Which Post Procesor?

Moderators: TomKerekes, dynomotion

Post Reply
men8ifr
Posts: 19
Joined: Tue Mar 26, 2019 2:30 pm

Which Post Procesor?

Post by men8ifr » Wed Nov 15, 2023 12:45 pm

Using Fusion 360 and it is for the custom/homemade 3 axis milling machine in my signature.

Also I would be interested in a 4th axis later down the line - can Fusion do that (and a post processor) on a hobby license?
My Set-up
PM30 Milling Machine - 3 axis
Kflop
Leadshine copy closed loop 'hybrid' stepper drivers similar to HBS86
Nema 34 6A 8.5Nm motors with encoder (encoder connects to stepper driver)
Fusion 360 Software

User avatar
TomKerekes
Posts: 2604
Joined: Mon Dec 04, 2017 1:49 am

Re: Which Post Procesor?

Post by TomKerekes » Wed Nov 15, 2023 6:26 pm

You might check the wiki.
Regards,

Tom Kerekes
Dynomotion, Inc.

Alexanders
Posts: 33
Joined: Wed May 03, 2023 12:54 am

Re: Which Post Procesor?

Post by Alexanders » Mon Mar 04, 2024 8:43 am

I have exactly the same question, but about a SolidCAM postprocessor for a three-axis milling machine (later 3+1).
If there is no exact answer, then please advise which machines the Kflop G-code system looks like? (Fanuc/ Siemens/ Heidenhain/ Haas/....)

User avatar
TomKerekes
Posts: 2604
Joined: Mon Dec 04, 2017 1:49 am

Re: Which Post Procesor?

Post by TomKerekes » Mon Mar 04, 2024 5:21 pm

Hi Alexanders,

I don't see anything for SolidCam posted. If you come up with something please add it to the wiki.

KMotion's interpreter is derived from the EMC public domain Interpreter as was Mach3 and LinuxCNC which was originally derived from Fanuc documentation.
Regards,

Tom Kerekes
Dynomotion, Inc.

Alexanders
Posts: 33
Joined: Wed May 03, 2023 12:54 am

Re: Which Post Procesor?

Post by Alexanders » Wed Jun 19, 2024 12:05 pm

I'm dealing with the Fanuc postprocessor for SolidCAM. And there was a question.
SolidCAM offers compact tool inlet/outlet trajectories in the form of arcs with simultaneous application of tool radius compensation.
Example of an inlet/outlet trajectory:
N124 G02 G42 D1 X18. Y0. I0. J3.6
However, when specifying in KMotionCNC, the diameter of the tool more than specified in "ARC beg/ end radius Tol", an error occurs when the starting and ending points of the arc do not match.

As a result, there is no way to compensate for the radius of the tool when moving in an arc. Only if you increase it significantly parameter "ARC beg/ end radius Tol", which is not the right way, as I understand it.

Linear inlet/outlet tool trajectories do not cause problems in KMotionCNC, but it is not as compact as arcs.

User avatar
TomKerekes
Posts: 2604
Joined: Mon Dec 04, 2017 1:49 am

Re: Which Post Procesor?

Post by TomKerekes » Wed Jun 19, 2024 9:13 pm

Hi Alexanders,

Could you post a complete example? That line of GCode is not helpful without knowing the initial conditions. What is the tool diameter? What Units?

What Version of Software are you using?

Have you read Internal/concave Path Tool Radius Compensation Example G41/G42

Are you using EMC or Fanuc Entry Styles?
Regards,

Tom Kerekes
Dynomotion, Inc.

Alexanders
Posts: 33
Joined: Wed May 03, 2023 12:54 am

Re: Which Post Procesor?

Post by Alexanders » Thu Jun 20, 2024 12:19 pm

I'll try to explain it differently.
Initial conditions:
- KMotion5.3.1
- FANUC_COMP_ENTRY_STYLE
- Units mm
- ARC beg/ end radius Tol = 0.0007 inch

A simple code example:
N1 G54 G17 G40
N2 G1 X0 Y0 F500
N3 G3 G42 D1 X10 Y0 I5 J0
N4 M30
Executing line N3 will cause an error "Radius to end of arc differs from radius to start". This error will occur in cases where D1 greater or equal to "ARC beg/ end radius Tol" X 2. (Of course, with the condition of recalculation of units.)

User avatar
TomKerekes
Posts: 2604
Joined: Mon Dec 04, 2017 1:49 am

Re: Which Post Procesor?

Post by TomKerekes » Thu Jun 20, 2024 10:25 pm

Hi Alexanders,

Did you read the article of the link I posted?

Its not clear what you are trying to do. The GCode you provided is a CCW arc. Uncompensated would be this:

Arc.png
Arc.png (8.96 KiB) Viewed 66 times

You didn't tell us the Tool Diameter. G42 will compensate to the right of contour. So I expect you desire the tool to pass over the outside of the arc.

The G42 GCode Block should contain an entry linear move to the beginning of the contour over which the compensation will be applied. The actual linear move will be to where the tool is tangent to the specified contour. Note the entry move is delayed because the direction of the contour needs to be known to determine the tangent position.

Shown here is a 2mm Tool placed tangent to the beginning of the contour you specified.


Tangent.png
Tangent.png (9.22 KiB) Viewed 66 times

The next question would be the tool starting point before moving to be tangent to the contour? The starting point can be anywhere including the start of the contour. But that wouldn't normally make sense as it would gouge the contour that we are trying to create. Normally it would be away from the contour and in the direction of the contour such as shown here X=-2 Y=3:

EntryMove.png

The corresponding GCode would be:

Code: Select all

G40
N1 G21 G54 G17
N2 G0 X-2 Y3 (Starting Point)
N3 G1 G42 D1 X0 Y0 F500  (Entry move to beginning of contour)
N4 G3 X10 Y0 I5 J0 (First compensated contour motion)
N5 M30

Resulting in this tool path:

Compensated.png
Compensated.png (8.62 KiB) Viewed 66 times
HTH
Regards,

Tom Kerekes
Dynomotion, Inc.

Alexanders
Posts: 33
Joined: Wed May 03, 2023 12:54 am

Re: Which Post Procesor?

Post by Alexanders » Thu Jun 20, 2024 11:23 pm

TomKerekes wrote:
Thu Jun 20, 2024 10:25 pm
Did you read the article of the link I posted?
I have read this material several times. The Fanuc pictures are very unclear there. The description of the graph points is not clear. However, I understand how to apply the cutter radius compensation.
TomKerekes wrote:
Thu Jun 20, 2024 10:25 pm
So I expect you desire the tool to pass over the outside of the arc.
I made a little mistake writing G42, there should be G41. The cutter should not have gone beyond the arc. But it was just an example causing an error. This is the trajectory that you call "entry move to beginning of contour". SolidCAM suggests doing this in the form of an arc, without linear motion. It's more compact this way.

It is difficult for me to write and read in English, it is not my native language. Therefore, I cannot write much and there may be inaccuracies of perception. Thank you for taking the time to answer my questions!

User avatar
TomKerekes
Posts: 2604
Joined: Mon Dec 04, 2017 1:49 am

Re: Which Post Procesor?

Post by TomKerekes » Fri Jun 21, 2024 12:21 am

The link has an example of an internal contour with an arc to the cutting contour if needed.

HelixBoreTopView.png
HelixBoreTopView.png (8.88 KiB) Viewed 63 times
Regards,

Tom Kerekes
Dynomotion, Inc.

Post Reply