C axis Milling G112 Haas - Help

[ThickChips]

Hello all,
I am new to G112. All the milling we've done prior has been relatively simple things and I haven't had a need to use the code. Until recently, a milling toolpath was more complex. The C-axis began to "stutter" severely. And my first thought was "OK I need G112". Sure, the arc filtering / tolerance could be it. But i tried increasing values and what-not to no avail. 

G112 worked on said job, no more axis "stutter". But had a bunch of bugs. Did weird random moves at start and end of toolpath (g41 Comp reasons? nah dont think so). 

Long story short, I'm back today on G112 and pretty lost. Its a simple face-contour. I keep getting  "INVALID CODE IN G112" (see attachments). It does a strange X-axis move when plunging to depth (G1 X5.545 Z-.231 C0. F3.5), where the tool moves in-ward (x negative).

The generic post has radial values instead of diametric. 
Perhaps I do not need G112, Non-g112 looks so much simpler. Less code and easier to understand, but the C-axis stutter is killing me. 

Would someone mind taking a look at my files and telling me if they see anything obviously wrong, before I continue to troubleshoot? 
I appreciate any insight you can offer.

Machine is:  New HAAS ST35LY

Thanks
 

G112_TEST.mcam G112_SAMPLE.nc

[TFarrell9]

I'm unfamiliar with Haas, but the post for our Doosan (fanuc) posted the same code where you're getting the "invalid code" and we've had no issues with interpolation on that machine, including using wear comp. Of course I'd have to run this code say for sure, but it looks fine to me.

As for the first line of your code following the G112 command (where you get a bad plunge), try giving "clearance" a value and see if that corrects that issue, because it does on my post.

I'd personally never mill any contour on a lathe without G107/G112.

 

Edit: It ran fine on the Doosan other than where cutter comp is enabled due to lack of lead-in/lead-out.

[ThickChips]

@TFarrell9

Thanks a lot for taking time to look at my program. That's comforting to know that the output looks good. I'm going to add a clearance value and re-test.

Reason for no leadin/leadout is nature of the part and cutter I'm using. In short, adding these would cut portions of the finished part. But anyway thats why

 

I didn't know about G112 until about 3 months ago. At my last job, we used a fanuc machine and did some C Axis things when they came through the door but I don't recall ever using it. Besides "translating the coordinates" to milling, what does G112 actually do? I think I once read that it also converts the proper IPM feed rate of the C Axis, whereas omitting the G112, the C axis doesn't know how to rotate at a correct federated. Curious on learning more.

 

Thanks again I'll report back with my results 

[TFarrell9]

@ThickChips

Like you said, it's really for controlling the commanded feed rates for the C-axis by essentially mimicking a Y-axis. Without the use of G112 (polar coordinate interpolation), the motion and coordinates will still be correct, but the feed rates will be all over the place. Cutting in a circle would be somewhat okay (bad feed, but constant), but if you interpolate off-center, it will be excessively fast in one part of the cut and excessively slow in another.

[ThickChips]

Hi,

I tested another toolpath using leadin/out.

Result is the same. "INVALID CODE IN G112"

It does this on the first G1 move after G112 is called. I deleted the line and continued. Then it alarm the same o. The G41 line.

 

Edit:  Update. I believe the issue is that C-axis commands are being posted erroneously, as the post doesn't work. It should be outputting Y Axis moves when converted with G112. I am using the generic post now.

 

The problem is "EXCESSIVE AXIS SPEED OR ACCELERATION" when trying to process the G1 line directly after G112. 

 

Going to call Haas and get answers. Will report back. 

 

[AMCNitro]

1 hour ago, ThickChips said:

Hi,

I tested another toolpath using leadin/out.

Result is the same. "INVALID CODE IN G112"

It does this on the first G1 move after G112 is called. I deleted the line and continued. Then it alarm the same o. The G41 line.

 

Edit:  Update. I believe the issue is that C-axis commands are being posted erroneously, as the post doesn't work. It should be outputting Y Axis moves when converted with G112. I am using the generic post now.

 

The problem is "EXCESSIVE AXIS SPEED OR ACCELERATION" when trying to process the G1 line directly after G112. 

 

Going to call Haas and get answers. Will report back. 

 

Don't have a lot of experience C axis, but if its giving alarms on the G41 line make sure you have a straight lead in BEFORE the radius lead in.  It's a problem with Haas, it needs the straight lead in, then the radius, .005 is enough.

[gcode]

What post are you using?

There is an excellent post available on the Mastercam Tech exchange

It should  be plug and play for your machine

[ThickChips]

Hello all, 

Returning with more information after troubleshooting. 

 

@gcode I am using the generic post. It doesn't support a true Y axis machine, so requires zero-ing out the Y Axis before G112 is called. Other than that, it's working.

My custom post for the machine does not even work with G112, as it outputs C Axis moves, rather than converting to Y Axis. So there was that confusion.

With all that said, the generic post is working except for one problem. The machine is throwing an "excessive Axis speed or acceleration" alarm during the G41 comp lines. I now remember how I fixed this 3 weeks ago.

I made each G41 line have a slow feed (3.0 ipm).  This prevented the alarm and allowed me to get a good working toolpath. 

I'm also going to avoid "C Axis Face Contour" and just stick to milling type toolpaths. Had problems adjusting leadin/out inside mcam with C Axis toolpath. Side question:  now that I have G112 figured out, can I use virtually any of the basic milling toolpaths to my hearts content? Or is there some that don't work well with C Axis G112?

 

Thanks for the help and discussion.

[gcode]

1 hour ago, ThickChips said:

My custom post for the machine does not even work with G112, as it outputs C Axis moves, rather than converting to Y Axis. So there was that confusion.

did you look in misc intergers?

Our Postability posts have a switch to turn it off or on

 

[ThickChips]

3 hours ago, gcode said:

did you look in misc intergers?

Our Postability posts have a switch to turn it off or on

 

 

I'll have to check tomorrow. Interesting.

If it does have it, I guess "Face/OD Interpolation" is quite a vague description. Thus, I would've never even considered it.  "Polar Conversion", "Convert C to Y", "Convert Polar Coordinates" would've all been much better names, if that's in fact what the switch does. I'll check.

 

Thanks 

[ThickChips]

Update:

 

The Haas alarm I was receiving about excessive acceleration was due to a C Axis offset in the work offset menu. According to Haas this is a bug they have fixed in a software patch for the machine and are going to send a tech out to Update it.

 

Thanks for everyone's help.