Cutter comp not working - Makino V33 w/ Fanuc Proffesional 3

[s***@hotmail.com]

Ran a program yesterday and cutter comp appeared to be working fine
(Tool 2)

Tried running a program today using cutter comp on Tool 6 and it just
wont work. Runs right on cutter path and doesn't change no matter what
I change the offset to.

Changing my "D" in "Custom/ Tool Detail/ Input/ D-Value"

Code generated in Surfcam as "Offset w/ compensation" so my D-Value
default is 0.0, -.01 for a .010 smaller cutter, ect...

Anyone have a hint for me as to why this isn't working? Any help
appreciated -
Thanks
Sean

%
G20
O1234
(MAKINO SUB)
G91 G28 Z0
T06
M6
M1
G00 G54 G90 G40 G49 G80 G99
S16306 M3
T03
X-0.247 Y0.029
G43 Z0.2 H1 M8
G05 P10000
G00 Z0.1
G01 Z-0.125 F5.9

(Comp call ...)
G41 X-0.297 F11.7 D6
(Cuts ...)

G01 Y-0.029
X0.235
.................

[Bryce]

Post by s***@hotmail.com
Tried running a program today using cutter comp on Tool 6 and it just
wont work. Runs right on cutter path and doesn't change no matter what
I change the offset to.
G01 Z-0.125 F5.9
(Comp call ...)
G41 X-0.297 F11.7 D6
(Cuts ...)
G01 Y-0.029
X0.235
.................

Is there still a G01 modally active at the line that has the G41?
IIRC most controllers won't turn on cutter comp if G00 is active.
Might check that.

[BottleBob]

Post by s***@hotmail.com
Ran a program yesterday and cutter comp appeared to be working fine
(Tool 2)
Tried running a program today using cutter comp on Tool 6 and it just
wont work. Runs right on cutter path and doesn't change no matter what
I change the offset to.

Sean:

Someone at work yesterday was having cutter comp. problems with our
Makino J55 with ProIII control. His problem was that he had a start
hole that he wanted the endmill to start in and he programmed a .030
radius entry path before the actual cut began. The tool was 3/16" in
diameter and it seems there wasn't enough entry length to engage comp.
He changed to a longer straight entry path and the problem was solved.
I wonder if that could be related to your own problem. You could try a
longer entry (over half the dia. of the tool), while calling out comp.
before the actual part cut path starts.

[s***@hotmail.com]

Post by BottleBob

Post by s***@hotmail.com
Ran a program yesterday and cutter comp appeared to be working fine
(Tool 2)
Tried running a program today using cutter comp on Tool 6 and it just
wont work. Runs right on cutter path and doesn't change no matter what
I change the offset to.

Someone at work yesterday was having cutter comp. problems with our
Makino J55 with ProIII control. His problem was that he had a start
hole that he wanted the endmill to start in and he programmed a .030
radius entry path before the actual cut began. The tool was 3/16" in
diameter and it seems there wasn't enough entry length to engage comp.
He changed to a longer straight entry path and the problem was solved.
I wonder if that could be related to your own problem. You could try a
longer entry (over half the dia. of the tool), while calling out comp.
before the actual part cut path starts.
--
BottleBob
http://home.earthlink.net/~bottlbob

Thanks for the suggestions -

My G1 is active for the G41 move.
I am using a radial ramp in to my face, with a linear comp-in move of
.05 for a .0937 cutter.
I wonder if my tool pre-select call could be screwing it up? Although I
had a tool pre-select in my program yesterday - the one in which the
cutter comp actually worked. Have to try that next if I can find a
minute.
Fucking problems always appear when I have a 10hr job that needs to be
done in 5hrs.

Thanks
Sean

[BottleBob]

Post by s***@hotmail.com
My G1 is active for the G41 move.
I am using a radial ramp in to my face, with a linear comp-in move of
.05 for a .0937 cutter.
I wonder if my tool pre-select call could be screwing it up? Although I
had a tool pre-select in my program yesterday - the one in which the
cutter comp actually worked. Have to try that next if I can find a
minute.

