tool changer, I will not
crash the tool changer, I will not crash the tool changer,)<g> Shit,
ever see wore out tool arm grippers? wHam! tool in the back of the
inclosure. How bout worn out carousel grippers? Tool falls out right
over your piece- hello mr. welder?
How come this shit only happens to me? :-)
So I guess this Hedidenhain/Anayak is my punshment? reward? for all
those years of "other" machine tools. We'll see, the saga
continues.........

Loading Image...


--

___ ___
/ \ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------------ \ \/\/
\ _\/ \__\/

Gil©
==American Toolmaker==
*born & raised in the USA*
Jerry
2009-09-04 16:25:18 UTC
Permalink
Raw Message
Below is a taping cycle for 426. You should be able to find it under
drilling, move cursor to second page and pick cycle 2.
Jerry

0 BEGIN PGM 426tap INCH
1 TOOL DEF 1 L+0 R+0.25
2 TOOL CALL 1 Z S500
3 * - 1/2-13 tap
4 * - to figure out 2.4( feed rate) 1 div pitch times rpm (1/13=0.7692
*500~
rpm=38.46
5 CYCL DEF 2.0 TAPPING
6 CYCL DEF 2.1 SET UP0.1
7 CYCL DEF 2.2 DEPTH-0.5
8 CYCL DEF 2.3 DWELL0
9 CYCL DEF 2.4 F38.46
10 L X+0 Y+0 R0 FMAX M3
11 L Z+0.1 R0 FMAX M8
12 CYCL CALL
13 L Z+6 R0 FMAX M9 M5
14 M30
15 END PGM 426tap INCH
Post by Cliff
Post by cncmillgil
I took a 3"wide 5mm dp. cut in TI the other day, the
whole machine osilated & howled! Never hear nothing like that before.
Nothing happend to the carbides on the face mill (positive 3/4"round
inserts), it was just as it entered on the part. After it was in the
cut no probelem. Sure did turn some heads. hehehehe. It has to be the
way the machine tool is designed. The Y travels the Z column with it,
not like most bed type mills where the Z is stationary & X/Y travel on
the bed. Must have been like the way covers, kinda tiny tattle sound??
Slop in the ways or a screw/nut?
Use indicator & 2X4 to pry & see what moves.
--
Cliff
Could be.. but I dont think so. Just by standard indicator use, you
can kinda tell how much approx back lash is in the screw/nut just by
reversing a jog increment like .001. How many clicks to get the
indicator ro move?= approx back lash? Usually a half ass indication of
how many time's she been crashed <g>... But............... this pig
has Heidenhien glass $scales$ on the all 3 axis table travels unlike
standard CNC resolver or feedback from the drive moter/screw rotation-
iregardless to actual table position. So what does that mean? All back
lash & end thrust is compensated by the controler auto-magicly? maybe.
Any hoot, I looked for the Q209 taping cycle today, it aint got it.
Is the 530 control newer than the 426? dumb question. never mind.
Looks like I'll have to play with what I know: ISO-G-CODE for taping.
Whole thing is, most who have Heidi's dont use ISO.
I have to say, again, this is the wierdest damn CNC machine I've ever
run across. I've seen a few in my trip around the mold shop block.
Not only the control, but the machine tool itself! No shit, this
morning, just for shits& giggles, I timed myself from flip power
switch on to cutter in steel cutting. Any guess's?
30 sec max! No shit......... well a few things have to be in place the
day before. Like Z almost to upper limit, setup/prog/block the same.
So its turn on & continue cutting. But 30 sec? hell the Hurco takes
5min before you can open the network drive up & begin to start looking
for a file, let alone login-P/W machine/toolchanger calibration. The
Roders some times took an hour before it would go. Freekin old
Fadels...... shit, look out you could be miss-aligned instead of
aligned. So the majority of CNC's must be calibrated/aligened by
traveling the XYZ to extents-hitting the overtavel limit switch, then
screw rotation for align at a slooooooowwwwww feedrate of course. The
the tool changer has to go around the world a few times, hopfully not
asking which tool is in the spindle, because I plain ass forgot from
yesterday. SOB if i tell it the wrong tool, guess what? (I will not
crash the tool changer, I will not crash the tool changer, I will not
crash the tool changer, I will not crash the tool changer,)<g> Shit,
ever see wore out tool arm grippers? wHam! tool in the back of the
inclosure. How bout worn out carousel grippers? Tool falls out right
over your piece- hello mr. welder?
How come this shit only happens to me? :-)
So I guess this Hedidenhain/Anayak is my punshment? reward? for all
those years of "other" machine tools. We'll see, the saga
continues.........

http://users.cin.net/~milgil/SeniorAnayak.jpg


--

___ ___
/ \ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------------ \ \/\/
\ _\/ \__\/

Gil©
==American Toolmaker==
*born & raised in the USA*
Cliff
2009-09-04 16:45:56 UTC
Permalink
Raw Message
Post by cncmillgil
Post by cncmillgil
I took a 3"wide 5mm dp. cut in TI the other day, the
whole machine osilated & howled! Never hear nothing like that before.
Nothing happend to the carbides on the face mill (positive 3/4"round
inserts), it was just as it entered on the part. After it was in the
cut no probelem. Sure did turn some heads. hehehehe. It has to be the
way the machine tool is designed. The Y travels the Z column with it,
not like most bed type mills where the Z is stationary & X/Y travel on
the bed. Must have been like the way covers, kinda tiny tattle sound??
  Slop in the ways or a screw/nut?
  Use indicator & 2X4 to pry & see what moves.
--
Cliff
Could be.. but I dont think so.
Backlash in the spindle's drivetrain?
--
Cliff
cncmillgil
2009-09-05 00:11:45 UTC
Permalink
Raw Message
Post by cncmillgil
Post by cncmillgil
I took a 3"wide 5mm dp. cut in TI the other day, the
whole machine osilated & howled! Never hear nothing like that before.
Nothing happend to the carbides on the face mill (positive 3/4"round
inserts), it was just as it entered on the part. After it was in the
cut no probelem. Sure did turn some heads. hehehehe. It has to be the
way the machine tool is designed. The Y travels the Z column with it,
not like most bed type mills where the Z is stationary & X/Y travel on
the bed. Must have been like the way covers, kinda tiny tattle sound??
  Slop in the ways or a screw/nut?
  Use indicator & 2X4 to pry & see what moves.
--
Cliff
Could be.. but I dont think so.
  Backlash in the spindle's drivetrain?
--
Cliff
Hmmmm......... its a gear drive head. max RPM 4K! hehehehe. But I'm
not allowed to use that much. Aparentley the head heats up after??? &
all the seals peuch oil. Oh boy..... kinda reminds of the ol
Cincinnati Milcron 10v 2000 gear drive head. The first hour in the
morning hydraulic oil seeped down to & thru the lower spindle outter
bearings. We had a tin drip pan under the spindle for about 10min with
it running to catch the drain oil. Run when first Turing on the
spindle, else your very spotty after that.<g>
Well today was another learning experience on the beast. Heidi's way
to mill a circle. WTH? Its just me. Not used to their "lingo" It aint
G98/G99
fer rapid & travel planes- no damn R plane......... I'm lost. No G2/G3
its RL RL.
Ah its just another language to add to all the rest of the cultural
melting pots I've been in. DOS,UNIX,LINUX,WinBlows,
Chinese,Polish,Laos,German,Russian,Swede, & of course See Habla press
uono for gringo - dose for espanyol.

Hey anyone know about TIVO's? I wana hack into mine. Its an old Series
2 40hr record time. Works sweet! fer 20bucks at a garage sale. Their
video play back/recording/FFwd/frame-frame is far superior my
DishNetwork satellite DVR. By what I'm finding, its a Linux computer,
programed to do what Tivo lets you to do.
Not good enough for me. I want full control of the DVR/hard drive &
file structure. I dont care about signing up for a tivo contract.
http://electronics.howstuffworks.com/tivo.htm

--

Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterdays technology
building
Tomorrows Dreams
Cliff
2009-09-05 06:29:49 UTC
Permalink
Raw Message
Post by cncmillgil
Hey anyone know about TIVO's? I wana hack into mine.
There may be newsgroup .... probably a BBS too.
--
Cliff
b***@gmail.com
2009-09-07 14:37:37 UTC
Permalink
Raw Message
Hi,
 Will someone post or email some programming example of a tap cycle.
 Specifically  CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
 I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
 CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
 Regards
Thanks for your posts. Norman at Bostomatic, too.

Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.

Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?

And just in case you have concerns about running Internet servers out
of drive space ..... I didn't want to edit the program for length lest
I delete something which might lead to confusion.

