Need Help with WinCNC Post Processor driving custom CNC setup

[Anonymous]

We have a hand built CNC driven by WinCNC, and have been creating tool paths in Surfcam2000.

I was able to get a partially working Post file exported from Fusion using the link in this discussion:

https://camforum.autodesk.com/index.php?topic=6359.0

I get no errors, but the origin point is not in the correct place when I try to run the file. The spindle drives over several inches from where I set 0,0, but then seems to follow all the paths correctly.

Additionally, my post file has no M-codes to turn on/off the spindle.

I'm including the Fusion file, the post file from Fusion, and a comparable post file from Surfcam.

Is it possible to examine the Surfcam version to modify the Fusion post processor?

Thank you!

Jason

[HughesTooling]

I helped someone else out in this thread. Try the post in this link, seemed to work for them.

Mark

[HughesTooling]

---

@Anonymous wrote:

I get no errors, but the origin point is not in the correct place when I try to run the file. The spindle drives over several inches from where I set 0,0, but then seems to follow all the paths correctly.

Thank you!

Jason

---

Are you setting up and using the same work offset in the CAM and on the machine, for example using G54 on both?

Mark

[bob.schultz]

Hello Jason,

Here is a version of the wincnc post that closely matches your output from Surfcam.  I left the circular interpolation (G3) in it since you did not ask for it to be removed, even though the Surfcam post does not use it.  I also made the G0,G1,G3 modal so that they are not output on every line.

As far as the machine moving over a few inches prior to machining, I don't see anything wrong with the numbers output by the post.  The [G54] block is now output, but it is a comment and I don't know if your control does anything with this.  All I can say is to try this post and see if the machine still performs in the same way.

The accompanying advice and or non-standard post processor is provided as-is and without warranty of any kind, and usage is at the user’s own risk. 

[HughesTooling]

@bob.schultz just thought I'd let you know that wincnc only supports G2\G3 in the XY plane, haven't test your post so you may already know this.

Mark

[bob.schultz]

@HughesTooling Thanks Mark,

I have added the limitation for circular interpolation in the XY-plane only in the attachment to this post.  I did not know of the limitation and as an established post, I was surprised that this check was not already there.

The accompanying advice and or non-standard post processor is provided as-is and without warranty of any kind, and usage is at the user’s own risk.

[Anonymous]

Thank you Mark and Bob!

I will test the new settings this week and let you know how it goes!

[Anonymous]

Hi Bob and Mark,

Thanks so much for your help! I've tried with the new configuration. When I simulate in WinCNC it gives "multiple commands" error.

Here is the specific error:

Error, X1.0238 Y1.4874 Z2.1287 I-0.0099 J-0.2373, Line 14

I got this error initially with the built-in WinCNC settings, which led me to try the version with G0, etc. at the beginning of each line, even though our Surfcam output doesn't have it. That version seemed to work, except my zero coordinates when cutting where not where I zero'd the machine.

[bob.schultz]

Hello Jason,

Here is a version of the post with the interpolation codes on every block.  From what you mentioned, this should be acceptable to your control.

The accompanying advice and or non-standard post processor is provided as-is and without warranty of any kind, and usage is at the user’s own risk.

[Anonymous]

It now errors here:

Error, G0 G43 Z2.6, Line 10

However, in my haste, I neglected to test the file for CAMaster_wincnc_m3x.cps Mark sent from this forum post.

With some slight modification, this one seems to be working. I deleted the T2 (gave syntax error) and M3 codes, and changed the final M5 to M6 in a text editor. I will test further with some additional part files.

[Anonymous]

Correction, this was the link.

CAMaster_wincnc_m3xa.cps ‏25 KB

[HughesTooling]

---

@Anonymous wrote:

I deleted the T2 (gave syntax error) 

---

Have you got a tool library on your control and are the tools and length offsets set?

---

@Anonymous wrote:

and M3 codes, and changed the final M5 to M6 in a text editor. I will test further with some additional part files.

---

In you first post you said "Additionally, my post file has no M-codes to turn on/off the spindle." did this mean you don't need spindle control in your post processor or that it was missing from your posted G code?

Mark

[bob.schultz · Accepted solution]

Hello Jason,

Here is an updated version of the wincnc_a.cps post.  I looked at the CAMaster_wincnc_m3xa.cps post and it is setup to have a tool changer, while the wincnc_a.cps post already has an option to disable the tool changer, plus work has  been done to match the output that you are looking for.  Please give this version a try and see if it works.

One difference I noticed between the two posts is that the surfcam post outputs the G54 in a comment and the m3xa post does not.  Which is your requirement here?  I left it in a comment for now and if the machine does not position correctly, you can simply remove it from the comment and try it.  I also noticed that the S-codes are commented in the surfcam and wincnc_a post, but not in the m3xa post.  Again, which syntax do you require?

Thanks.

The accompanying advice and or non-standard post processor is provided as-is and without warranty of any kind, and usage is at the user’s own risk.

[Anonymous]

---

@HughesTooling wrote:

---

@Anonymous wrote:

I deleted the T2 (gave syntax error) 

---

Have you got a tool library on your control and are the tools and length offsets set?

No tool library, all tools are installed manually and manually set the Z height each time.

---

@Anonymous wrote:

and M3 codes, and changed the final M5 to M6 in a text editor. I will test further with some additional part files.

---

In you first post you said "Additionally, my post file has no M-codes to turn on/off the spindle." did this mean you don't need spindle control in your post processor or that it was missing from your posted G code?

The codes were missing in that posted code. I need M5 to turn on, M6 to turn off the spindle.

[Anonymous]

Bob,

This worked like a charm on my test part!! I'll try some more complex parts and see if any issues come up.

Thank you!!!!!