Sean:

If all else fails you can try to do ALL your tool offset in the CAM
system rather than in the control. <g>

[s***@hotmail.com]

Post by BottleBob

Post by s***@hotmail.com
My G1 is active for the G41 move.
I am using a radial ramp in to my face, with a linear comp-in move of
.05 for a .0937 cutter.
I wonder if my tool pre-select call could be screwing it up? Although I
had a tool pre-select in my program yesterday - the one in which the
cutter comp actually worked. Have to try that next if I can find a
minute.

If all else fails you can try to do ALL your tool offset in the CAM
system rather than in the control. <g>
--
BottleBob
http://home.earthlink.net/~bottlbob

Yeah - thats what I'm doing. Easier changing an offset at the control,
rather than running back and reposting in Surfcam every time I need a
slight change, though. Oh well.

[Bryce]

Post by s***@hotmail.com

Post by BottleBob
If all else fails you can try to do ALL your tool offset in the CAM
system rather than in the control. <g>
--
BottleBob
http://home.earthlink.net/~bottlbob

Yeah - thats what I'm doing. Easier changing an offset at the control,
rather than running back and reposting in Surfcam every time I need a
slight change, though. Oh well.

Maybe you can have Cliff post it for you, since Engineers/Programmers
are always right the first time. <G>

Operators always enter the wrong offsets. <G>

[brewertr]

Post by Bryce
Maybe you can have Cliff post it for you, since Engineers/Programmers
are always right

Bryce,

"Cliff, Programmer" says Alex Trebek

"What is an Oxymoron?" responds jeopardy contestant

"Correct for $200"

I guess you missed where Cliff posted a sample of his CNC Lathe
programming, Cliff posted 2 lines of G-Code with 5 mistakes in it.

Tom

[s***@hotmail.com]

Post by Bryce
Maybe you can have Cliff post it for you, since Engineers/Programmers
are always right the first time. <G>
Operators always enter the wrong offsets. <G>
--
Bryce
----== Posted via Newsfeeds.Com - Unlimited-Unrestricted-Secure Usenet News==----
http://www.newsfeeds.com The #1 Newsgroup Service in the World! 120,000+ Newsgroups
----= East and West-Coast Server Farms - Total Privacy via Encryption =----

Maybe thats the problem.
Since I am programmer and operator, I'm doing things wrong HALF the time

[Bryce]

Post by s***@hotmail.com

Post by Bryce
Maybe you can have Cliff post it for you, since Engineers/Programmers
are always right the first time. <G>
Operators always enter the wrong offsets. <G>

Maybe thats the problem.
Since I am programmer and operator, I'm doing things wrong HALF the time

LOL. Me too.

Great thing is I always (well, usually) know what I was thinking when
I programmed it. Does tend to help during setup.

[Dave Lyon]

Post by s***@hotmail.com
Ran a program yesterday and cutter comp appeared to be working fine
(Tool 2)
Tried running a program today using cutter comp on Tool 6 and it just
wont work. Runs right on cutter path and doesn't change no matter what
I change the offset to.
Changing my "D" in "Custom/ Tool Detail/ Input/ D-Value"
Code generated in Surfcam as "Offset w/ compensation" so my D-Value
default is 0.0, -.01 for a .010 smaller cutter, ect...
Anyone have a hint for me as to why this isn't working? Any help
appreciated -
Thanks
Sean
%
G20
O1234
(MAKINO SUB)
G91 G28 Z0
T06
M6
M1
G00 G54 G90 G40 G49 G80 G99
S16306 M3
T03
X-0.247 Y0.029
G43 Z0.2 H1 M8
G05 P10000
G00 Z0.1
G01 Z-0.125 F5.9
(Comp call ...)
G41 X-0.297 F11.7 D6
(Cuts ...)
G01 Y-0.029
X0.235
.................

Many years ago, we had a machine that wouldn't use cutter comp for tool 2. I
don't know why, never figured it out. We just made sure we didn't use tool
2.

