C-Axis cross contour depths

[Brian Pallas]

Hello,

 

I just started a new job and they have Mori NL-2500SY Lathes.  I have never programmed the live tools before.  Doing a milling path down the length of a tube, and in MCAM the depth is right, and it verifies correctly.  When I post the code though the X dimension is doubled, like the depth of the cut is being read as a radius and is then being converted into a diameter in the code.  They have a post for the the NL-2500's that they have been using, but from my understanding the programs have always been cut and pasted together from the MCAM output, and manually change some things to what they are supposed to be.  I also downloaded the mplmaster post and machine.  I am getting the same output with the X value depth for the milling for both posts (their original NL-2500 post and the mplmaster post).

 

Does anyone know what I am doing wrong? Or what I need to change to get the correct output?  

 

I tried to attach a Zip 2 Go and the MCAM file but both were to big to attach, even though the sample program is two lines and one milling op.

 

I have X7.

 

Thanks,

[Guest]

My immediate guess is they don't really have a post, they have something they hacked together that they use.....

 

The fact that you say they hack and paste programs together, I believe supports the notion....

 

Bottom line, you may not be doing anything wrong but likely have a post that isn't configured properly

 

Those machines can have many options and a purchased post is almost always the best way to go....

[Colin Gilchrist]

Does the machine use Diameter coordinates for the Turning paths, and only use Radius for the Milling paths? The output (Radius vs. Diameter) is usually set as an option inside the post. It will depend on who wrote your post, and how they set it up, to know which value to change.

 

Try creating a Zip file with your MCX-7 file, MD/CD/PST, and attach that to your post. Someone will be able to give you a hand in editing the setting.

[Colin Gilchrist]

I have a post for a Mori NLX at home. I can check that output against your MCX-7 file, once you upload it here, and I get home this evening...

[Brian Pallas]

Thanks, I would definitely appreciate the help.

 

 When I tried attaching the Zip2Go onto the original post there was a message saying that the file attachement was to large.  Zip2Go is 506kb, and the max is 398.3kb.

 

Is there an upload section for files?  

 

Or I could email it if that works for you?

 

Thanks.

 

[Brian Pallas]

Oops.  Actually the post and everything works fine.  I confused myself with expecting to see the radius value as the X value for the milling - but we're on a lathe so it is doubled to the diameter.  Duh:)!  No harm no foul - thanks for the offers of help.

[Brian Pallas]

Allright I have a couple more newbie questions

 

I have an axial live tool on the subspindle.  For the planes I have the WCS at top, and then copied the left plane and moved the zero, and used that for the T/C planes.  I used a 2d mill contour path, with a C axis sub.  The toolpath looks good in backplot and verify.  But in the code I have an M14 for the rotary tool spindle on instead of an M13, and also a G42 instead of the G41.  In backplot I verified I am climb milling, so I should have a G41, it seems like.  

 

Are my planes setup wrong, or how should I set up the planes?  Something doesn't seem quite right.

 

Also, I programmed a linear feed of 29 IPM, but the feed output in the code is F2000. for the cutting moves with the C axis.  How are the C axis feed rates figured?  Any insight into that would be appreciated.  

 

Thanks.

[bd41612]

On some machines, even though you are working on the sub spindle, the turret is still driven as if your facing the main.  That being said G2, G3 and G41, G42, X, I, etc are swapped. 

 

Try using CView utility.  Go to Toolpaths, Mill, then over to CView utility.  Set up your axis config for the next toolpath.  Go back to Toolpaths, Mill, over to the desired toolpath you wish to use.  This method seems very stable and you don't have to worry about what planes you are using.

 

Once you have done this, if you have any other issues with outputs being backwards, wrong etc. the try this:

Look for the following in your post:

 

#Machining position turret/spindle settings

Read the directions for the 17 digit string definition.  Go to #Top turret/Right spindle setting (I'm assuming we are talking the top turret) set each bit accordingly.  That should fix it for good.

[Brian Pallas]

I'll try that and take a look.

 

Thanks!

[bd41612]

No problem

[mirek1017]

"

Also, I programmed a linear feed of 29 IPM, but the feed output in the code is F2000. for the cutting moves with the C axis"

 

WHAT ABOUT THIS , QUESTION  BECAUSE SOMETIMES RUNS 4 AXIS  IN AND HAVE THE SAME PROBLEM???

[bd41612]

 

Check control definition

[Brian Pallas]

I used the Cview utility and reposted and got the M14 and G42.  I am assuming that the output is correct.  We will find out!  Thanks for introducing me to the Cview utility.

It does make sense that if you rotate your axial tool 180 for the subspindle that the live tool motor would need to spin the opposite direction.

 

I made the change in the control definition for the rotary feed rates, but am still getting the F2000. feed rate.  Do you know what else could be causing that, or maybe a switch in the post that the control definition didn't actually change?  

 

Thanks for the help.

[bd41612]

F2000 degrees per minute.  Should work unless you have the G93 inverse feed time option from FANUC.  What type of tool path is this?

[Brian Pallas]

It is a 2d contour path, with C axis for the rotation type.  I was wondering if the control interprets the F when there C present differently?  Is it degrees per minute?

 

I changed the feedrate in MCAM to 60IPM, and reposted to see what would change.  And in the code it is the same F2000. feedrate.

 

Ah, then I slowed it down and then the feedrates changed, so I am guessing that the rotary feedrate is limited to 2000 degrees per minute?

 

Are feed rates for C axis lathes with milling normally in degrees per minute?

[bd41612]

Look for these in your Machine Specific Settings:

 

#C axis and Index switches

 

maxfrdeg    : 2000  #Limit for feed in deg/min

 

Every one I've worked on was degrees per minute...

[Brian Pallas]

Cool, thanks for the info.

 

I appreciate your help!

[Brian Pallas]

So, if you have the ability to use either the C axis or Y axis, which one do you think is better to use? 

[Brian Pallas]

Well, I got the post changed to the Pick off cut off almost all like I would like.  There the section with the cutoff tool positioning that I can't find/figure out.  I would like to pre- posistion the cutoff tool at X8. all the time and at the Z cutoff posistion, then do all the M-codes for part eject and spindle sync, grab the part in the main spindle, cutoff, retract to X8., then part off detect, de-sync the spindles, and send the subspindle home, then move the turret to the G53 tool change position.

 

I attached my POCO code from MCAM with notes on where I wanted to change and was wondering if anyone could point me where to look in the post.

 

Thanks.

 

POCO SAMPLE CODE.txt