Community
HSM Post Processor Forum
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

2D Chamfer, giving 0 Feedrate?

8 REPLIES 8
Reply
Message 1 of 9
zac.perston
314 Views, 8 Replies

2D Chamfer, giving 0 Feedrate?

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.

8 REPLIES 8
Message 2 of 9


@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 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.


Are you using a drill for the chamfering?

 

Laurens Wijnschenk
3DTechDraw

AutoDesk CAM user & Post editor.
René for Legend.


Message 3 of 9

G'day Laurens.

 

Yes, a spot-drill.

Message 4 of 9
zac.perston
in reply to: zac.perston

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.

Message 5 of 9
Steinwerks
in reply to: zac.perston

It was recently broken in Fusion 360 as part of the January 19 update. I have heard it has been this way in Inventor HSM too but I have not tried it yet. Which software are you using?
Neal Stein



New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Message 6 of 9
zac.perston
in reply to: Steinwerks

Fusion360.

Message 7 of 9
Steinwerks
in reply to: zac.perston

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

Neal Stein



New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
Message 8 of 9
zeljnik2014
in reply to: zac.perston

I allways use spot-drill 90 degrees for champfering (from 2D contour feature) on all my machines without any problems.

Message 9 of 9
Steinwerks
in reply to: zeljnik2014


@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.

Neal Stein



New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report