;
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
;
;09/01/2009 08:08:08 AM
; C:\TAP THIS
;
;
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
;
;
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
;
;
CYCL DEF 32.0 TOLERANCE
CYCL DEF 32.1 T0.001
CYCL DEF 32.2 HSC-MODE:0 TA0.01
;
;
; TOOL NUMBER - 10
; DESCRIPTION - CDRILL
; TOOL LENGTH FROM HOLDER 2.000
;
; TOOL NUMBER - 11
; DESCRIPTION - .070DIA
; TOOL LENGTH FROM HOLDER 3.500
;
; TOOL NUMBER - 12
; DESCRIPTION - 2-56 TAP
; TOOL LENGTH FROM HOLDER 2.000
;
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
;
;***CDRILL***
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000
;
;***DRILL***
60 L X.3835 Y.1625 R0 FMAX M3
70 L Z.05 FMAX
80 M8
90 L Z.05 FMAX
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
;
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
;
;
;***.070DIA***
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
790 TOOL CALL 11 Z S2000
;
;***.070 DRILL***
800 L X.3835 Y.1625 R0 FMAX M3
810 L Z.05 FMAX
820 M8
830 L Z.05 FMAX
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
850 L X.3835 Y.1625 FMAX M3
860 CYCL CALL
870 L X1.0385 FMAX M99
880 L X1.6935 FMAX M99
890 L X2.3485 FMAX M99
900 L X3.0035 FMAX M99
910 L X3.6585 FMAX M99
920 L X4.3135 FMAX M99
930 L X4.9685 FMAX M99
940 L X4.3769 Y-.1625 FMAX M99
950 L X3.7219 FMAX M99
960 L X3.0669 FMAX M99
970 L X2.4119 FMAX M99
980 L X1.7569 FMAX M99
990 L X1.1019 FMAX M99
1000 L X.4469 FMAX M99
1010 L X-.2081 FMAX M99
1020 L X.3835 Y-.3825 FMAX M99
1030 L X1.0385 FMAX M99
1040 L X1.6935 FMAX M99
1050 L X2.3485 FMAX M99
1060 L X3.0035 FMAX M99
1070 L X3.6585 FMAX M99
1080 L X4.3135 FMAX M99
1090 L X4.9685 FMAX M99
1100 L X4.3769 Y-.7075 FMAX M99
1110 L X3.7219 FMAX M99
1120 L X3.0669 FMAX M99
1130 L X2.4119 FMAX M99
1140 L X1.7569 FMAX M99
1150 L X1.1019 FMAX M99
1160 L X.4469 FMAX M99
1170 L X-.2081 FMAX M99
1180 L X.3835 Y-.9275 FMAX M99
1190 L X1.0385 FMAX M99
1200 L X1.6935 FMAX M99
1210 L X2.3485 FMAX M99
1220 L X3.0035 FMAX M99
1230 L X3.6585 FMAX M99
1240 L X4.3135 FMAX M99
1250 L X4.9685 FMAX M99
1260 L X4.3769 Y-1.2525 FMAX M99
1270 L X3.7219 FMAX M99
1280 L X3.0669 FMAX M99
1290 L X2.4119 FMAX M99
1300 L X1.7569 FMAX M99
1310 L X1.1019 FMAX M99
1320 L X.4469 FMAX M99
1330 L X-.2081 FMAX M99
1340 L X.3835 Y-1.4725 FMAX M99
1350 L X1.0385 FMAX M99
1360 L X1.6935 FMAX M99
1370 L X2.3485 FMAX M99
1380 L X3.0035 FMAX M99
1390 L X3.6585 FMAX M99
1400 L X4.3135 FMAX M99
1410 L X4.9685 FMAX M99
1420 L X4.3769 Y-1.7975 FMAX M99
1430 L X3.7219 FMAX M99
1440 L X3.0669 FMAX M99
1450 L X2.4119 FMAX M99
1460 L X1.7569 FMAX M99
1470 L X1.1019 FMAX M99
1480 L X.4469 FMAX M99
1490 L X-.2081 FMAX M99
;
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
;
;
;***2-56 TAP***
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
;
;***2-56 TAP***
1540 L X.3835 Y.1625 R0 FMAX M3
1550 L Z.05 FMAX
1560 M8
1570 L FMAX
1580 L Z.05 FMAX
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1600 L X.3835 Y.1625 FMAX
1610 CYCL CALL
1620 L X1.0385 FMAX M99
1630 L X1.6935 FMAX M99
1640 L X2.3485 FMAX M99
1650 L X3.0035 FMAX M99
1660 L X3.6585 FMAX M99
1670 L X4.3135 FMAX M99
1680 L X4.9685 FMAX M99
1690 L X4.3769 Y-.1625 FMAX M99
1700 L X3.7219 FMAX M99
1710 L X3.0669 FMAX M99
1720 L X2.4119 FMAX M99
1730 L X1.7569 FMAX M99
1740 L X1.1019 FMAX M99
1750 L X.4469 FMAX M99
1760 L X-.2081 FMAX M99
1770 L X.3835 Y-.3825 FMAX M99
1780 L X1.0385 FMAX M99
1790 L X1.6935 FMAX M99
1800 L X2.3485 FMAX M99
1810 L X3.0035 FMAX M99
1820 L X3.6585 FMAX M99
1830 L X4.3135 FMAX M99
1840 L X4.9685 FMAX M99
1850 L X4.3769 Y-.7075 FMAX M99
1860 L X3.7219 FMAX M99
1870 L X3.0669 FMAX M99
1880 L X2.4119 FMAX M99
1890 L X1.7569 FMAX M99
1900 L X1.1019 FMAX M99
1910 L X.4469 FMAX M99
1920 L X-.2081 FMAX M99
1930 L X.3835 Y-.9275 FMAX M99
1940 L X1.0385 FMAX M99
1950 L X1.6935 FMAX M99
1960 L X2.3485 FMAX M99
1970 L X3.0035 FMAX M99
1980 L X3.6585 FMAX M99
1990 L X4.3135 FMAX M99
2000 L X4.9685 FMAX M99
2010 L X4.3769 Y-1.2525 FMAX M99
2020 L X3.7219 FMAX M99
2030 L X3.0669 FMAX M99
2040 L X2.4119 FMAX M99
2050 L X1.7569 FMAX M99
2060 L X1.1019 FMAX M99
2070 L X.4469 FMAX M99
2080 L X-.2081 FMAX M99
2090 L X.3835 Y-1.4725 FMAX M99
2100 L X1.0385 FMAX M99
2110 L X1.6935 FMAX M99
2120 L X2.3485 FMAX M99
2130 L X3.0035 FMAX M99
2140 L X3.6585 FMAX M99
2150 L X4.3135 FMAX M99
2160 L X4.9685 FMAX M99
2170 L X4.3769 Y-1.7975 FMAX M99
2180 L X3.7219 FMAX M99
2190 L X3.0669 FMAX M99
2200 L X2.4119 FMAX M99
2210 L X1.7569 FMAX M99
2220 L X1.1019 FMAX M99
2230 L X.4469 FMAX M99
2240 L X-.2081 FMAX M99
;
2250 M9
2260 M5
;
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
;
L R0 FMAX
M30
END PGM 1 INCH
Jerry
2009-09-07 16:36:05 UTC
Permalink
Raw Message
Every time you define a cycle like drilling or taping it takes precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say depth all you
have to do is describe new Q value.
For example you drill hole 1" deep (Q201=-0.055 ;DEPTH) before next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5" deep.
Same with any other Q value in cycles. You could make a say LBL 10 with any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I did with
your program below.
All your positioning is in a label and is called up with every tool. Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.

0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Thanks for your posts. Norman at Bostomatic, too.

Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.

Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?

And just in case you have concerns about running Internet servers out
of drive space ..... I didn't want to edit the program for length lest
I delete something which might lead to confusion.
cncmillgil
2009-09-08 11:19:46 UTC
Permalink
Raw Message
Post by Jerry
Every time you define a cycle like drilling or taping it takes precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say depth all you
have to do is describe new Q value.
For example  you drill hole 1" deep (Q201=-0.055 ;DEPTH) before next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5" deep.
Same with any other Q value in cycles. You could make a  say LBL 10 with any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I did with
your program below.
All your positioning is in a label and is called up with every tool. Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z  X-1.0  Y-1.0  Z-1.1
BLK FORM 0.2  X+1.0  Y+1.0  Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1;   WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL  TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
     Q200=0.05 ;SET-UP CLEARANCE~
     Q201=-0.055 ;DEPTH~
     Q206=15 ;FEED RATE~
     Q202=0.03 ;PLUNGE DEPTH~
     Q203=0.0 ;SURFACE COORDINATE~
     Q204=0.05 ;2ND SET-UP CLEARANCE~
     Q212=0. ;DECREMENT~
     Q205=0.0 ;MIN. PLUNGE DEPTH~
     Q258=0.02 ;UPPER ADV STOP DIST~
     Q259=0.04 ;LOWER ADV STOP DIST~
     Q257=0 ;DEPTH FOR CHIP BREAKING~
     Q256=0.02 ;DIST. FOR CHIP BREAKING~
     Q211=1.0 ;DWELL AT DEPTH~
     Q379=0 ;RETRACT FEED RATE~
     Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
     Q200=0.05 ;SET-UP CLEARANCE~
     Q201=-0.28 ;DEPTH~
     Q206=13 ;FEED RATE~
     Q202=0.06 ;PLUNGE DEPTH~
     Q203=0.0 ;SURFACE COORDINATE~
     Q204=0.05 ;2ND SET-UP CLEARANCE~
     Q212=0. ;DECREMENT~
     Q205=0.0 ;MIN. PLUNGE DEPTH~
     Q258=0.02 ;UPPER ADV STOP DIST~
     Q259=0.04 ;LOWER ADV STOP DIST~
     Q257=0 ;DEPTH FOR CHIP BREAKING~
     Q256=0.02 ;DIST. FOR CHIP BREAKING~
     Q211=1.0 ;DWELL AT DEPTH~
     Q379=0 ;RETRACT FEED RATE~
     Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG  ~
     Q200=0.05 ;SET-UP CLEARANCE~
     Q201=-0.265 ;DEPTH OF THREAD  ~
     Q239=0.0179 ;PITCH OF THREAD  ~
     Q203=0.0 ;SURFACE COORDINATE~
     Q204=0.05 ;2ND SET-UP CLEARANCE~
     Q257=0.085 ;DEPTH FOR CHIP BRKNG  ~
     Q256=0.02 ;DIST FOR CHIP BRKNG  ~
     Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Thanks for your posts. Norman at Bostomatic, too.
Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.
 Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?
 And just in case you have concerns about running Internet servers out
of drive space ..... I didn't want to edit the program for length lest
I delete something which might lead to confusion.
Thanks guys for the posts on Heidi's cycles.
Looks like the 530 control has a lot more cycles than than the ol 426
I'm on.

Billynevada: What CAM system outputs Heidi format? I was thinking only
ISO?
Also guys, what machine tools is the control on?

Last Fri, I had a 24"sqr electrical cabinet the service guys wanted a
"nice" 5" hole thru. What a fascicle. Setup top of the 2 kurts clapmed
to wood.
There was about 3/16-1/4" clearance to get the tool over & in. I
thought I had more, but turns out the last little bit, maybe 1/2" of Z
travel close to the upper limit switch is not usable during cycle.
Only took an hour or so to figure that out. So after machine
alignment, Z backs off the upper switch, so that position is max Z.

What's the cycle to just plunge & mill a circle- letting letting the
slug fall? I only found pocketing(taking the middle out), but thats
not what I wanted. Maybe there is no cycle, & its just input of circle
cent & rad? Remember I have a vintage 1996 - 426.
Hey that sounds like an old Hemi moter only 66-426?<g>

Thanks for your help.

--

Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterday's technology
building
Tomorrows Dreams!
Cliff
2009-09-08 19:26:52 UTC
Permalink
Raw Message
Post by cncmillgil
Thanks for your help.
http://www.heidenhain.com/index.php?WCMSGroup_2238_177=2243&WCMSGroup_2243_177=779

??
Jerry
2009-09-08 22:14:46 UTC
Permalink
Raw Message
Hi cncmillgil.
It is so easy to mill a circle like you describing there is no sense to use
a cycle.
All you do is to go to center of your pocket and down in Z and
CC IX0 IY0
LP PR 2.5 PA 0 RL F
ICP +360 DR+
Done.
If you want to do this on 426 with a cycle you can lie to the control and
add an even round number to you comp and the same to rad of your circle.
This way cutter will go straight to the edge of your circle.
We have Butlers, Correas and DMG with this control in our shop and if you
programming on the machine and you are good you can program it faster than
any other control I have ever seen.
Jerry
Post by Jerry
Every time you define a cycle like drilling or taping it takes precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say depth all you
have to do is describe new Q value.
For example you drill hole 1" deep (Q201=-0.055 ;DEPTH) before next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5" deep.
Same with any other Q value in cycles. You could make a say LBL 10 with
any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I did with
your program below.
All your positioning is in a label and is called up with every tool. Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Thanks for your posts. Norman at Bostomatic, too.
Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.
Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?
And just in case you have concerns about running Internet servers out
of drive space ..... I didn't want to edit the program for length lest
I delete something which might lead to confusion.
Thanks guys for the posts on Heidi's cycles.
Looks like the 530 control has a lot more cycles than than the ol 426
I'm on.

