Post processor for siemens 840D Mill give me problem

[peter.andersson_Sunnerbo]

Hi!

When posting a file with Siemens 840D Post processor Mill and trying to run nc code in the machine (EMCO Concept Mill 250) it runs into trouble. If I am using "smooth" lead in and lead out where there is a horizontal and vertical radius on the approach the machine stops and complains about the "wrong plane selected". In nc code, I can see it shifts from G17 to ex. G19. it seems it can´t handle that. Back in Fusion and get rid of ALL such moves, and the code works fine. Sad though to have to do that with every toolpath it applies to. This machine is used in a school and that makes it even worse.

I didn´t mention that sometimes I got nc-code faults like "wrong circle center point" or "wrong circle endpoint" or something like that, I don´t know exactly what it says but I understand the meaning of it. When switching planes the center and end coordinates become for example in X/Z-plane or Y/Z-plane

I would be happy if I could get some help with this problem.

Regards /Peter

[serge.quiblier]

Hello @peter.andersson_Sunnerbo 

If you edit your post and look near the start you will find a varaible defintion:

allowedCircularPlanes = undefined;

When the variable is equal to undefined, arc interpolation in all 3 planes are allowed (XY, YZ, XZ)

If equal to 0, no arcs will be generated, It will be linearized for all planes.

If you want to keep arcs in a single plane, then it should be the XY plane.

So, you can change the variable to that setting:

allowedCircularPlanes = (1 << PLANE_XY)

Regards

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[peter.andersson_Sunnerbo]

Hi!

Sorry for my late reply!

Thanks a lot for this suggestion of a solution.  But, there is always a but;-)

Is there any way to overcome this problem on the "machine side"? Those toolpaths work really well with for example the HAAS VF2 we also used. I mean the Siemens 840D should be capable to solve this and do as I (or Fusion360) want.

Regards /Peter