G'day.
I've written a post processor for our mill at work, it uses an Anilam 6000M controller. Just running through some tests, and everything is pretty hunky-dory so far. Getting a weird output when using a 2d Chamfer operation though, it tried to perform G1 moves with a 0 feedrate:
N65 X39.501 Y-21.85 Z15 N70 Z5 N75 G1 Z2 F0 N80 Z-2 F167 N85 Y-21.25 F0 N90 X0 F500 N95 G17 G2 X-1.25 Y-20 I0 J1.25 N100 G1 Y0 N105 G2 X0 Y1.25 I1.25 J0 N110 G1 X40 N115 G2 X41.25 Y0 I0 J-1.25 N120 G1 Y-20 N125 G2 X40 Y-21.25 I-1.25 J0 N130 G1 X39.501 N135 Y-21.85 F0 N140 G0 Z15
I've written the post from scratch, as it was a great learning exercise, so I figured it must be something I've done wrong. To check, I use the RS274d post, and the generic Fanuc post, both of which do the same thing:
RS274D:
N65 G0 X39.501 Y-21.85 N70 G43 Z15 H2 N75 Z5 N80 G1 Z2 F0 N85 Z-2 F166.7 N90 Y-21.25 F0 N95 X0 F500 N100 G2 X-1.25 Y-20 J1.25 N105 G1 Y0 N110 G2 X0 Y1.25 I1.25 N115 G1 X40 N120 G2 X41.25 Y0 J-1.25 N125 G1 Y-20 N130 G2 X40 Y-21.25 I-1.25 N135 G1 X39.501 N140 Y-21.85 F0 N145 G0 Z15
Generic Fanuc:
N55 G00 X39.501 Y-21.85 N60 G43 Z15. H02 N65 G00 Z5. N70 G01 Z2. F0. N75 Z-2. F167. N80 Y-21.25 F0.
N85 X0. F500. N90 G02 X-1.25 Y-20. J1.25 N95 G01 Y0. N100 G02 X0. Y1.25 I1.25 N105 G01 X40. N110 G02 X41.25 Y0. J-1.25 N115 G01 Y-20. N120 G02 X40. Y-21.25 I-1.25 N125 G01 X39.501 N130 Y-21.85 F0. N135 G00 Z15.
The Anilam control errors out and stops when it gets to a feed line with a rate of zero, less than ideal. I can manually edit the program of course, but I'd love to have it working directly from post. I've double checked the tool setup, and feedrates are definitely set. I tried it with a sample tool instead of one from my library, and had the same result. I tried different lead-in and lead-out radii, still no dice. I also tried setting it to always fast-feed instead of rapid, and still no change!'
Searches on the forum / google didnt lead to any results either.
Can anyone help me out?
Cheers.
Zac.
@zac.perston wrote:
G'day.
I've written a post processor for our mill at work, it uses an Anilam 6000M controller. Just running through some tests, and everything is pretty hunky-dory so far. Getting a weird output when using a 2d Chamfer operation though, it tried to perform G1 moves with a 0 feedrate:
N65 X39.501 Y-21.85 Z15 N70 Z5 N75 G1 Z2 F0 N80 Z-2 F167 N85 Y-21.25 F0 N90 X0 F500 N95 G17 G2 X-1.25 Y-20 I0 J1.25 N100 G1 Y0 N105 G2 X0 Y1.25 I1.25 J0 N110 G1 X40 N115 G2 X41.25 Y0 I0 J-1.25 N120 G1 Y-20 N125 G2 X40 Y-21.25 I-1.25 J0 N130 G1 X39.501 N135 Y-21.85 F0 N140 G0 Z15I've written the post from scratch, as it was a great learning exercise, so I figured it must be something I've done wrong. To check, I use the RS274d post, and the generic Fanuc post, both of which do the same thing:
RS274D:
N65 G0 X39.501 Y-21.85 N70 G43 Z15 H2 N75 Z5 N80 G1 Z2 F0 N85 Z-2 F166.7 N90 Y-21.25 F0 N95 X0 F500 N100 G2 X-1.25 Y-20 J1.25 N105 G1 Y0 N110 G2 X0 Y1.25 I1.25 N115 G1 X40 N120 G2 X41.25 Y0 J-1.25 N125 G1 Y-20 N130 G2 X40 Y-21.25 I-1.25 N135 G1 X39.501 N140 Y-21.85 F0 N145 G0 Z15Generic Fanuc:
N55 G00 X39.501 Y-21.85 N60 G43 Z15. H02 N65 G00 Z5. N70 G01 Z2. F0. N75 Z-2. F167. N80 Y-21.25 F0.
N85 X0. F500. N90 G02 X-1.25 Y-20. J1.25 N95 G01 Y0. N100 G02 X0. Y1.25 I1.25 N105 G01 X40. N110 G02 X41.25 Y0. J-1.25 N115 G01 Y-20. N120 G02 X40. Y-21.25 I-1.25 N125 G01 X39.501 N130 Y-21.85 F0. N135 G00 Z15.The Anilam control errors out and stops when it gets to a feed line with a rate of zero, less than ideal. I can manually edit the program of course, but I'd love to have it working directly from post. I've double checked the tool setup, and feedrates are definitely set. I tried it with a sample tool instead of one from my library, and had the same result. I tried different lead-in and lead-out radii, still no dice. I also tried setting it to always fast-feed instead of rapid, and still no change!'
Searches on the forum / google didnt lead to any results either.
Can anyone help me out?
Cheers.
Zac.
Are you using a drill for the chamfering?
Laurens Wijnschenk
3DTechDraw
AutoDesk CAM user & Post editor.
René for Legend.
Ahhh, legend. Inputting the spot drill measurements as a chamfer mill instead seems to make it all work. Is there any reason for that? It'd be nice to be able to just have one tool setup in my library, instead of having the spot drill in there twice, but with the same tool offset number specified.
Cheers.
Zac.
Change the tool definition to a Chamfer Mill to fix the feed issue. There is supposed to be a temporary fix coming soon with a more comprehensive fix in the March update. I'm afraid I don't know what those fixes are to be, but I have asked that question here: https://forums.autodesk.com/t5/computer-aided-machining-cam/fusion-360-posting-f0/td-p/6867387
I allways use spot-drill 90 degrees for champfering (from 2D contour feature) on all my machines without any problems.
@zeljnik2014 wrote:
I allways use spot-drill 90 degrees for champfering (from 2D contour feature) on all my machines without any problems.
HSMWorks has been unaffected by this so far. If you're using Fusion 360 or Inventor HSM I suggest trying it again.