5 axis post processor for Mach3 for DIY CNC machine.

[Poduhvat1]

We just got custom made 5 axis CNC machine. I got machine kinematics in place and simulation for the test part is working properly. The problem is the post processor for Mach3.  I have managed using instructions from this forum to create rudimentary  5 axis post from generic Fanuc using Autodesk Manufacturing Post Processor Utility but this somwhat works without RTCP while with RTCP if creates Gcode inconsistent with simulation.

The main difference is the Y coordinates with and without RTCP option post file. Without RTCP there is no fluent simultaneous movement of the machine it just rotates B axis for a long time before starting to use Z with minuscule movement while with RTCP gcode due to inadequate y distance it tool collides with B axis table.

The goal is to have truly simultaneous 5 axis movement as in simulation. 

And this can be done by optimizing post for Mach3. Machine has manual tool change. 

I will post .cut file with some .pmoptz  post files with RTCP and without.

Can anyone help with adequate 5 axis simultaneous Mach3 postprocesor for this machine?

[Anonymous]

If this error occurs again with the macro, then please type to Powermill command window:  print=$SimuLogFile

[Poduhvat1]

This is what I got. I might not doing something right.

[Anonymous]

If this error

occurs again with the macro, then please type right after to Powermill command window:  print=$SimuLogFile

[Poduhvat1]

These are the mistake and debug file.

[Anonymous]

The new version of macro  no longer writes a file, but writes the result (up to 200 lines) to the Powermill command window. A known flaw is that Lead-in / out is not displayed in full detail. 

"flip-flop a-axis for 180 degrees(-90 to +90)"  - I avoid this by having a separate machine model and postprocessor for each of the three options: Such as A [-120 -> 0], A [0 -> 30], A [-120 -> +30]. But I use them mainly for 3 + 2 machining.

[Poduhvat1]

It seems that it is matching 

the difference is in the z but I guess this is because of the tool gauge height.

By the way I noticed in post processor in rapid moves there is no B Machine is this correct?

Also I noticed interesting thing when doing simulation in PM when starting from setup it shows flip-flops in A axis

video

While when the simulation is run from nc there is no flip-flopping video . Also I noticed and this probably due to bad tool-path setting the program did not detected collision in sim even though it should have as it seems that tool is going trough the model video.                       

[Anonymous · Accepted solution]

The B axis missig in rapid moves my mistake. Please copy from Linear Moves. 

The Z difference in macro -please replace the "REAL ToolLengthComp=round(entity('tool',$TP.Tool.Name).Overhang,3)" line with this code:

 REAL ToolLengthComp=$TP.Tool.Overhang
   FOREACH H IN $TP.Tool.HolderSetValues {
      $ToolLengthComp=$ToolLengthComp+ $H.Length
   }

- Move Zmax for Tool change: https://forums.autodesk.com/t5/powermill-forum/5-axis-post-processor-for-mach3-for-diy-cnc-machine/m...

G53 Z417 (your Z axis range is  -158  -> +417 in .MTD)

[Anonymous]

I wonder if everything worked out. You are using your CNC 5 simultaneous shafts with mach3.

[Meysam_Ghorbani]

if you want i can make it for you

send message to me :

highcamgorup@gmail.com

see this clip :

https://www.aparat.com/v/woqGK

[Anonymous]

There were at least two problems with this solution:
1. It is much more sensitive to point distribution than controls using classic RTCP/TCPM. More points, finer tolerance -> slower execution and/or rougher surface.
2. I did not consider compensatory axis movements when determining the feedrate.

As far as I know it worked well on 3 + 2 toolpaths.

[Poduhvat1]

I did not have time to test this thoroughly. This is the latest files for set up. I guess there are still some set up to make it in full 5 axes simultaneous mode.

Some people send me the messages for the files as well as how to make the machine work in 5 axes. So I will post the latest files I have for the post-processor setup. To make it work if you have a 5 axis machine controlled with Mach3 you need to have 6axis screen which I will also share here.

I'm not sure that I will have time to fully work out this machine so I may sell it. If anyone interested let me know. It is new, unused full 5 axes with quite large work area.

[jlmccuan]

I'm ok on the screenset.  I appreciate the help.  Hopefully we can get up and running once we proof this out.

[nocturnalrccnc]

Can anyone help on loading this mtd file ? i get an error when trying to load it ?