Discussion:
Mori Seki SL1 NC lathe programming
(too old to reply)
c***@cox.net
2006-04-27 01:36:28 UTC
Permalink
Raw Message
THanks to the several who have helped me get my lathe running! It all
seems to be fixed up and even the BTR is working. Now I have to get
the programming figured out. When I write simple code to move or turn
the turret, I keep getting error message 14 indicating bad characters.
Should I be able to enter something like that below as a test?

N01 G98 S1000 M3 M8
N02 G00 X2.0 Z-2.0
N03 M5 M9
N05 G00 X0 Z0
N04 M30

Thanks,
Keith Clark
John
2006-04-27 01:49:49 UTC
Permalink
Raw Message
Post by c***@cox.net
THanks to the several who have helped me get my lathe running! It all
seems to be fixed up and even the BTR is working. Now I have to get
the programming figured out. When I write simple code to move or turn
the turret, I keep getting error message 14 indicating bad characters.
Should I be able to enter something like that below as a test?
N01 G98 S1000 M3 M8
N02 G00 X2.0 Z-2.0
N03 M5 M9
N05 G00 X0 Z0
N04 M30
Thanks,
Keith Clark
The control may only be able to handle one M code in a block/

John
John
2006-04-27 01:50:46 UTC
Permalink
Raw Message
Post by c***@cox.net
THanks to the several who have helped me get my lathe running! It all
seems to be fixed up and even the BTR is working. Now I have to get
the programming figured out. When I write simple code to move or turn
the turret, I keep getting error message 14 indicating bad characters.
Should I be able to enter something like that below as a test?
N01 G98 S1000 M3 M8
N02 G00 X2.0 Z-2.0
N03 M5 M9
N05 G00 X0 Z0
N04 M30
Thanks,
Keith Clark
The G98 may not be used on that machine.

John
c***@cox.net
2006-04-27 03:05:15 UTC
Permalink
Raw Message
Thanks John, I discovered that only one M code is allowed, that
helped. I think I may have some other problems with parameters. I
will post another question on that problem. I am still having the
error message but the parameters are wrong.

thanks
Keith
Dave Lyon
2006-04-27 14:13:02 UTC
Permalink
Raw Message
Post by c***@cox.net
THanks to the several who have helped me get my lathe running! It all
seems to be fixed up and even the BTR is working. Now I have to get
the programming figured out. When I write simple code to move or turn
the turret, I keep getting error message 14 indicating bad characters.
Should I be able to enter something like that below as a test?
N01 G98 S1000 M3 M8
N02 G00 X2.0 Z-2.0
N03 M5 M9
N05 G00 X0 Z0
N04 M30
Thanks,
Keith Clark
Are you sending this program to the machine?

It could be that your parity, or other comm setting is wrong.

Try sending from the machine to the computer.
c***@cox.net
2006-04-27 14:22:51 UTC
Permalink
Raw Message
My machine does not have the rs232 port to send out from machine to
punch or BTR but when I look manually at the content of the addresses
the program seems to be there correctly downloaded. I think I just
have to get more familiar with the conventions required.

I plan to do a one block at a time download to see where the problems
occur.

I am confused by the g50 command. When the machine is zeroed the x and
z coordinates are 0 and 0. Why do I need the g50.? Is is possible to
change the absolute coordinates of the zero position for x and z? How
does one know what values to enter?

Thanks
Keith
Dave Lyon
2006-04-27 14:55:58 UTC
Permalink
Raw Message
Post by c***@cox.net
My machine does not have the rs232 port to send out from machine to
punch or BTR but when I look manually at the content of the addresses
the program seems to be there correctly downloaded. I think I just
have to get more familiar with the conventions required.
I'm a little confused. You said you have a BTR, which to me means a board
that emulates a tape reader/punch so you can send info to and from a
computer. Is that correct?

It is possible that you are putting in some codes that your machine doesn't
like, such as the 2 M codes in one line. If I am correct in what you are
trying to do, it is also possible that you're getting some noise from your
communication line. If you're sending code from a computer, make sure that
you are using a text only word processor. Sometimes, if you're not, the
software may send a formatting or other hidden character that your machine
does not understand, and can't display. Or, you could be overflowing the
buffer on your older machine and dropping characters (probably not on that
short of a program).
brewertr
2006-04-27 15:59:13 UTC
Permalink
Raw Message
Keith,

G50 is your tool offset geometry and you need it for each tool.
Normaly X is to centerline of spindle and Z is usually to the end of
your completed part.

Zero Return the machine
Origin X and Z axis if not 0 in each counter
Index to tool
Start Spindle

Face off your part or touch the front.
Z axis reading + or - whatever the raw material condition is and
this is your G50 Z input.

Turn the OD
X axis reading + the OD diameter and the answer is your G50 X input.

Now some machines the Z could be Z- or + so you need to work that out
and X is the same way.

In this example I am assuming Z zero is the finish face (length) and X
is Zero is Spindle Centerline.

Tool #1

Z axis at home counter is 0. Face off part and the counter reading is
Z9.850, you check the part and you have .025 material left to face off.
Z = 9.850+.025 = 9.875

X axis at home counter is 0. Turn the OD and the counter reading
X5.908 mic the OD and the part is 1.507. X= 5.908
+ 1.507= 7.415

In this example G50 X7.415 Z9.875

Once your tools are set and you don't change the tool you never need to
change the X value. For Z you only need check one tool then make the
same adjustment to all the others (this is equivalent to a work shift).

For drills indicate the center of tool holder and that is your X value
and that will never change unless something changes on the machine.

For my example it assumes you are programming X+ values and Z- values.