Billynevada: What CAM system outputs Heidi format? I was thinking only
ISO?
Also guys, what machine tools is the control on?

Last Fri, I had a 24"sqr electrical cabinet the service guys wanted a
"nice" 5" hole thru. What a fascicle. Setup top of the 2 kurts clapmed
to wood.
There was about 3/16-1/4" clearance to get the tool over & in. I
thought I had more, but turns out the last little bit, maybe 1/2" of Z
travel close to the upper limit switch is not usable during cycle.
Only took an hour or so to figure that out. So after machine
alignment, Z backs off the upper switch, so that position is max Z.

What's the cycle to just plunge & mill a circle- letting letting the
slug fall? I only found pocketing(taking the middle out), but thats
not what I wanted. Maybe there is no cycle, & its just input of circle
cent & rad? Remember I have a vintage 1996 - 426.
Hey that sounds like an old Hemi moter only 66-426?<g>

Thanks for your help.

--

Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterday's technology
building
Tomorrows Dreams!
cncmillgil
2009-09-09 23:30:44 UTC
Permalink
Raw Message
Post by Jerry
Hi cncmillgil.
It is so easy to mill a circle like you describing there is no sense to use
a cycle.
All you do is to go to center of your pocket and down in Z and
CC IX0 IY0
LP PR 2.5 PA 0 RL F
ICP +360 DR+
Done.
If you want to do this on 426 with a cycle you can lie to the control and
add an even round number to you comp and the same to rad of your circle.
This way cutter will go straight to the edge of your circle.
We have Butlers, Correas and DMG with this control in our shop and if you
programming on the machine and you are good you can program it faster than
any other control I have ever seen.
Jerry
Post by Jerry
Every time you define a cycle like drilling or taping it takes precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say depth all you
have to do is describe new Q value.
For example you drill hole 1" deep (Q201=-0.055 ;DEPTH) before next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5" deep.
Same with any other Q value in cycles. You could make a say LBL 10 with
any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I did with
your program below.
All your positioning is in a label and is called up with every tool. Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Thanks for your posts. Norman at Bostomatic, too.
Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.
Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?
And just in case you have concerns about running Internet servers out
of drive space ..... I didn't want to edit the program for length lest
I delete something which might lead to confusion.
Thanks guys for the posts on Heidi's cycles.
Looks like the 530 control has a lot more cycles than than the ol 426
I'm on.
Billynevada: What CAM system outputs Heidi format? I was thinking only
ISO?
Also guys, what machine tools is the control on?
Last Fri, I had a 24"sqr electrical cabinet the service guys wanted a
"nice" 5" hole thru. What a fascicle. Setup top of the 2 kurts clapmed
to wood.
There was about 3/16-1/4" clearance to get the tool over & in. I
thought I had more, but turns out the last little bit, maybe 1/2" of Z
travel close to the upper limit switch is not usable during cycle.
Only took an hour or so to figure that out. So after machine
alignment, Z backs off the upper switch, so that position is max Z.
What's the cycle to just plunge & mill a circle- letting letting the
slug fall? I only found pocketing(taking the middle out), but thats
not what I wanted. Maybe there is no cycle, & its just input of circle
cent & rad? Remember I have a vintage 1996 - 426.
Hey that sounds like an old Hemi moter only 66-426?<g>
Thanks for your help.
--
        Gil©
      Member of
 ==American Toolmakers==
 using the "old world" ways
with yesterday's technology
       building
    Tomorrows Dreams!
I'm beginning to understand the format of Heide's language, finally!
Got a lot of cycles down now,labels/repeats ect. Complex print
geometry can be done with very little calulations. Heck, I'm a Hurco
head, so for comparison, take away Hurco's DXF & I think Heide may be
faster & smarter math wise.
So, my standing question: How do I circular interpolate in Y-Z or X-Z?
Being an ol ISO g-coder, Its G18/19 plane select, then I/J/K circ-cen.
G2/G3- G91 increm. over- ect.
How does that translate to Heide? Say I want to sweep a convex 1"R.
across a 5"?(x or y) block using a 1/4"ball EM, taking .025" step
overs?
Sweeping simple 2.5D contours across blocks is a lot of what my place
does.
It aint rocket science, I was doing work like this back in '80, hand
coding & manualy punching mylar tape, splicing the ends together to
make a continuese running loop tape, by switching on block-delete /
after prog is started, operator stops it after it runs off the block
or before it cuts into the table.<g>

Thanks Again.
--
___ ___
/ \ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------------ \ \/\/
\ _\/ \__\/
Gil©
Jerry
2009-09-10 00:29:47 UTC
Permalink
Raw Message
In one of my replays above I showed you how to put a rod on an edge. That
sample is for a 0.5" rad but the principle is the same. There arte a lot of
ways to do it but those are the two simplest.

0 BEGIN PGM rad1 INCH
1 BLK FORM 0.1 Z X+0 Y+0 Z-2
2 BLK FORM 0.2 X+3 Y+3 Z+0
3 TOOL CALL 18 Z S5000
4 * - 0.25" ballnose
5 * - 0.5" rad
6 * - machining along X axis
7 CYCL DEF 247 DATUM SETTING ~
Q339=+0 ;DATUM NUMBER
8 L X-0.2 Y-0.125 R0 FMAX M3
9 L Z+0 R0 FMAX M8
10 CC Y+0.5 Z-0.625
11 L Z-0.625 R0 F500
12 LBL 1
13 LP IPA-5 R0
14 L X+3.2
15 LP IPA-5
16 L X-0.2
17 LBL 0
18 CALL LBL 1 REP8
19 L Z+6 R0 FMAX M9 M5
20 L Z-0.1 Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad1 INCH


0 BEGIN PGM rad2 INCH
1 BLK FORM 0.1 Z X+0 Y+0 Z-2
2 BLK FORM 0.2 X+3 Y+3 Z+0
3 TOOL CALL 18 Z S5000
4 * - 0.25" ballnose
5 * - 0.5" rad
6 * - machining along radius
7 CYCL DEF 247 DATUM SETTING ~
Q339=+0 ;DATUM NUMBER
8 L X-0.2 Y-0.125 R0 FMAX M3
9 L Z+0 R0 FMAX M8
10 CC Y+0.5 Z-0.625
11 L Z-0.625 R0 F500
12 LBL 1
13 L IX+0.01
14 CP IPA-90 DR-
15 L IX+0.01
16 CP IPA+90 DR+
17 LBL 0
18 CALL LBL 1 REP160
19 L Z+6 R0 FMAX M9 M5
20 L Z-0.1 Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad2 INCH

erry
Post by Jerry
Hi cncmillgil.
It is so easy to mill a circle like you describing there is no sense to use
a cycle.
All you do is to go to center of your pocket and down in Z and
CC IX0 IY0
LP PR 2.5 PA 0 RL F
ICP +360 DR+
Done.
If you want to do this on 426 with a cycle you can lie to the control and
add an even round number to you comp and the same to rad of your circle.
This way cutter will go straight to the edge of your circle.
We have Butlers, Correas and DMG with this control in our shop and if you
programming on the machine and you are good you can program it faster than
any other control I have ever seen.
Jerry
Post by Jerry
Every time you define a cycle like drilling or taping it takes precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say depth all you
have to do is describe new Q value.
For example you drill hole 1" deep (Q201=-0.055 ;DEPTH) before next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5" deep.
Same with any other Q value in cycles. You could make a say LBL 10 with
any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I did with
your program below.
All your positioning is in a label and is called up with every tool. Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Thanks for your posts. Norman at Bostomatic, too.
Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.
Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?
And just in case you have concerns about running Internet servers out
of drive space ..... I didn't want to edit the program for length lest
I delete something which might lead to confusion.
Thanks guys for the posts on Heidi's cycles.
Looks like the 530 control has a lot more cycles than than the ol 426
I'm on.
Billynevada: What CAM system outputs Heidi format? I was thinking only
ISO?
Also guys, what machine tools is the control on?
Last Fri, I had a 24"sqr electrical cabinet the service guys wanted a
"nice" 5" hole thru. What a fascicle. Setup top of the 2 kurts clapmed
to wood.
There was about 3/16-1/4" clearance to get the tool over & in. I
thought I had more, but turns out the last little bit, maybe 1/2" of Z
travel close to the upper limit switch is not usable during cycle.
Only took an hour or so to figure that out. So after machine
alignment, Z backs off the upper switch, so that position is max Z.
What's the cycle to just plunge & mill a circle- letting letting the
slug fall? I only found pocketing(taking the middle out), but thats
not what I wanted. Maybe there is no cycle, & its just input of circle
cent & rad? Remember I have a vintage 1996 - 426.
Hey that sounds like an old Hemi moter only 66-426?<g>
Thanks for your help.
--
Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterday's technology
building
Tomorrows Dreams!
I'm beginning to understand the format of Heide's language, finally!
Got a lot of cycles down now,labels/repeats ect. Complex print
geometry can be done with very little calulations. Heck, I'm a Hurco
head, so for comparison, take away Hurco's DXF & I think Heide may be
faster & smarter math wise.
So, my standing question: How do I circular interpolate in Y-Z or X-Z?
Being an ol ISO g-coder, Its G18/19 plane select, then I/J/K circ-cen.
G2/G3- G91 increm. over- ect.
How does that translate to Heide? Say I want to sweep a convex 1"R.
across a 5"?(x or y) block using a 1/4"ball EM, taking .025" step
overs?
Sweeping simple 2.5D contours across blocks is a lot of what my place
does.
It aint rocket science, I was doing work like this back in '80, hand
coding & manualy punching mylar tape, splicing the ends together to
make a continuese running loop tape, by switching on block-delete /
after prog is started, operator stops it after it runs off the block
or before it cuts into the table.<g>