[PrecisionMachinisT]

Post by Dave Lyon

Post by s***@hotmail.com
Ran a program yesterday and cutter comp appeared to be working fine
(Tool 2)
Tried running a program today using cutter comp on Tool 6 and it just
wont work. Runs right on cutter path and doesn't change no matter what
I change the offset to.
Changing my "D" in "Custom/ Tool Detail/ Input/ D-Value"
Code generated in Surfcam as "Offset w/ compensation" so my D-Value
default is 0.0, -.01 for a .010 smaller cutter, ect...
Anyone have a hint for me as to why this isn't working? Any help
appreciated -
Thanks
Sean
%
G20
O1234
(MAKINO SUB)
G91 G28 Z0
T06
M6
M1
G00 G54 G90 G40 G49 G80 G99
S16306 M3
T03
X-0.247 Y0.029
G43 Z0.2 H1 M8
G05 P10000
G00 Z0.1
G01 Z-0.125 F5.9
(Comp call ...)
G41 X-0.297 F11.7 D6
(Cuts ...)
G01 Y-0.029
X0.235
.................

Many years ago, we had a machine that wouldn't use cutter comp for tool 2. I
don't know why, never figured it out. We just made sure we didn't use tool
2.

But...he's having a problem with tool 6, NOT tool 2.

Suggest do try and keep up.....

--

SVL

[Dave Lyon]

Post by PrecisionMachinisT

Post by Dave Lyon
Many years ago, we had a machine that wouldn't use cutter comp for tool

2.

Post by PrecisionMachinisT
I

Post by Dave Lyon
don't know why, never figured it out. We just made sure we didn't use tool
2.

But...he's having a problem with tool 6, NOT tool 2.
Suggest do try and keep up.....
--
SVL

Sorry, I don't know what I was thinking.

[s***@hotmail.com]

Post by Dave Lyon

Post by PrecisionMachinisT

Post by Dave Lyon
Many years ago, we had a machine that wouldn't use cutter comp for tool

2.

Post by PrecisionMachinisT
I

Post by Dave Lyon
don't know why, never figured it out. We just made sure we didn't use

tool

Post by PrecisionMachinisT

Post by Dave Lyon
2.

But...he's having a problem with tool 6, NOT tool 2.
Suggest do try and keep up.....
--
SVL

Sorry, I don't know what I was thinking.

YEAh! Tool #2 is the only one that I could get to work.

[Dave Lyon]

Post by s***@hotmail.com

Post by Dave Lyon

Post by PrecisionMachinisT

Post by Dave Lyon
Many years ago, we had a machine that wouldn't use cutter comp for tool

2.

Post by PrecisionMachinisT
I

Post by Dave Lyon
don't know why, never figured it out. We just made sure we didn't use

tool

Post by PrecisionMachinisT

Post by Dave Lyon
2.

But...he's having a problem with tool 6, NOT tool 2.
Suggest do try and keep up.....
--
SVL

Sorry, I don't know what I was thinking.

YEAh! Tool #2 is the only one that I could get to work.

Have you tried different tool and "D" numbers? I know it's a long shot with
the quality of controls today, but I'm curious.

[PrecisionMachinisT]

Post by Dave Lyon

Post by s***@hotmail.com

Post by Dave Lyon

Post by PrecisionMachinisT

Post by Dave Lyon
Many years ago, we had a machine that wouldn't use cutter comp for

tool

Post by s***@hotmail.com

Post by Dave Lyon
2.

Post by PrecisionMachinisT
I

Post by Dave Lyon
don't know why, never figured it out. We just made sure we didn't

use

Post by s***@hotmail.com

Post by Dave Lyon
tool

Post by PrecisionMachinisT

Post by Dave Lyon
2.

But...he's having a problem with tool 6, NOT tool 2.
Suggest do try and keep up.....
--
SVL

Sorry, I don't know what I was thinking.

YEAh! Tool #2 is the only one that I could get to work.

Have you tried different tool and "D" numbers? I know it's a long shot with
the quality of controls today, but I'm curious.

My experiences are that usually it's a problem with lead-in / leadout, else
there some geometry that isn't developable without a possible undercut where
enveloping a cutcom profile is concerned--whereas no such advance checks are
possible where only the pure x y moves are provided.

Suspect to me is the fact that he is using a .093 tool yet his y axis data
suggests that he might only .058 total of wiggle room in the y axis.--what
I'd really like to see is to have him to post the entire code output, what
with look-ahead as advanced as it is now-adays--maybe then could we run it
through different controllers if nothing obvious is seen...kinda see what
happens.

