Supermax lathe programming problem.

I'm very new to this CNC lathe world. I purchased a supermax ycm-tc-2 last fall and finally have the phase converter up and running, tooling dialed in, and have written a program for the OT fanuc controls. I've been struggling with programming "part zero" but think I figured that out. I am mentioning this in case it is part of my current issue. In addition, I wrote a simple facing program that I could not to get to work, After hours wasted I read in the manual that in MDI mode you cannot use canned cycles G71 g72 or G73. I then attempted to use G75 cycle as the manual states that will work. This is an old "tape" machine and I cannot load any data unless I use MDI. As if right now, in addition to being really frustrated, I've discovered that no matter how I write the code I cannot use any form of "Feed" specification or the program stops. I do not get an alarm message though. I can use g00 all day and send tooling where ever I want, but as soon as I use any g01 code with a feed the machine just stops, in the same way it did every time I used a canned cycle. When I run a "previous owner program" from the memory it works just fine and has no issues with feed values. I've searched the memory and I can't find any programs from previous owner using canned cycles, he used all g01 codes with feeds. I've tried just very simple programming using go1 codes also. But for some reason they only wont work in "my" program. I don't know what I am missing in setup or in the program? Any ideas? I even copied his program line for line using the size parameters I needed and still can't get it to work. Thanks in advance for the help!

Where to begin? Never tried running canned cycles from MDI. Feed override on zero? G99 G1 X/Z Feed won't move unless the spindle is turning, try G98 G1 X/Z Feed?

Instead of a thousand questions from the group maybe you can post the exact code your trying to run for us to see. Most likely someone will get you going

Brent

yardbird said:

...Instead of a thousand questions from the group maybe you can post the exact code your trying to run for us to see. Most likely someone will get you going

Click to expand...

Gotta love trying to help someone asking to troubleshoot their program when they don't post the problem program!

trouble shooting

Vancbiker said:

Gotta love trying to help someone asking to troubleshoot their program when they don't post the problem program!

Click to expand...

I figured I'd be asked a bunch of questions if I received responses. Stating the program was an obvious idea, but perhaps there was something much more basic I missed that someone more knowledgeable might see that I would have overlooked as a beginner. Plus, I basically copied and pasted a working program in the memory. I've not been on this forum before and posting a two hundred word post did not seem like a great idea with every parameter and code in the machine as I understand it. I'll post the programming I used later tonight.

Simple fix!

yardbird said:

Where to begin? Never tried running canned cycles from MDI. Feed override on zero? G99 G1 X/Z Feed won't move unless the spindle is turning, try G98 G1 X/Z Feed?

Instead of a thousand questions from the group maybe you can post the exact code your trying to run for us to see. Most likely someone will get you going


Brent

Click to expand...

It really was that simple! I was originally using the G72 code, that, as mentioned, can't be programmed in the MDI mode. When I switched to g75 cycle while trying to figure everything out I set spindle speed to zero as I was tired of it starting up every time I was testing, and then it not working. In addition I had the feed rate so ridiculously low out of caution and a spindle speed of only 733 rpm so that even when I finally got it to work I did not even realize it, as you could not see movement with the naked eye. I thought the program froze,apparently it was only waiting for the tooling to catch up! That is why I did not get an error message, as there was none. Only when I flipped over to the position sensor screen is when I finally realized it was working!

I'm so new to this that I don't even know..... that I didn't know..... but was exactly what I thought that I had no idea I was even looking for... One g code was all I needed! Thank you for your help.

What year is this machine ? The OT can run anything my HAAS runs. I load through the RS232

This is part of a program running in my TC-2 today. IT starts at the mouth of a bore faces the front turns a .02 rad and turns a 1.693 Dia .891 long. Note the machine does not use a G54 work offset it uses the work shift in the work offset page.

Set your work shift well away from the chuck until you know what you are doing and be careful.

%
O0600
(PROGRAM NAME - 16006)

G20
(TOOL - 9 OFFSET - 9)
(OD 55 DEG RIGHT INSERT - DNMG-432)
G0 T0909
M8
G97 S2000 M03
G0 X.662 Z.1
G50 S2000
G96 S970
G99 G1 Z0. F.003
X1.637
G3 X1.693 Z-.028 R.028
G1 Z-.088
Z-.891
X1.8344 Z-.861
M9
G00 X6.0 Z6.0 M05
T0900
M30
%

Good luck

Ron

Dupa3872 said:

This is part of a program running in my TC-2 today. IT starts at the mouth of a bore faces the front turns a .02 rad and turns a 1.693 Dia .891 long. Note the machine does not use a G54 work offset it uses the work shift in the work offset page.