Thanks Again.
--
___ ___
/ \ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------------ \ \/\/
\ _\/ \__\/
Gil©
cncmillgil
2009-09-10 01:55:14 UTC
Permalink
Raw Message
Post by Jerry
In one of my replays above I showed you how to put a rod on an edge. That
sample is for a 0.5" rad but the principle is the same. There arte a lot of
ways to do it but those are the two simplest.
0  BEGIN PGM rad1 INCH
1  BLK FORM 0.1 Z  X+0  Y+0  Z-2
2  BLK FORM 0.2  X+3  Y+3  Z+0
3  TOOL CALL 18 Z S5000
4  * - 0.25" ballnose
5  * - 0.5" rad
6  * - machining along X axis
7  CYCL DEF 247 DATUM SETTING ~
    Q339=+0    ;DATUM NUMBER
8  L  X-0.2  Y-0.125 R0 FMAX M3
9  L  Z+0 R0 FMAX M8
10 CC  Y+0.5  Z-0.625
11 L  Z-0.625 R0 F500
12 LBL 1
13 LP IPA-5 R0
14 L  X+3.2
15 LP IPA-5
16 L  X-0.2
17 LBL 0
18 CALL LBL 1 REP8
19 L  Z+6 R0 FMAX M9 M5
20 L  Z-0.1  Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad1 INCH
0  BEGIN PGM rad2 INCH
1  BLK FORM 0.1 Z  X+0  Y+0  Z-2
2  BLK FORM 0.2  X+3  Y+3  Z+0
3  TOOL CALL 18 Z S5000
4  * - 0.25" ballnose
5  * - 0.5" rad
6  * - machining along radius
7  CYCL DEF 247 DATUM SETTING ~
    Q339=+0    ;DATUM NUMBER
8  L  X-0.2  Y-0.125 R0 FMAX M3
9  L  Z+0 R0 FMAX M8
10 CC  Y+0.5  Z-0.625
11 L  Z-0.625 R0 F500
12 LBL 1
13 L IX+0.01
14 CP IPA-90 DR-
15 L IX+0.01
16 CP IPA+90 DR+
17 LBL 0
18 CALL LBL 1 REP160
19 L  Z+6 R0 FMAX M9 M5
20 L  Z-0.1  Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad2 INCH
erry
Post by Jerry
Hi cncmillgil.
It is so easy to mill a circle like you describing there is no sense to use
a cycle.
All you do is to go to center of your pocket and down in Z and
CC IX0 IY0
LP PR 2.5 PA 0 RL F
ICP +360 DR+
Done.
If you want to do this on 426 with a cycle you can lie to the control and
add an even round number to you comp and the same to rad of your circle.
This way cutter will go straight to the edge of your circle.
We have Butlers, Correas and DMG with this control in our shop and if you
programming on the machine and you are good you can program it faster than
any other control I have ever seen.
Jerry
Post by Jerry
Every time you define a cycle like drilling or taping it takes precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say depth all you
have to do is describe new Q value.
For example you drill hole 1" deep (Q201=-0.055 ;DEPTH) before next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5" deep.
Same with any other Q value in cycles. You could make a say LBL 10 with
any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I did with
your program below.
All your positioning is in a label and is called up with every tool. Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Thanks for your posts. Norman at Bostomatic, too.
Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.
Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?
And just in case you have concerns about running Internet servers out
of drive space ..... I didn't want to edit the program for length lest
I delete something which might lead to confusion.
Thanks guys for the posts on Heidi's cycles.
Looks like the 530 control has a lot more cycles than than the ol 426
I'm on.
Billynevada: What CAM system outputs Heidi format? I was thinking only
ISO?
Also guys, what machine tools is the control on?
Last Fri, I had a 24"sqr electrical cabinet the service guys wanted a
"nice" 5" hole thru. What a fascicle. Setup top of the 2 kurts clapmed
to wood.
There was about 3/16-1/4" clearance to get the tool over & in. I
thought I had more, but turns out the last little bit, maybe 1/2" of Z
travel close to the upper limit switch is not usable during cycle.
Only took an hour or so to figure that out. So after machine
alignment, Z backs off the upper switch, so that position is max Z.
What's the cycle to just plunge & mill a circle- letting letting the
slug fall? I only found pocketing(taking the middle out), but thats
not what I wanted. Maybe there is no cycle, & its just input of circle
cent & rad? Remember I have a vintage 1996 - 426.
Hey that sounds like an old Hemi moter only
...
read more »
Looks all "greek" to me:-) I will give these a try tomorrow during a
long run on slots.

Thanks
--
___ ___
/ \ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------------ \ \/\/
\ _\/ \__\/
Gil©
cncmillgil
2009-09-23 10:58:42 UTC
Permalink
Raw Message
Post by Jerry
Post by Jerry
In one of my replays above I showed you how to put a rod on an edge. That
sample is for a 0.5" rad but the principle is the same. There arte a lot of
ways to do it but those are the two simplest.
0  BEGIN PGM rad1 INCH
1  BLK FORM 0.1 Z  X+0  Y+0  Z-2
2  BLK FORM 0.2  X+3  Y+3  Z+0
3  TOOL CALL 18 Z S5000
4  * - 0.25" ballnose
5  * - 0.5" rad
6  * - machining along X axis
7  CYCL DEF 247 DATUM SETTING ~
    Q339=+0    ;DATUM NUMBER
8  L  X-0.2  Y-0.125 R0 FMAX M3
9  L  Z+0 R0 FMAX M8
10 CC  Y+0.5  Z-0.625
11 L  Z-0.625 R0 F500
12 LBL 1
13 LP IPA-5 R0
14 L  X+3.2
15 LP IPA-5
16 L  X-0.2
17 LBL 0
18 CALL LBL 1 REP8
19 L  Z+6 R0 FMAX M9 M5
20 L  Z-0.1  Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad1 INCH
0  BEGIN PGM rad2 INCH
1  BLK FORM 0.1 Z  X+0  Y+0  Z-2
2  BLK FORM 0.2  X+3  Y+3  Z+0
3  TOOL CALL 18 Z S5000
4  * - 0.25" ballnose
5  * - 0.5" rad
6  * - machining along radius
7  CYCL DEF 247 DATUM SETTING ~
    Q339=+0    ;DATUM NUMBER
8  L  X-0.2  Y-0.125 R0 FMAX M3
9  L  Z+0 R0 FMAX M8
10 CC  Y+0.5  Z-0.625
11 L  Z-0.625 R0 F500
12 LBL 1
13 L IX+0.01
14 CP IPA-90 DR-
15 L IX+0.01
16 CP IPA+90 DR+
17 LBL 0
18 CALL LBL 1 REP160
19 L  Z+6 R0 FMAX M9 M5
20 L  Z-0.1  Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad2 INCH
erry
Post by Jerry
Hi cncmillgil.
It is so easy to mill a circle like you describing there is no sense to use
a cycle.
All you do is to go to center of your pocket and down in Z and
CC IX0 IY0
LP PR 2.5 PA 0 RL F
ICP +360 DR+
Done.
If you want to do this on 426 with a cycle you can lie to the control and
add an even round number to you comp and the same to rad of your circle.
This way cutter will go straight to the edge of your circle.
We have Butlers, Correas and DMG with this control in our shop and if you
programming on the machine and you are good you can program it faster than
any other control I have ever seen.
Jerry
Post by Jerry
Every time you define a cycle like drilling or taping it takes precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say depth all you
have to do is describe new Q value.
For example you drill hole 1" deep (Q201=-0.055 ;DEPTH) before next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5" deep.
Same with any other Q value in cycles. You could make a say LBL 10 with
any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I did with
your program below.
All your positioning is in a label and is called up with every tool. Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Thanks for your posts. Norman at Bostomatic, too.
Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.
Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?
And just in case you have concerns about running Internet servers out
of drive space ..... I didn't want to edit the program for length lest
I delete something which might lead to confusion.
Thanks guys for the posts on Heidi's cycles.
Looks like the 530 control has a lot more cycles than than the ol 426
I'm on.
Billynevada: What CAM system outputs Heidi format? I was thinking only
ISO?
Also guys, what machine tools is the control on?
Last Fri, I had a 24"sqr electrical cabinet the service guys wanted a
"nice" 5" hole thru. What a fascicle. Setup top of the 2 kurts clapmed
to wood.
...
read more »
Help Mr. Wizzard Help!
This F'in Ol Basdard 426 will be my bitch some day.........
Ain no damn CNC freekin control gonna intimadate me<g>
I'm good at fegger'in out stuff ya no..........:-)
Like back in 95, A Mitsubishi v55 with the M2a control. that was
another sleeping giant. Slow as a turtle but a great moldbase
machine.

Loading Image...