Tom
Post by c***@cox.net
My machine does not have the rs232 port to send out from machine to
punch or BTR but when I look manually at the content of the addresses
the program seems to be there correctly downloaded. I think I just
have to get more familiar with the conventions required.
I plan to do a one block at a time download to see where the problems
occur.
I am confused by the g50 command. When the machine is zeroed the x and
z coordinates are 0 and 0. Why do I need the g50.? Is is possible to
change the absolute coordinates of the zero position for x and z? How
does one know what values to enter?
Thanks
Keith
Cliff
2006-04-27 16:13:51 UTC
Permalink
Raw Message
Post by brewertr
G50 is your tool offset geometry and you need it for each tool.
Normaly X is to centerline of spindle and Z is usually to the end of
your completed part.
Z: I'd think any locating surface .... to the chuck or fixture ... not
some later machined feature.
--
Cliff
Cliff
2006-04-27 16:15:55 UTC
Permalink
Raw Message
Post by brewertr
G50 is your tool offset geometry and you need it for each tool.
Normaly X is to centerline of spindle and Z is usually to the end of
your completed part.
X: Would that be to tool touch-off or to the center
of the tool nose radius?

Might be some good fishing here <G>.
--
Cliff
brewertr
2006-04-27 20:43:26 UTC
Permalink
Raw Message
Cliff wrote:
snip
Post by Cliff
X: Would that be to tool touch-off or to the center
of the tool nose radius?
My example is Tool edge for both Z & X.

Tom
Cliff
2006-04-27 20:58:48 UTC
Permalink
Raw Message
Post by brewertr
snip
Post by Cliff
X: Would that be to tool touch-off or to the center
of the tool nose radius?
My example is Tool edge for both Z & X.
Kind of hard to cut to center then ...?
Diameter programming .... or radial ....
--
Cliff
D Murphy
2006-04-27 20:51:38 UTC
Permalink
Raw Message
Post by Cliff
X: Would that be to tool touch-off or to the center
of the tool nose radius?
Nope. It would be to the center of a drill holder. Offset other tools from
there.
--
Dan

Quid Aere Perennius
Cliff
2006-04-27 21:00:38 UTC
Permalink
Raw Message
Post by D Murphy
Post by Cliff
X: Would that be to tool touch-off or to the center
of the tool nose radius?
Nope. It would be to the center of a drill holder. Offset other tools from
there.
On some machines that might be about the same as the turret
centerline ..
--
Cliff
c***@cox.net
2006-04-27 16:22:52 UTC
Permalink
Raw Message
I see the logic and this is described in the manual but I did not
realize I had to enter a g50 for each tool. I may have been confused
between g50 and tool offset. It seems like with tool offset feature I
could enter x and z tool offset value obtained as you have described
for each tool. Then, I would not have to issue g50 for each tool?

Thanks,
Keith
Cliff
2006-04-27 16:10:10 UTC
Permalink
Raw Message
Post by c***@cox.net
Thanks
Can you get any support from the machine's seller?
--
Cliff
john
2006-04-27 16:29:11 UTC
Permalink
Raw Message
Post by c***@cox.net
My machine does not have the rs232 port to send out from machine to
punch or BTR but when I look manually at the content of the addresses
the program seems to be there correctly downloaded. I think I just
have to get more familiar with the conventions required.
I plan to do a one block at a time download to see where the problems
occur.
I am confused by the g50 command. When the machine is zeroed the x and
z coordinates are 0 and 0. Why do I need the g50.? Is is possible to
change the absolute coordinates of the zero position for x and z? How
does one know what values to enter?
Thanks
Keith
I would start with a very simple program to check the data link...Turn
the spindle on, turn it off end of program. That machine may not
have a lot of stuff like newer machines have... like a G50.

M03 S200
M05
M30


Then make a prgram with a simple X move and Z move. Use only G00 codes
and G01 codes with a feedrate.

One thing at a time until you find what it takes. Or get a programming
book for the control with all the info in it.


John
c***@cox.net
2006-04-27 17:44:17 UTC
Permalink
Raw Message
Sounds like a good suggestion. I just discovered that I have a Yasnac
2000B not G but Yaskawa says to use the G manual. It does have a G50
supposedly. I'll see if it works line by line as you suggest.

Keith
F. George McDuffee
2006-04-27 17:31:00 UTC
Permalink
Raw Message
Post by c***@cox.net
THanks to the several who have helped me get my lathe running! It all
seems to be fixed up and even the BTR is working. Now I have to get
the programming figured out. When I write simple code to move or turn
the turret, I keep getting error message 14 indicating bad characters.
Should I be able to enter something like that below as a test?
N01 G98 S1000 M3 M8
N02 G00 X2.0 Z-2.0
N03 M5 M9
N05 G00 X0 Z0
N04 M30
Thanks,
Keith Clark
=============
What are you using for an editor? In many cases a general purpose
editor program inserts non-printing control characters with the
text. Try using a cnc specific editor. You can also download
one of the old DOS sector patcher programs to examine the file
character by character. This can be helpful if you can down-up
load programs from the machine to the computer but not programs
you write on the computer to the machine. Typically the manuals
never mention this, but the programs written on the machine and
downloaded to the computer will contain non-printing control
characters.

Just a though.

Unka George
(George McDuffee)

There is something to be said for government by a great aristocracy
which has furnished leaders to the nation in peace and war for generations;
even a democrat like myself must admit this.

But there is absolutely nothing to be said for government by a plutocracy,
for government by men very powerful in certain lines and gifted with the "money touch,"
but with ideals which in their essence are merely those of so many glorified pawnbrokers.

Theodore Roosevelt (1858-1919), U.S. Republican (later Progressive) politician, president. Letter, 15 Nov. 1913.
c***@cox.net
2006-04-27 17:45:18 UTC
Permalink
Raw Message
Thanks, good suggestion!

Keith
Loading...