--

SVL

[Dave Lyon]

Post by PrecisionMachinisT
My experiences are that usually it's a problem with lead-in / leadout, else
there some geometry that isn't developable without a possible undercut where
enveloping a cutcom profile is concerned--whereas no such advance checks are
possible where only the pure x y moves are provided.

Yep, that is the normal problem. I just assumed he had already checked for
the obvious.

[ff]

Post by s***@hotmail.com
Ran a program yesterday and cutter comp appeared to be working fine
(Tool 2)
Tried running a program today using cutter comp on Tool 6 and it just
wont work. Runs right on cutter path and doesn't change no matter what
I change the offset to.
Changing my "D" in "Custom/ Tool Detail/ Input/ D-Value"
Code generated in Surfcam as "Offset w/ compensation" so my D-Value
default is 0.0, -.01 for a .010 smaller cutter, ect...
Anyone have a hint for me as to why this isn't working? Any help
appreciated -
Thanks
Sean
%
G20
O1234
(MAKINO SUB)
G91 G28 Z0
T06
M6
M1
G00 G54 G90 G40 G49 G80 G99
S16306 M3
T03
X-0.247 Y0.029
G43 Z0.2 H1 M8
G05 P10000
G00 Z0.1
G01 Z-0.125 F5.9
(Comp call ...)
G41 X-0.297 F11.7 D6
(Cuts ...)
G01 Y-0.029
X0.235
.................

I'm late to the party again, but shouldn't that line:

G43 Z0.2 H1 M8

be instead:

G43 Z0.2 H6 M8

????

[PrecisionMachinisT]

Post by s***@hotmail.com

Post by s***@hotmail.com
Ran a program yesterday and cutter comp appeared to be working fine
(Tool 2)
Tried running a program today using cutter comp on Tool 6 and it just
wont work. Runs right on cutter path and doesn't change no matter what
I change the offset to.
Changing my "D" in "Custom/ Tool Detail/ Input/ D-Value"
Code generated in Surfcam as "Offset w/ compensation" so my D-Value
default is 0.0, -.01 for a .010 smaller cutter, ect...
Anyone have a hint for me as to why this isn't working? Any help
appreciated -
Thanks
Sean
%
G20
O1234
(MAKINO SUB)
G91 G28 Z0
T06
M6
M1
G00 G54 G90 G40 G49 G80 G99
S16306 M3
T03
X-0.247 Y0.029
G43 Z0.2 H1 M8
G05 P10000
G00 Z0.1
G01 Z-0.125 F5.9
(Comp call ...)
G41 X-0.297 F11.7 D6
(Cuts ...)
G01 Y-0.029
X0.235
.................

G43 Z0.2 H1 M8
G43 Z0.2 H6 M8

Naww, H is for tool lenght, and D is for cutcom--differnt aminals.

FWIW usually the g43 / g49 cancel codes is redundant code...what with std
parameter setting generally specifying g43 as defaulkt bootup modal, the
common practice is one toggles outa last the called H ## by specifying an H0
along with any move to g91 g28 ( g30 ) so as to bring slide to machine atc
position....and then afterwards, he specifys the new H along with the first
g90 move after atc completion.

--

SVL

[Bart]

Post by PrecisionMachinisT

Post by s***@hotmail.com

Post by s***@hotmail.com
%
G20
O1234
(MAKINO SUB)
G91 G28 Z0
T06
M6
M1
G00 G54 G90 G40 G49 G80 G99
S16306 M3
T03
X-0.247 Y0.029
G43 Z0.2 H1 M8
G05 P10000
G00 Z0.1
G01 Z-0.125 F5.9
(Comp call ...)
G41 X-0.297 F11.7 D6
(Cuts ...)
G01 Y-0.029
X0.235
.................