--

___ ___
/ /\ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------- \ \/\/
\__\/ \__\/


Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterdays technology
building
Tomorrows Dreams
cncmillgil
2009-09-25 11:25:41 UTC
Permalink
Raw Message
Post by Jerry
Post by Jerry
In one of my replays above I showed you how to put a rod on an edge. That
sample is for a 0.5" rad but the principle is the same. There arte a lot of
ways to do it but those are the two simplest.
0  BEGIN PGM rad1 INCH
1  BLK FORM 0.1 Z  X+0  Y+0  Z-2
2  BLK FORM 0.2  X+3  Y+3  Z+0
3  TOOL CALL 18 Z S5000
4  * - 0.25" ballnose
5  * - 0.5" rad
6  * - machining along X axis
7  CYCL DEF 247 DATUM SETTING ~
    Q339=+0    ;DATUM NUMBER
8  L  X-0.2  Y-0.125 R0 FMAX M3
9  L  Z+0 R0 FMAX M8
10 CC  Y+0.5  Z-0.625
11 L  Z-0.625 R0 F500
12 LBL 1
13 LP IPA-5 R0
14 L  X+3.2
15 LP IPA-5
16 L  X-0.2
17 LBL 0
18 CALL LBL 1 REP8
19 L  Z+6 R0 FMAX M9 M5
20 L  Z-0.1  Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad1 INCH
0  BEGIN PGM rad2 INCH
1  BLK FORM 0.1 Z  X+0  Y+0  Z-2
2  BLK FORM 0.2  X+3  Y+3  Z+0
3  TOOL CALL 18 Z S5000
4  * - 0.25" ballnose
5  * - 0.5" rad
6  * - machining along radius
7  CYCL DEF 247 DATUM SETTING ~
    Q339=+0    ;DATUM NUMBER
8  L  X-0.2  Y-0.125 R0 FMAX M3
9  L  Z+0 R0 FMAX M8
10 CC  Y+0.5  Z-0.625
11 L  Z-0.625 R0 F500
12 LBL 1
13 L IX+0.01
14 CP IPA-90 DR-
15 L IX+0.01
16 CP IPA+90 DR+
17 LBL 0
18 CALL LBL 1 REP160
19 L  Z+6 R0 FMAX M9 M5
20 L  Z-0.1  Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad2 INCH
erry
Post by Jerry
Hi cncmillgil.
It is so easy to mill a circle like you describing there is no sense to use
a cycle.
All you do is to go to center of your pocket and down in Z and
CC IX0 IY0
LP PR 2.5 PA 0 RL F
ICP +360 DR+
Done.
If you want to do this on 426 with a cycle you can lie to the control and
add an even round number to you comp and the same to rad of your circle.
This way cutter will go straight to the edge of your circle.
We have Butlers, Correas and DMG with this control in our shop and if you
programming on the machine and you are good you can program it faster than
any other control I have ever seen.
Jerry
Post by Jerry
Every time you define a cycle like drilling or taping it takes precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say depth all you
have to do is describe new Q value.
For example you drill hole 1" deep (Q201=-0.055 ;DEPTH) before next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5"
deep.
Same with any other Q value in cycles. You could make a say LBL 10 with
any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I did with
your program below.
All your positioning is in a label and is called up with every tool. Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Thanks for your posts. Norman at Bostomatic, too.
Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.
Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?
And just in case you have concerns about running Internet
...
read more »
Ok overall consensise so far, about 25-50hrs actual machine time over
the last 9mo.
Heidenhain 426 conversational input on Anayak VH1800.
Its a bitch<g>
The thinking mentality , logic, behind the the predefined cycles are
different than today. Gotta remember they did not have & readily
avalaible, good CAM systems to get data feed to the machine & get'r
running. Besides Mastercam/Smartcam/Sufcam early 90 ish. High end
systems McD/Slumberje?/CV/Camax/IT/ were the few REAL cam systems out
there, and were few & far between.
So take a shop floor guy & give'em a way to get basic geometry off
basic prints in to the machine, let the control do all the hard trig
math, with a few "rules" for those cycles & wala! Yer cut'in 3D shit
with cycle looping /inrementaly progressing & multi passing milling
controled by number of repeats stuff. Plus while the machine is
running, next up programs can be witten/ screen tested(backploted),pre
difined work offsets calculated(programing in background). & it has
its own user defined macro input called "Q" programs for "family of
parts" type work. . Make a d
It's input & editing key functions & terminolgy are kinda funky as
comparied to US? IE: no entry=clear entry - NC start=Cycle Start
NC stop=interrupt cycle/feed hold. It's ok, but just makes you think
for a second. The reasoning is, that control was put on all kinds of
machines, prolly robots & other cnc controled equipt. So across the
board terminolgy is used.
Its just another Freekin machine tool. Another notch in the belt.
Gonna need a bigger belt here soon.
As I said before, I will own you bitch! You are a piece of ancient
shit.
But you still work, so this crazy ol moldmaker is gonna have some fun
with you, with your big ass 50taper (no tool changer) 30hp gear drive
dick head shaped head.<g>
This machine tool is what happens when German engineering & Spanish
engineering get together. WTH? were they thinking?
Freekin goof balls. Such a big ass machine but not enough rigidity to
hold large face mills from deflection - noticed on mainly exit off of
part.
Just slightly, again noticalble by cutter marks (trailing & leading
edge) & size measurement. +-.001 over 4"dia face mill. Not so much
head out of sqr as seen from stepover, but deflection in direction of
travel. Its gotta be not enough strength by desgin of the physical
head shape. It looks like a swivel dick sticking out of the Y carrage.
This compact swiveling head design was intended for a purpose.? Maybe
tall cores/ castings with small corner radii? Thus the head could be
swiveled to gain access way down vertical walls? Its big enough &
strong enough to preform very well at jobs like that. Kinda reminds me
of giant version of the old Bridgeport "Quilmaster" head. With a huge
X(70") Y Z travels open bed, full front loading - door access. You
just don't see the likes of one of these too often. I dont think this
beast has ever been fully tammed. This shop has been "captive" so
production output was not much?
Any hoot, its a play thing for me, as I feel semi-retired at 52. I
just do this shit so I dont get bored, as can be clearly seen here, by
me wasting my time here<g>

Ya Ya you know, Its German..........the BEST! oh sorry Swiss,&
Norwegian guys.

--

___ ___
/ /\ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------- \ \/\/
\__\/ \__\/


Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterdays technology
building
Tomorrows Dreams
Jerry
2009-09-25 16:38:05 UTC
Permalink
Raw Message
cncmillgil.
I have a feeling you do not like this control to much.
All my experience on Heidenhain in all those years was positive and I think
if I had a choice I would never
work on any other control.
It is just different to you and it will take some time to adjust.
If you have any specific questions you can send me an email or just post
here but I usually don't go back
in posts so far so you may want to start a new thread. I will try to help
you out and you will see you will learn to like Heindenhain.
Jerry
Post by Jerry
Post by Jerry
In one of my replays above I showed you how to put a rod on an edge. That
sample is for a 0.5" rad but the principle is the same. There arte a lot of
ways to do it but those are the two simplest.
0 BEGIN PGM rad1 INCH
1 BLK FORM 0.1 Z X+0 Y+0 Z-2
2 BLK FORM 0.2 X+3 Y+3 Z+0
3 TOOL CALL 18 Z S5000
4 * - 0.25" ballnose
5 * - 0.5" rad
6 * - machining along X axis
7 CYCL DEF 247 DATUM SETTING ~
Q339=+0 ;DATUM NUMBER
8 L X-0.2 Y-0.125 R0 FMAX M3
9 L Z+0 R0 FMAX M8
10 CC Y+0.5 Z-0.625
11 L Z-0.625 R0 F500
12 LBL 1
13 LP IPA-5 R0
14 L X+3.2
15 LP IPA-5
16 L X-0.2
17 LBL 0
18 CALL LBL 1 REP8
19 L Z+6 R0 FMAX M9 M5
20 L Z-0.1 Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad1 INCH
0 BEGIN PGM rad2 INCH
1 BLK FORM 0.1 Z X+0 Y+0 Z-2
2 BLK FORM 0.2 X+3 Y+3 Z+0
3 TOOL CALL 18 Z S5000
4 * - 0.25" ballnose
5 * - 0.5" rad
6 * - machining along radius
7 CYCL DEF 247 DATUM SETTING ~
Q339=+0 ;DATUM NUMBER
8 L X-0.2 Y-0.125 R0 FMAX M3
9 L Z+0 R0 FMAX M8
10 CC Y+0.5 Z-0.625
11 L Z-0.625 R0 F500
12 LBL 1
13 L IX+0.01
14 CP IPA-90 DR-
15 L IX+0.01
16 CP IPA+90 DR+
17 LBL 0
18 CALL LBL 1 REP160
19 L Z+6 R0 FMAX M9 M5
20 L Z-0.1 Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad2 INCH
erry
Post by Jerry
Hi cncmillgil.
It is so easy to mill a circle like you describing there is no sense
to
use
a cycle.
All you do is to go to center of your pocket and down in Z and
CC IX0 IY0
LP PR 2.5 PA 0 RL F
ICP +360 DR+
Done.
If you want to do this on 426 with a cycle you can lie to the control and
add an even round number to you comp and the same to rad of your circle.
This way cutter will go straight to the edge of your circle.
We have Butlers, Correas and DMG with this control in our shop and if you
programming on the machine and you are good you can program it faster than
any other control I have ever seen.
Jerry
Post by Jerry
Every time you define a cycle like drilling or taping it takes precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say
depth all
you
have to do is describe new Q value.
For example you drill hole 1" deep (Q201=-0.055 ;DEPTH) before next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5"
deep.
Same with any other Q value in cycles. You could make a say LBL 10 with
any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I did with
your program below.
All your positioning is in a label and is called up with every
tool.
Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Thanks for your posts. Norman at Bostomatic, too.
Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.
Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?
And just in case you have concerns about running Internet
...
read more »
Ok overall consensise so far, about 25-50hrs actual machine time over
the last 9mo.
Heidenhain 426 conversational input on Anayak VH1800.
Its a bitch<g>
The thinking mentality , logic, behind the the predefined cycles are
different than today. Gotta remember they did not have & readily
avalaible, good CAM systems to get data feed to the machine & get'r
running. Besides Mastercam/Smartcam/Sufcam early 90 ish. High end
systems McD/Slumberje?/CV/Camax/IT/ were the few REAL cam systems out
there, and were few & far between.
So take a shop floor guy & give'em a way to get basic geometry off
basic prints in to the machine, let the control do all the hard trig
math, with a few "rules" for those cycles & wala! Yer cut'in 3D shit
with cycle looping /inrementaly progressing & multi passing milling
controled by number of repeats stuff. Plus while the machine is
running, next up programs can be witten/ screen tested(backploted),pre
difined work offsets calculated(programing in background). & it has
its own user defined macro input called "Q" programs for "family of
parts" type work. . Make a d
It's input & editing key functions & terminolgy are kinda funky as
comparied to US? IE: no entry=clear entry - NC start=Cycle Start
NC stop=interrupt cycle/feed hold. It's ok, but just makes you think
for a second. The reasoning is, that control was put on all kinds of
machines, prolly robots & other cnc controled equipt. So across the
board terminolgy is used.
Its just another Freekin machine tool. Another notch in the belt.
Gonna need a bigger belt here soon.
As I said before, I will own you bitch! You are a piece of ancient
shit.
But you still work, so this crazy ol moldmaker is gonna have some fun
with you, with your big ass 50taper (no tool changer) 30hp gear drive
dick head shaped head.<g>
This machine tool is what happens when German engineering & Spanish
engineering get together. WTH? were they thinking?
Freekin goof balls. Such a big ass machine but not enough rigidity to
hold large face mills from deflection - noticed on mainly exit off of
part.
Just slightly, again noticalble by cutter marks (trailing & leading
edge) & size measurement. +-.001 over 4"dia face mill. Not so much
head out of sqr as seen from stepover, but deflection in direction of
travel. Its gotta be not enough strength by desgin of the physical
head shape. It looks like a swivel dick sticking out of the Y carrage.
This compact swiveling head design was intended for a purpose.? Maybe
tall cores/ castings with small corner radii? Thus the head could be
swiveled to gain access way down vertical walls? Its big enough &
strong enough to preform very well at jobs like that. Kinda reminds me
of giant version of the old Bridgeport "Quilmaster" head. With a huge
X(70") Y Z travels open bed, full front loading - door access. You
just don't see the likes of one of these too often. I dont think this
beast has ever been fully tammed. This shop has been "captive" so
production output was not much?
Any hoot, its a play thing for me, as I feel semi-retired at 52. I
just do this shit so I dont get bored, as can be clearly seen here, by
me wasting my time here<g>

Ya Ya you know, Its German..........the BEST! oh sorry Swiss,&
Norwegian guys.

