[phillip]

On my final pass making a hole 1.370 in dia, .500 deep, bit starts to run backwards and takes out a .030 gouge out of the side.
Running mach3 taig mill. help!

Here is the last bit of g-code:

N2290 G03 X7.2625 Y-2.1893 I0.0088 J0.075
N2295 X7.1443 Y-2.2892 I-0.2583 J0.1856
N2300 G02 X7.2171 Y-2.2806 I0.0487 J-0.0992
N2305 G03 X7.2869 Y-2.2583 I0.0159 J0.0709
N2310 X7.1717 Y-2.3452 I-0.2827 J0.2547
N2315 G02 X7.2427 Y-2.3392 I0.0433 J-0.0882
N2320 G03 X7.3119 Y-2.3222 I0.02 J0.0679
N2325 X7.1992 Y-2.4013 I-0.3078 J0.3186
N2330 G02 X7.269 Y-2.397 I0.0401 J-0.0817
N2335 G03 X7.3375 Y-2.3835 I0.0227 J0.0658
N2340 X7.2267 Y-2.4574 I-0.3333 J0.3799
N2345 G02 X7.2955 Y-2.4543 I0.0379 J-0.0774
N2350 G03 X7.3635 Y-2.4433 I0.0245 J0.0641
N2355 X7.3635 Y-2.4433 I-0.3593 J0.4397
N2360 G00 Z1.0
(=============================================)
(====== Tool No 2 = 3/16 flat end mill 2 flu-finish)
(====== Tool No 2 diam. = 0.1875)
(..... Segment = SIDE1)
(..... Operation = FINISH SIDE)
(=============================================)
N2395 T2 M6
N2400 G43 H2 Z1.0
N2405 S2500 M08
N2410G00 X7.3635 Y-2.4433 Z1.0 F1.8
N2415 Z0.1
N2420 G01 Z-0.5 F1.8
N2425 G41 X7.4127 Y-2.5346 F3.6 D02
N2430 G03 X7.4777 Y-2.4986 I-0.0355 J0.1409 F1.8
N2435 X7.4777 Y-2.4986 I-0.4735 J0.495 F3.11
N2440 X7.5542 Y-2.4119 I-0.4735 J0.495
N2445 X7.5818 Y-2.3429 I-0.1167 J0.0866 F1.8
N2450 G01 G40 X7.4851 Y-2.3054 F3.6
N2455 G00 Z1.0
N2460 G91 Z0 M09
N2465 G40 G49 G17 G80 G61 G70 G90 (Inch mode & Exact Stop)
N2470 M91001
N2475 M30
(----------------------------------------------------------------------)
(------------------------------ E N D -----------------------------)
(----------------------------------------------------------------------)
%

If anyone could help I would appreciate it.

[Geof]

I have not analysed your code but I suggest you look at the move associated with the G40 cancelling tool compensation. If this move is not large enough or in the correct direction I have found sometimes the machine will move in a direction I did not expect.

[bborb]

I agree with Geof
Seems like your tool approach and exit (lead-in and lead-out) from the large circle aren't large enough, can't handle the tool compensation mathematically.

[phillip]

so do I need to change bit overlap % to more. What would I look for to make it larger? Im using featurecam.
Thanks so much for your help.

[phillip]

Ok, In featurecam in the rough pass i set the finish allowance from .o26 to
.010 and now it makes the final pass. At the very end though It still wants to
make a small move in the x dir and takes a small chunk out of the stock.
But the final part is the corect size at least:rainfro:
Thanks so much for all the help.

[ger21]

No, what Geof is saying is that when the comp is turned off with G40, the tool is not far enough clear of the part.

[bborb]

At this point its not a Mach Software problem, its a FeatureCam problem.
Try posting this in the FeatureCAM CAD/CAM forum and you'll get quicker/better responses.
HTH

[Geof]

I was wrong; it is not the G40 move.

I crunched the numbers for the last move and the straight line distance is greater than the tool radius so there is no problem here.

So I copied that segment of code, ran it in my simulator and took some screen shots.

First picture (Phillip1.jpg) is the full circle with the little glitch at the start and end point for the circle.

Second picture (Phillip2.jpg) is just the starting moves. The tool has just moved to line N2435 from N2430 and you can see how it was inside the circle at lin N2430.

Third picture (Phillip3.jpg) shows the circle stopped part way round you can see the glitch at the beginning.

Trying to find the error by looking at the wrong end of the horse doesn't help.

Sorry I gave you a wrong lead.

[phillip]

I will post on the futurecam site and see why it is generating such code.
Thanks so much for pointing me in the right direction.