G43 Z0.2 H1 M8
G43 Z0.2 H6 M8

Naww, H is for tool lenght, and D is for cutcom--differnt aminals.
snip>
SVL

Many programmers use an "H" number that coincides with the tool number they
are using.
In this case the code calls H1 for tool number 6 (T6;M6;)
Good observation by "ff", should not be dismissed so lightly. Irregularities
in code/offsets, and a complaint that comp is not working deserves thorough
scrutiny.
HTH
Bart

[r***@chartermi.net]

Post by s***@hotmail.com
Ran a program yesterday and cutter comp appeared to be working fine
(Tool 2)
Tried running a program today using cutter comp on Tool 6 and it just
wont work. Runs right on cutter path and doesn't change no matter what
I change the offset to.
Changing my "D" in "Custom/ Tool Detail/ Input/ D-Value"
Code generated in Surfcam as "Offset w/ compensation" so my D-Value
default is 0.0, -.01 for a .010 smaller cutter, ect...
Anyone have a hint for me as to why this isn't working? Any help
appreciated -
Thanks
Sean
%
G20
O1234
(MAKINO SUB)
G91 G28 Z0
T06
M6
M1
G00 G54 G90 G40 G49 G80 G99
S16306 M3
T03
X-0.247 Y0.029
G43 Z0.2 H1 M8
G05 P10000
G00 Z0.1
G01 Z-0.125 F5.9
(Comp call ...)
G41 X-0.297 F11.7 D6
(Cuts ...)
G01 Y-0.029
X0.235
.................

On all of our Makino machines, we must use H1 & D2 in all of our
programs. The data for the length and cutter comp is transfered from
the Makino tool data page to H1 & D2 at tool change. The D6 will not
work, on our machines anyway.

Hope this helps,

RJ

[Joe788]

Post by r***@chartermi.net
On all of our Makino machines, we must use H1 & D2 in all of our
programs. The data for the length and cutter comp is transfered from
the Makino tool data page to H1 & D2 at tool change. The D6 will not
work, on our machines anyway.
Hope this helps,
RJ

I believe this is the answer to the problem. I forgot that Makinos just
want to see H1 D2 for every tool, which would explain why D2 worked for
him, but D6 won't.

[brewertr]

Post by Joe788

Post by r***@chartermi.net
On all of our Makino machines, we must use H1 & D2 in all of our
programs. The data for the length and cutter comp is transfered from
the Makino tool data page to H1 & D2 at tool change. The D6 will not
work, on our machines anyway.
Hope this helps,
RJ

I believe this is the answer to the problem. I forgot that Makinos just
want to see H1 D2 for every tool, which would explain why D2 worked for
him, but D6 won't.

Joe,

Easy to see how that can be confusing for someone who is new to / not
familiar with Makino.

Tom

[Dave Lyon]

Post by Joe788
I believe this is the answer to the problem. I forgot that Makinos just
want to see H1 D2 for every tool, which would explain why D2 worked for
him, but D6 won't.

I ran a Makino a number of years ago that did NOT work that way. Of course
it was using a Fanuc control.

[BottleBob]

Post by Dave Lyon

Post by Joe788
I believe this is the answer to the problem. I forgot that Makinos just
want to see H1 D2 for every tool, which would explain why D2 worked for
him, but D6 won't.

I ran a Makino a number of years ago that did NOT work that way. Of course
it was using a Fanuc control.

Dave:

Our Makino works that way and has a Pro-III control that I believe is
Fanuc.

[Dave Lyon]

Post by BottleBob

Post by Dave Lyon
I ran a Makino a number of years ago that did NOT work that way. Of course
it was using a Fanuc control.

Our Makino works that way and has a Pro-III control that I believe is
Fanuc.
--
BottleBob
http://home.earthlink.net/~bottlbob

That seems strange to me. Why did they deviate from the norm? What advantage
is there?

[Nagesh S K]

Post by s***@hotmail.com
Ran a program yesterday and cutter comp appeared to be working fine
(Tool 2)
Tried running a program today using cutter comp on Tool 6 and it just
wont work. Runs right on cutter path and doesn't change no matter what
I change the offset to.
Changing my "D" in "Custom/ Tool Detail/ Input/ D-Value"

Try entering D-value in offset/setting -->offset page. It works on our
Makino S56 with Pro3.

Post by s***@hotmail.com
Code generated in Surfcam as "Offset w/ compensation" so my D-Value
default is 0.0, -.01 for a .010 smaller cutter, ect...
Anyone have a hint for me as to why this isn't working? Any help
appreciated -
Thanks
Sean

HTH

SKN