--

___ ___
/ /\ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------- \ \/\/
\__\/ \__\/


Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterdays technology
building
Tomorrows Dreams
Jerry
2009-09-25 16:39:07 UTC
Permalink
Raw Message
BTW.
Did you try to run any of the programs I posted for you?
Jerry
Post by Jerry
cncmillgil.
I have a feeling you do not like this control to much.
All my experience on Heidenhain in all those years was positive and I
think if I had a choice I would never
work on any other control.
It is just different to you and it will take some time to adjust.
If you have any specific questions you can send me an email or just post
here but I usually don't go back
in posts so far so you may want to start a new thread. I will try to help
you out and you will see you will learn to like Heindenhain.
Jerry
Post by Jerry
Post by Jerry
In one of my replays above I showed you how to put a rod on an edge. That
sample is for a 0.5" rad but the principle is the same. There arte a lot of
ways to do it but those are the two simplest.
0 BEGIN PGM rad1 INCH
1 BLK FORM 0.1 Z X+0 Y+0 Z-2
2 BLK FORM 0.2 X+3 Y+3 Z+0
3 TOOL CALL 18 Z S5000
4 * - 0.25" ballnose
5 * - 0.5" rad
6 * - machining along X axis
7 CYCL DEF 247 DATUM SETTING ~
Q339=+0 ;DATUM NUMBER
8 L X-0.2 Y-0.125 R0 FMAX M3
9 L Z+0 R0 FMAX M8
10 CC Y+0.5 Z-0.625
11 L Z-0.625 R0 F500
12 LBL 1
13 LP IPA-5 R0
14 L X+3.2
15 LP IPA-5
16 L X-0.2
17 LBL 0
18 CALL LBL 1 REP8
19 L Z+6 R0 FMAX M9 M5
20 L Z-0.1 Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad1 INCH
0 BEGIN PGM rad2 INCH
1 BLK FORM 0.1 Z X+0 Y+0 Z-2
2 BLK FORM 0.2 X+3 Y+3 Z+0
3 TOOL CALL 18 Z S5000
4 * - 0.25" ballnose
5 * - 0.5" rad
6 * - machining along radius
7 CYCL DEF 247 DATUM SETTING ~
Q339=+0 ;DATUM NUMBER
8 L X-0.2 Y-0.125 R0 FMAX M3
9 L Z+0 R0 FMAX M8
10 CC Y+0.5 Z-0.625
11 L Z-0.625 R0 F500
12 LBL 1
13 L IX+0.01
14 CP IPA-90 DR-
15 L IX+0.01
16 CP IPA+90 DR+
17 LBL 0
18 CALL LBL 1 REP160
19 L Z+6 R0 FMAX M9 M5
20 L Z-0.1 Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad2 INCH
erry
Post by Jerry
Hi cncmillgil.
It is so easy to mill a circle like you describing there is no
sense to
use
a cycle.
All you do is to go to center of your pocket and down in Z and
CC IX0 IY0
LP PR 2.5 PA 0 RL F
ICP +360 DR+
Done.
If you want to do this on 426 with a cycle you can lie to the control and
add an even round number to you comp and the same to rad of your circle.
This way cutter will go straight to the edge of your circle.
We have Butlers, Correas and DMG with this control in our shop and if you
programming on the machine and you are good you can program it faster than
any other control I have ever seen.
Jerry
Post by Jerry
Every time you define a cycle like drilling or taping it takes precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say
depth all
you
have to do is describe new Q value.
For example you drill hole 1" deep (Q201=-0.055 ;DEPTH) before next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5"
deep.
Same with any other Q value in cycles. You could make a say LBL 10 with
any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I did with
your program below.
All your positioning is in a label and is called up with every
tool.
Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
Thanks for your posts. Norman at Bostomatic, too.
Here is a spot/drill/ rigid peck tap I got out of our CAM after some
post tweaks.
I am not versed in any Heidenhain programming so the structure may be
off. Comments welcomed. But the trick was to get the post to issue
hole locations after the cycle is defined. Then called with an M99 or
a Location <eob> CYCLE CALL couplet.
Can the cycles all be defined then called later on in the program or
must it be cycle/motion cycle/motion ?
And just in case you have concerns about running Internet
...
read more »
Ok overall consensise so far, about 25-50hrs actual machine time over
the last 9mo.
Heidenhain 426 conversational input on Anayak VH1800.
Its a bitch<g>
The thinking mentality , logic, behind the the predefined cycles are
different than today. Gotta remember they did not have & readily
avalaible, good CAM systems to get data feed to the machine & get'r
running. Besides Mastercam/Smartcam/Sufcam early 90 ish. High end
systems McD/Slumberje?/CV/Camax/IT/ were the few REAL cam systems out
there, and were few & far between.
So take a shop floor guy & give'em a way to get basic geometry off
basic prints in to the machine, let the control do all the hard trig
math, with a few "rules" for those cycles & wala! Yer cut'in 3D shit
with cycle looping /inrementaly progressing & multi passing milling
controled by number of repeats stuff. Plus while the machine is
running, next up programs can be witten/ screen tested(backploted),pre
difined work offsets calculated(programing in background). & it has
its own user defined macro input called "Q" programs for "family of
parts" type work. . Make a d
It's input & editing key functions & terminolgy are kinda funky as
comparied to US? IE: no entry=clear entry - NC start=Cycle Start
NC stop=interrupt cycle/feed hold. It's ok, but just makes you think
for a second. The reasoning is, that control was put on all kinds of
machines, prolly robots & other cnc controled equipt. So across the
board terminolgy is used.
Its just another Freekin machine tool. Another notch in the belt.
Gonna need a bigger belt here soon.
As I said before, I will own you bitch! You are a piece of ancient
shit.
But you still work, so this crazy ol moldmaker is gonna have some fun
with you, with your big ass 50taper (no tool changer) 30hp gear drive
dick head shaped head.<g>
This machine tool is what happens when German engineering & Spanish
engineering get together. WTH? were they thinking?
Freekin goof balls. Such a big ass machine but not enough rigidity to
hold large face mills from deflection - noticed on mainly exit off of
part.
Just slightly, again noticalble by cutter marks (trailing & leading
edge) & size measurement. +-.001 over 4"dia face mill. Not so much
head out of sqr as seen from stepover, but deflection in direction of
travel. Its gotta be not enough strength by desgin of the physical
head shape. It looks like a swivel dick sticking out of the Y carrage.
This compact swiveling head design was intended for a purpose.? Maybe
tall cores/ castings with small corner radii? Thus the head could be
swiveled to gain access way down vertical walls? Its big enough &
strong enough to preform very well at jobs like that. Kinda reminds me
of giant version of the old Bridgeport "Quilmaster" head. With a huge
X(70") Y Z travels open bed, full front loading - door access. You
just don't see the likes of one of these too often. I dont think this
beast has ever been fully tammed. This shop has been "captive" so
production output was not much?
Any hoot, its a play thing for me, as I feel semi-retired at 52. I
just do this shit so I dont get bored, as can be clearly seen here, by
me wasting my time here<g>
Ya Ya you know, Its German..........the BEST! oh sorry Swiss,&
Norwegian guys.
--
___ ___
/ /\ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------- \ \/\/
\__\/ \__\/
Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterdays technology
building
Tomorrows Dreams
cncmillgil
2009-09-26 08:13:55 UTC
Permalink
Raw Message
Post by Jerry
cncmillgil.
I have a feeling you do not like this control to much.
All my experience on Heidenhain in all those years was positive and I think
if I had a choice I would never
work on any other control.
It is just different to you and it will take some time to adjust.
If you have any specific questions you can send me an email or just post
here but I usually don't go back
in posts so far so you may want to start a new thread. I will try to help
you out and you will see you will learn to like Heindenhain.
Jerry
Post by Jerry
In one of my replays above I showed you how to put a rod on an edge. That
sample is for a 0.5" rad but the principle is the same. There arte a lot of
ways to do it but those are the two simplest.
0 BEGIN PGM rad1 INCH
1 BLK FORM 0.1 Z X+0 Y+0 Z-2
2 BLK FORM 0.2 X+3 Y+3 Z+0
3 TOOL CALL 18 Z S5000
4 * - 0.25" ballnose
5 * - 0.5" rad
6 * - machining along X axis
7 CYCL DEF 247 DATUM SETTING ~
Q339=+0 ;DATUM NUMBER
8 L X-0.2 Y-0.125 R0 FMAX M3
9 L Z+0 R0 FMAX M8
10 CC Y+0.5 Z-0.625
11 L Z-0.625 R0 F500
12 LBL 1
13 LP IPA-5 R0
14 L X+3.2
15 LP IPA-5
16 L X-0.2
17 LBL 0
18 CALL LBL 1 REP8
19 L Z+6 R0 FMAX M9 M5
20 L Z-0.1 Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad1 INCH
0 BEGIN PGM rad2 INCH
1 BLK FORM 0.1 Z X+0 Y+0 Z-2
2 BLK FORM 0.2 X+3 Y+3 Z+0
3 TOOL CALL 18 Z S5000
4 * - 0.25" ballnose
5 * - 0.5" rad
6 * - machining along radius
7 CYCL DEF 247 DATUM SETTING ~
Q339=+0 ;DATUM NUMBER
8 L X-0.2 Y-0.125 R0 FMAX M3
9 L Z+0 R0 FMAX M8
10 CC Y+0.5 Z-0.625
11 L Z-0.625 R0 F500
12 LBL 1
13 L IX+0.01
14 CP IPA-90 DR-
15 L IX+0.01
16 CP IPA+90 DR+
17 LBL 0
18 CALL LBL 1 REP160
19 L Z+6 R0 FMAX M9 M5
20 L Z-0.1 Y-0.1 R0 FMAX M91
21 M30
22 END PGM rad2 INCH
erry
Post by Jerry
Hi cncmillgil.
It is so easy to mill a circle like you describing there is no sense
to
use
a cycle.
All you do is to go to center of your pocket and down in Z and
CC IX0 IY0
LP PR 2.5 PA 0 RL F
ICP +360 DR+
Done.
If you want to do this on 426 with a cycle you can lie to the control and
add an even round number to you comp and the same to rad of your circle.
This way cutter will go straight to the edge of your circle.
We have Butlers, Correas and DMG with this control in our shop and if you
programming on the machine and you are good you can program it faster than
any other control I have ever seen.
Jerry
Post by Jerry
Every time you define a cycle like drilling or taping it takes
precedence
over any pervious cycle.
If you are changing only one of the cycle parameters like say
depth all
you
have to do is describe new Q value.
For example you drill hole 1" deep (Q201=-0.055 ;DEPTH) before
next hole
you may describe Q201=-1.5 and next hole drilled with M99 will be 1.5"
deep.
Same with any other Q value in cycles. You could make a say LBL 10 with
any
cycle in it and call it up when needed.
If you want to make your program smaller you can edit it like I
did with
your program below.
All your positioning is in a label and is called up with every
tool.
Don't
worry about the block numbers. When you send it to your machine it will
rearrange it.
0 BEGIN PGM 1 INCH
; FROM BEGIN PGM joe
BLK FORM 0.1 Z X-1.0 Y-1.0 Z-1.1
BLK FORM 0.2 X+1.0 Y+1.0 Z+0.0110
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
10 CYCL DEF 7.0 DATUM SHIFT
20 CYCL DEF 7.1 X+0
30 CYCL DEF 7.2 Y+0
40 CYCL DEF 7.3 Z+0
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
50 TOOL CALL 10 Z S2000;
55 TOOL NUMBER - 10 DESCRIPTION - CDRILL TOOL LENGTH FROM HOLDER 2.000
100 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.055 ;DEPTH~
Q206=15 ;FEED RATE~
Q202=0.03 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
105 LBL 1
110 L X.3835 Y.1625 FMAX M3
120 CYCL CALL M8
130 L X1.0385 FMAX M99
140 L X1.6935 FMAX M99
150 L X2.3485 FMAX M99
160 L X3.0035 FMAX M99
170 L X3.6585 FMAX M99
180 L X4.3135 FMAX M99
190 L X4.9685 FMAX M99
200 L X4.3769 Y-.1625 FMAX M99
210 L X3.7219 FMAX M99
220 L X3.0669 FMAX M99
230 L X2.4119 FMAX M99
240 L X1.7569 FMAX M99
250 L X1.1019 FMAX M99
260 L X.4469 FMAX M99
270 L X-.2081 FMAX M99
280 L X.3835 Y-.3825 FMAX M99
290 L X1.0385 FMAX M99
300 L X1.6935 FMAX M99
310 L X2.3485 FMAX M99
320 L X3.0035 FMAX M99
330 L X3.6585 FMAX M99
340 L X4.3135 FMAX M99
350 L X4.9685 FMAX M99
360 L X4.3769 Y-.7075 FMAX M99
370 L X3.7219 FMAX M99
380 L X3.0669 FMAX M99
390 L X2.4119 FMAX M99
400 L X1.7569 FMAX M99
410 L X1.1019 FMAX M99
420 L X.4469 FMAX M99
430 L X-.2081 FMAX M99
440 L X.3835 Y-.9275 FMAX M99
450 L X1.0385 FMAX M99
460 L X1.6935 FMAX M99
470 L X2.3485 FMAX M99
480 L X3.0035 FMAX M99
490 L X3.6585 FMAX M99
500 L X4.3135 FMAX M99
510 L X4.9685 FMAX M99
520 L X4.3769 Y-1.2525 FMAX M99
530 L X3.7219 FMAX M99
540 L X3.0669 FMAX M99
550 L X2.4119 FMAX M99
560 L X1.7569 FMAX M99
570 L X1.1019 FMAX M99
580 L X.4469 FMAX M99
590 L X-.2081 FMAX M99
600 L X.3835 Y-1.4725 FMAX M99
610 L X1.0385 FMAX M99
620 L X1.6935 FMAX M99
630 L X2.3485 FMAX M99
640 L X3.0035 FMAX M99
650 L X3.6585 FMAX M99
660 L X4.3135 FMAX M99
670 L X4.9685 FMAX M99
680 L X4.3769 Y-1.7975 FMAX M99
690 L X3.7219 FMAX M99
700 L X3.0669 FMAX M99
710 L X2.4119 FMAX M99
720 L X1.7569 FMAX M99
730 L X1.1019 FMAX M99
740 L X.4469 FMAX M99
750 L X-.2081 FMAX M99
755 LBL 0
760 M9
770 M5
M140 MB MAX
780 M1 ; PROGRAM STOP
790 TOOL CALL 11 Z S2000
; TOOL NUMBER - 11 DESCRIPTION - .070DIA TOOL LENGTH FROM HOLDER 3.500
840 CYCL DEF 205 UNIVERSAL PECKING~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.28 ;DEPTH~
Q206=13 ;FEED RATE~
Q202=0.06 ;PLUNGE DEPTH~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q212=0. ;DECREMENT~
Q205=0.0 ;MIN. PLUNGE DEPTH~
Q258=0.02 ;UPPER ADV STOP DIST~
Q259=0.04 ;LOWER ADV STOP DIST~
Q257=0 ;DEPTH FOR CHIP BREAKING~
Q256=0.02 ;DIST. FOR CHIP BREAKING~
Q211=1.0 ;DWELL AT DEPTH~
Q379=0 ;RETRACT FEED RATE~
Q253=0 ;DIST. FOR CHIP BREAKING
1495 LBL CALL 1
1500 M9
1510 M5
M140 MB MAX
1520 M1 ; PROGRAM STOP
CYCL DEF 247 DATUM SETTING~
Q339=+1; WORK SHIFT NUMBER
1530 TOOL CALL 12 Z S600
; TOOL NUMBER - 12 DESCRIPTION - 2-56 TAP TOOL LENGTH FROM HOLDER 2.000
1590 CYCL DEF 209 TAPPING W/ CHIP BRKG ~
Q200=0.05 ;SET-UP CLEARANCE~
Q201=-0.265 ;DEPTH OF THREAD ~
Q239=0.0179 ;PITCH OF THREAD ~
Q203=0.0 ;SURFACE COORDINATE~
Q204=0.05 ;2ND SET-UP CLEARANCE~
Q257=0.085 ;DEPTH FOR CHIP BRKNG ~
Q256=0.02 ;DIST FOR CHIP BRKNG ~
Q336=0 ;ANGLE OF SPINDLE
1595 LBL CALL 1
2250 M9
2260 M5
M140 MB MAX
CYCL DEF 247 DATUM SETTING~
Q339=+49; UNLOAD PART WORK SHIFT NUMBER
L X0 Y0 FMAX
CYCL DEF 247 DATUM SETTING~
Q339=+1; RELOAD ASS-U-MED WORK SHIFT NUMBER
M30
END PGM 1 INCH
...
read more »
No no, I think Heide's control is very interesting! Its a different
way to program. Its,... special? Coming from the offline CNC prog.
path I've been down. I see that fan blade picture on the front of the
manuals & say" Hey, thats what I want to cut" <g> Ok show me.
This "Q" programming is in the back of my mind. Seems with that style,
one could do alot of work with very little input. Someone wrote a Q
program for a sloting opp we do. It works with a parameter file for
some variables. I'm sure you know of this, but for me its new.
I would like to write a Q program for our standard family of parts.
Same process/tools- different variables/dims.
IE: Input length,width,height,features - slap piece in vise & whahla
Yer cutt'in. That kind of work is alot of what the "hobby shop" I work
at does, or I should say should do.<g>
Can't beat that. Why use high end CAD/CAM when you dont need it. Its a
good way to do the basics very efficiatly. To manufacture a good job/
part, you need to start with a good base, ie nicely squared block in
our case. Related to CNC: 5 sides milled in one set-up. Finish
everything you can top-down. Saw/mill back / finish other half & yer
done. This type of thinking would be good for Heide's Q. (not Q from
Startrek!)<g>

