Post processor mangling the toolpaths?

[tluliak]

I am using the UCCNC post processor on a servo converted Bridgeport BOSS machine. 2D toolpaths machine beautifully, but 3D paths - despite looking perfect in Fusion - look like I carved the part with a Dremel tool in one hand and an Espresso in the other. Some areas of the part are machining perfectly where others are faceted both with and without arc fitting enabled. I've tried the part using a few different operation types and though the patterns change they continue to facet with curved areas cut with straight paths. The endmill may be slightly large for the curves. The convex portions appear perfectly machined but the concave portions appear gouged and faceted. 

Where should I begin troubleshooting this kind of problem?

[Richard.stubley]

Hi @tluliak,

One thing I would start with is some basic machine tests with cylinders, The G code should give nice curves and hopefully test the basics.

Have you done any backlash checks on the machine? 

If not these are really easy to do, hand jog your machine with a DTI or lever clock in one direction then with the smallest resolution on your jog move in the opposite direction and see at one point do you register movement. If you move 0.005mm before the DTI shows movement then that is your backlash. 

There are also lots of NC viewers out there, it will at least point you in the right direction. If you see those odd marks in the NC viewer then the chances are its CAM / Post, if the NC code looks nice and smooth then its more likely Controller / Machine

[Anonymous]

Looks like you have slop in your axis'.  Try and slow down your feed rate.  Does your controller support G61/G64 commands? If it is stopping for a microsecond at each point rather than just continuing through them, it could result in poor finish.   

[tluliak]

Excellent advice. This machine has been up and running for awhile and has completed quite a few projects successfully, but to be absolutely certain I went through the entire machine and tightened each belt to the point that just touching the belt is felt as the servo holding position with a slight buzz. Having completed that process on all three axes, I mounted a .0005" lever indicator and verified backlash. I then set backlash compensation for each axis until both even and odd number of movements in opposing directions always landed precisely on the indicator and always returned to the start position dead on. No axis required more than .0002" of compensation to meet this standard. 

Having completed alignment and being certain that the machine was configured as precisely as I can measure, I ran the part again. 

Without a doubt the resolution of the part improved - unfortunately only insofar as making the edges of the facets that much sharper. I've verified the toolpaths as generated by loading the Gcode result into NCPlot, zooming in and verifying that the toolpaths were indeed smooth arcs. The Gcode is being rendered with minute G3 arcs over ~10* of a circle connected by ~80* worth of G1 lines. It doesn't seem like the gcode does anything funny where the part is gouged, but the part gets those gouge marks at the same place in the part on every run.

I'll take this and the generated code over to the UCCNC forum and see if they can make any recommendations because I can't see anything in the generated code that should lead to the poor surface finish I'm getting on this particular part. It's confounding for sure. 

Thanks for your help 🙂 

[tluliak]

@Anonymous -

 During machine travel over the gouged areas it does dither through the path despite following the path smoothly elsewhere. The machine is commanded to making the gouging cuts - but it only does this on one particular part of the path and for no reason that is obvious to me.

Supported codes include G61, but the post isn't including G61/G63 codes in the output. The controller has lookahead to smooth out small linear movements as well as stopless backlash compensation with comp accel and in general the machine path is very smooth. Except, of course, where it isn't  😄

[daniel_lyall]

Try running an engrave toolpath with 10 letters and measure the start and finish position if an axis is out there is the problem.

A engrave toolpath is a good way to find if a machine can handle 3 axis moves with its tinny moves.

[tluliak · Accepted solution]

I feel pretty good that the machine is doing precisely what it's told.

https://photos.app.goo.gl/GAVUoHaeyFVZPCnr6

^ This is a video of the controller display moving the tool through what should be a perfectly smooth curve. If you watch closely you can see the tool icon moving in a faceted circular pattern that is drawn with great precision in the part. The tool is moving to a peak, then drawing a straight line path to the next peak. That's seen in the finish below.

But I don't see anything in the toolpath rendering that seems that abruptly pointed

After running more than 20,000 small moves, it then finishes the two upper triangular areas. If the machine was off at the end of the very long toolpath, then the registration of those small triangles would be off from their correct locations. 

Extreme close-up

So that triangular patch is the last portion of a 24k line file. That's an awful lot of small moves, and yet that's among the best surface finish on the part and appears to be located exactly where it should be on the part's surface.

Would that not meet the spirit of your engraving test?

Regardless, this doesn't seem to be a fault of Fusion or the post-processor in any way that is obvious to me, so I'll continue troubleshooting this problem from the controller side. Maybe there is an answer there.

Thank you all for your help, and have a great weekend.

[daniel_lyall]

Can you post a model with this problem To do this Go to File -> Export and save as a .F3D Archive File and attach it to your next post, if you can not post the file you can PM it to me or say in your next post you can not post the file and one of the Guys that do NDA work will help.
And can you put the post-processor in a zip file and attach that as well. 

[tluliak]

Both attached, thanks.

The machining operations include a roughing of the contour with Pocket2 followed by Steep and Shallow, both using the same ball-nose endmill. Following a tool change the rest of the part would be finished with a 2D contour but I've never bothered to run the part that far for obvious reasons.

[tluliak]

UCCNC includes two modes of operation for the machine; Exact Stop and Constant Velocity mode. The machine has been set in Exact Stop mode for all machining operations. After setting the linear and corner error settings dealing with the CV mode from .03" to .0005" the problem appears corrected. These settings should have no effect in ES mode, but the resulting part seems to indicate they may.

[tluliak]

Success. Thanks for everyone that helped!