Set your work shift well away from the chuck until you know what you are doing and be careful.

%
O0600
(PROGRAM NAME - 16006)

G20
(TOOL - 9 OFFSET - 9)
(OD 55 DEG RIGHT INSERT - DNMG-432)
G0 T0909
M8
G97 S2000 M03
G0 X.662 Z.1
G50 S2000
G96 S970
G99 G1 Z0. F.003
X1.637
G3 X1.693 Z-.028 R.028
G1 Z-.088
Z-.891
X1.8344 Z-.861
M9
G00 X6.0 Z6.0 M05
T0900
M30
%

Good luck

Ron

Click to expand...

That code will not produce .02 radius on outer corner if DNMG-432 insert is being used (.0312 TNR), it cuts air around corner and leaves it sharp, likely with burr hanging over face of the part.

Try this:
Diameter programming, cutter comp included in tool path.
----

G0 X.662 Z.1
G1 Z0. F.003
X1.5906
G3 X1.693 Z-.0512 R.0512
G1 Z-.891

----

Go to youtube, put in my name, Heinz Putz, and see a CNC DVD called CNC Partmaking, that will teach you exactly what to do, how to write the program, how to put it into the control, all of it.
Its a condensed , free version of all my CNC DVDs, so learn all you can.
On my website: www.doccnc.com. see more examples, also a description of all my CNC DVDs.
Write back with any questions: Heinz.

VicTLG said:

That code will not produce .02 radius on outer corner if DNMG-432 insert is being used (.0312 TNR), it cuts air around corner and leaves it sharp, likely with burr hanging over face of the part.

Try this:
Diameter programming, cutter comp included in tool path.
----

G0 X.662 Z.1
G1 Z0. F.003
X1.5906
G3 X1.693 Z-.0512 R.0512
G1 Z-.891

----

Click to expand...

I should have edited that insert out of the code my tool library is not correct I change the insert information on the fly. My insert has a .008 Rad. I was trying to get him going with some code, Nice catch though you got it right.

Thanks

Ron

Dupa3872 said:

What year is this machine ? The OT can run anything my HAAS runs. I load through the RS232

Click to expand...

It is a 1990 machine. I purchased it from a dealer in Michigan. I was told that something was wrong with the input/output card, and I would only be able to use it as a manual input machine. I know less than nothing about programming these and am on a very steep learning curve right now. Basically I've got an encyclopedia size stack of manuals, that might as well be written in French, and what seems like a really good book on programming. If I were to replace that card, could I set it up to connect to a laptop computer through that rs232 port? And what program would I need to use on that computer that could write and send the data over?

Typo in tool type on sample code, got it,....

I see a lot of posts having to do with "Help, I have no experience, what is wrong with ...? "how do I ....." ...??????

Hire is how, Google "CNC programming manuals", list pops up, pay attention to links starting with "PDF", download one and start reading on subject,....... get understanding of the theory as a starting point, all free of charge.

Another problem: same but different.

yardbird said:

Where to begin? Never tried running canned cycles from MDI. Feed override on zero? G99 G1 X/Z Feed won't move unless the spindle is turning, try G98 G1 X/Z Feed?

Instead of a thousand questions from the group maybe you can post the exact code your trying to run for us to see. Most likely someone will get you going

Brent

Click to expand...

I was doing really well since you helped me solve the mystery freeze up, I used the g98 code and am running most of the program, but now I'm having another similar issue. I'm almost at end of this program I am writing. I've built a bar feeder and am attempting to shut off the spindle, open the jaws, pull material, close jaws. Once I shut off the spindle and use a g00 command to locate my bar feeder I cannot use a g01 command to get my bar feeder to "slowly lock in" where I need it. If I skip this one line the jaws will open, then program sticks again when I need to move the bar. Skip that line and the jaws close fine also. Here is the end of the program.

g00 x3.5 (works)
g00 z4.5 (works)
m05 (works)
g04 u2.5 (works)
m09 (works)
t0200 (works tool change)
m05 g00 x0 z0 (works)
g00 z-3.975 (works)
g98 (was not in there originally, put in program trying to get it to work)
g01 x.075 f200 (will not move, stops working)
m10 g04 u2.5 (will work only if I skip previous line)
g01 z.250 f600 (will not move, stops working)
m11 g04 u2.5 (will work only if I skip previous line)
g01 x0.0 f300 (if I remember this is stuck also)
g00 z4.5
g00 x3.5