Thanks again for your help. I suggested to my colleges that I would,
in my down time, like to play around with inputing one of your
examples. He did not seem to go for it? He looked at some of the code
& said we dont have that cycle, blah blah blah, option on our machine?
End result: dont waste your time. Ok I'm the 9mo newbie, your the 10yr
veteran.
Life goes on. In the mean time, I figured out the sloting cycle #?
My opp was using a 1/16dia + 1/8R corner rounder around the top edge
of a slot. It has a limitation that gave me a fit right off the bat.
Due to Heide's thinking. You cannot use a smaller cutter rad. comp
value "R" in tool table, less than 1/4 width of slot. = Cutter Comp
Error. Because: Heide's cycle routine is : start at one end of slot,
mill down the center, get to the end, swing on to outer walls & finish
them. Basicaly 3 paths down the slot- with full rad at ends. If the
cutter rad. was less then 1/4 slot width, you'd leave a web of
material, thus not a slot. So I got that figgerd out<g> I got the job
done, by using the fin pkt cycle after pulling my hair out for 2 hrs &
before understanding this simple slot routine.
Apprentice work<g>

Thanks Again Jerry,


--

___ ___
/ /\ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------- \ \/\/
\__\/ \__\/


Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterdays technology
building
Tomorrows Dreams
Cliff
2009-09-26 13:41:28 UTC
Permalink
Raw Message
Post by cncmillgil
It works with a parameter file for
some variables. I'm sure you know of this, but for me its new.
I would like to write a Q program for our standard family of parts.
Same process/tools- different variables/dims.
Get APT.
--
Cliff
cncmillgil
2009-09-28 12:37:21 UTC
Permalink
Raw Message
Post by cncmillgil
It works with a parameter file for
some variables. I'm sure you know of this, but for me its new.
I would like to write a Q program for our standard family of parts.
Same process/tools- different variables/dims.
  Get APT.
--
Cliff
think i'm in-apt!
I came in whilst APT was going out - mid 70's?
MDSI (manuf.data systems inc.) & all that horse hockey time share dial-
up.

Q paramter in Heide's is user defined macro. Input varables & walla -
Just I have to design the input/math calc/ in reagards to speed/feed/
tool dia. ect.

--

~g~
cncmillgil
2009-09-30 01:29:45 UTC
Permalink
Raw Message
Post by cncmillgil
Post by cncmillgil
It works with a parameter file for
some variables. I'm sure you know of this, but for me its new.
I would like to write a Q program for our standard family of parts.
Same process/tools- different variables/dims.
  Get APT.
--
Cliff
think i'm in-apt!
I came in whilst APT was going out - mid 70's?
MDSI (manuf.data systems inc.) & all that horse hockey time share dial-
up.
Q paramter in Heide's is user defined macro. Input varables & walla -
Just I have to design the input/math calc/ in reagards to speed/feed/
tool dia. ect.
--
~g~
That's what I in-vision Q parameter programming Heidenhain style?
Ya ya kinda like BASIC - anybody ever write any BASIC stuff for
geometery calculation/tool path??? I'm sorry I have, back in the
"dark" ages. Before graphical user interfaces. Ya know, command
prompt>, black screen, cursor flashing, the dark ages? type: basic >
enter- wow! WTF is this? gwbasic shit?
Design a program to spit out XYZ numbers for CNC,with user input, use
any math functions on the computer,store varibles in arrays for use
later, if then determinable statements, jumpto/goto's, with counters,
easy stuff.
Beginners All Purpose Instruction Code. now its visual basic- what?
could'nt see it before? now its visual?
Ya did some pretty cool shit, also pulled my hair out,lost sleep,
crashed end mills<g> & bought the welder a new boat:-)

--

___ ___
/ /\ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------- \ \/\/
\__\/ \__\/


Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterdays technology
building
Tomorrows Dreams
Jerry
2009-09-30 02:28:37 UTC
Permalink
Raw Message
I will try to write a sample of Q parameter program tomorrow if I find a
moment.
Jerry
Post by cncmillgil
Post by Cliff
Post by cncmillgil
It works with a parameter file for
some variables. I'm sure you know of this, but for me its new.
I would like to write a Q program for our standard family of parts.
Same process/tools- different variables/dims.
Get APT.
--
Cliff
think i'm in-apt!
I came in whilst APT was going out - mid 70's?
MDSI (manuf.data systems inc.) & all that horse hockey time share dial-
up.
Q paramter in Heide's is user defined macro. Input varables & walla -
Just I have to design the input/math calc/ in reagards to speed/feed/
tool dia. ect.
--
~g~
That's what I in-vision Q parameter programming Heidenhain style?
Ya ya kinda like BASIC - anybody ever write any BASIC stuff for
geometery calculation/tool path??? I'm sorry I have, back in the
"dark" ages. Before graphical user interfaces. Ya know, command
prompt>, black screen, cursor flashing, the dark ages? type: basic >
enter- wow! WTF is this? gwbasic shit?
Design a program to spit out XYZ numbers for CNC,with user input, use
any math functions on the computer,store varibles in arrays for use
later, if then determinable statements, jumpto/goto's, with counters,
easy stuff.
Beginners All Purpose Instruction Code. now its visual basic- what?
could'nt see it before? now its visual?
Ya did some pretty cool shit, also pulled my hair out,lost sleep,
crashed end mills<g> & bought the welder a new boat:-)

--

___ ___
/ /\ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------- \ \/\/
\__\/ \__\/


Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterdays technology
building
Tomorrows Dreams
Jerry
2009-09-30 21:03:23 UTC
Permalink
Raw Message
See if you can figure this out. I was going to face the top with the same
cutter but this would be even more confusing for starters.
All you have to do is describe Q1 Q2 Q3 and Q4 and done. Rest of the Qs are
automatic.
You can copy and paste below program and run it.
Jerry

FN 0: Q1 =+4
* - Q1 is lenght in X
FN 0: Q2 =+2
* - Q2 is with in Y
FN 0: Q3 =+1
* - Q3 is depth in Z
FN 0: Q4 =+0.5
* - Q4 is cutter dia
FN 4: Q24 =+Q4 DIV +2
TOOL DEF 1 L+0 R+Q4
TOOL CALL 1 Z S3000
Q10 = ( Q1 / 2 ) + 0.25
* - Q10 is starting point in X
Q11 = ( Q2 / 2 ) + ( Q4 / 2 ) + 0.25
* - Q11 is starting point in Y
L X-Q10 Y+Q11 R0 FMAX M3
L Z-Q3 R0 FMAX M8
FN 4: Q22 =+Q2 DIV +2
L Y+Q22 RL F200
FN 4: Q21 =+Q1 DIV +2
L X+Q21
L Y-Q22
L X-Q21
L Y+Q22
L IY+0.05
L Z+5 R0 FMAX M9
L M5
Post by cncmillgil
Post by Cliff
Post by cncmillgil
It works with a parameter file for
some variables. I'm sure you know of this, but for me its new.
I would like to write a Q program for our standard family of parts.
Same process/tools- different variables/dims.
Get APT.
--
Cliff
think i'm in-apt!
I came in whilst APT was going out - mid 70's?
MDSI (manuf.data systems inc.) & all that horse hockey time share dial-
up.
Q paramter in Heide's is user defined macro. Input varables & walla -
Just I have to design the input/math calc/ in reagards to speed/feed/
tool dia. ect.
--
~g~
That's what I in-vision Q parameter programming Heidenhain style?
Ya ya kinda like BASIC - anybody ever write any BASIC stuff for
geometery calculation/tool path??? I'm sorry I have, back in the
"dark" ages. Before graphical user interfaces. Ya know, command
prompt>, black screen, cursor flashing, the dark ages? type: basic >
enter- wow! WTF is this? gwbasic shit?
Design a program to spit out XYZ numbers for CNC,with user input, use
any math functions on the computer,store varibles in arrays for use
later, if then determinable statements, jumpto/goto's, with counters,
easy stuff.
Beginners All Purpose Instruction Code. now its visual basic- what?
could'nt see it before? now its visual?
Ya did some pretty cool shit, also pulled my hair out,lost sleep,
crashed end mills<g> & bought the welder a new boat:-)

--

___ ___
/ /\ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------- \ \/\/
\__\/ \__\/


Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterdays technology
building
Tomorrows Dreams
D Murphy
2009-10-02 14:29:24 UTC
Permalink
Raw Message
Post by cncmillgil
That's what I in-vision Q parameter programming Heidenhain style?
Ya ya kinda like BASIC - anybody ever write any BASIC stuff for
geometery calculation/tool path??? I'm sorry I have, back in the
"dark" ages. Before graphical user interfaces. Ya know, command
prompt>, black screen, cursor flashing, the dark ages? type: basic >
enter- wow! WTF is this? gwbasic shit?
Yup. I wrote a program that would comp for the radius on a lather and
another to do trig.

When I was in high school we had a computer which was a huge deal back
then. I wrote a "moon laner" program where you input numbers representing
your thrust and the length of the burn and the program would return you
rate of descent and altitude.

We also learned how to use punch cards and read paper tape. Very cutting
edge back then but all useless today.
--
Dan
Dave B
2009-10-02 20:09:23 UTC
Permalink
Raw Message
Post by D Murphy
Post by cncmillgil
That's what I in-vision Q parameter programming Heidenhain style?
Ya ya kinda like BASIC - anybody ever write any BASIC stuff for
geometery calculation/tool path??? I'm sorry I have, back in the
"dark" ages. Before graphical user interfaces. Ya know, command
prompt>, black screen, cursor flashing, the dark ages? type: basic >
enter- wow! WTF is this? gwbasic shit?
Yup. I wrote a program that would comp for the radius on a lather and
another to do trig.
When I was in high school we had a computer which was a huge deal back
then. I wrote a "moon laner" program where you input numbers representing
your thrust and the length of the burn and the program would return you
rate of descent and altitude.
We also learned how to use punch cards and read paper tape. Very cutting
edge back then but all useless today.
Whoa.........don't offend Cliffie, he loves his Flexowriter.
He is probably knee deep in chad.

Nothing beats an accoutic modem with Compact II.
db
D Murphy
2009-10-02 22:56:36 UTC
Permalink
Raw Message
Post by Dave B
Whoa.........don't offend Cliffie, he loves his Flexowriter.
He is probably knee deep in chad.
Nothing beats an accoutic modem with Compact II.
LOL. Yeah, I can see him pining for the good ole days when he could blame
the horrific crashes caused by his error riddled code on hanging chad and
dirty tape readers.
--
Dan
cncmillgil
2009-10-02 23:48:49 UTC
Permalink
Raw Message
Post by Dave B
Post by D Murphy
Post by cncmillgil
That's what I in-vision Q parameter programming Heidenhain style?
Ya ya kinda like BASIC - anybody ever write any BASIC stuff for
geometery calculation/tool path??? I'm sorry I have, back in the
"dark" ages. Before graphical user interfaces. Ya know, command
prompt>, black screen, cursor flashing, the dark ages? type: basic >
enter- wow! WTF is this? gwbasic shit?
Yup. I wrote a program that would comp for the radius on a lather and
another to do trig.
When I was in high school we had a computer which was a huge deal back
then. I wrote a "moon laner" program where you input numbers representing
your thrust and the length of the burn and the program would return you
rate of descent and altitude.
We also learned how to use punch cards and read paper tape. Very cutting
edge back then but all useless today.
Whoa.........don't offend Cliffie, he loves his Flexowriter.
He is probably knee deep in chad.
Nothing beats an accoutic modem with Compact II.
  db
would that be the 150bps or the cadilac 300bps modem that fit the Bell
Telephone hand set on rubber cups?
Man I wish I had a couple of buckets of the ol chads. Mylar's were the
tits! Damn indestuctable. Better have a heavy duty punch.
The are great for gag joke/prank type silly string partys. Man their a
bitch to sweep up. Vacuum is the only way.
Hell at one time I could read the hole punchs ....:... ( X +
10.187)....... ya right. Man readable leaders were the ticket.

--

___ ___
/ /\ / /\
/ /__\ / /\/\
/__/ / ------------------------------------ /__/\/\/
\ \ / ------------------------------- \ \/\/
\__\/ \__\/


Gil©
Member of
==American Toolmakers==
using the "old world" ways
with yesterdays technology
building
Tomorrows Dreams
Dhinesh
2014-11-26 19:18:05 UTC
Permalink
Raw Message
replying to Jerry, Dhinesh wrote:




Jerry,

I am using Creo ( Pro/E) for CAD and CAM.

I need post processor for DMG DMU 80P with Heidenhain iTNC530 controller.

Can you help me?

--
Dhinesh
--
posted from
http://www.polytechforum.com/cnc/heidenhain-itnc-530-tap-cycle-help-conversational-format-43610-.htm
using PolytechForum's Web, RSS and Social Media Interface to
alt.machines.cnc and other engineering groups
s***@gmail.com
2014-03-11 11:03:27 UTC
Permalink
Raw Message
Hi,Will someone post or email some programming example of a tap cycle. Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206 floating would be a big help. I don't get an alarm, but I also don't get an tapped hole. Spindle comes down to xy then z point then the spindle looks like it releases from being engaged -it does a 1-degree wiggle- then home and done. Sans guzinta. CNC and control do have tapping. With no alarms popping up, it must be me and it must be simple because i am simple.Regards
s***@gmail.com
2017-04-11 07:30:54 UTC
Permalink
Raw Message
Post by b***@gmail.com
Hi,
Will someone post or email some programming example of a tap cycle.
Specifically CYCL DEF 209 TAPPING W/ CHIP BRKG but 207 or 206
floating would be a big help.
I don't get an alarm, but I also don't get an tapped hole. Spindle
comes down to xy then z point then the spindle looks like it releases
from being engaged -it does a 1-degree wiggle- then home and done.
Sans guzinta.
CNC and control do have tapping. With no alarms popping up, it must
be me and it must be simple because i am simple.
Regards
I have upto 4 axis positioning post processor Itnc530

Loading...