I think my CNC Head and Table are not coordinating with each other

[vaishnavinambiarr]

I'm running a 5-axis machine with XYZ on the head and A (rotating around Y-Axis) and B (rotating around Z-axis).

I'm using an edited version of a FANUC post as attached below to give an output based on this. However, although the code is generated correctly (toolpath generated in Mach3Mill seems accurate) and the zeroing in has been done perfectly, the head is cutting at a position slightly off in terms of X,Y coordinates with respect to the position of the part on the table. 

What could be the problem?

Attached: edited post-processor

[engineguy]

@vaishnavinambiarr 

Without seeing your Fusion file it may be that you have selected a Model Box Point in Fusion that is a litle different than the Stock Box Point that you are selecting at the CNC Machine.

To upload an f3d file go to :-

File > Export > Select f3d format > Save to a location on your computer > Then attach to your reply.

[serge.quiblier]

Hi  

the issue will most likely due to TCP support on the controller or no support.

By default, the Fanuc post is using TCP a.k.a Tool Control Point.

This is the command G43.4 for activating and the more generic G49 for cancellation.

When the controller does not support TCP (or RTCP, or TCPM depending on the builders), then the coordinates need to be recalculated when the rotary axes are moving.

The post needs to be set differently, and the eventual pivot distance of the machine must be passed to the createAxis function call to inform the post engine for the calculation.

Cheers

______________________________________________________________

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

[vaishnavinambiarr]

@engineguy 

Hey, thanks for replying!

I've attached the f3d file below. I'd edited the post-processor slightly to give B and C outputs as A and B instead, as the CNC responds to those axes. I am attaching that as well.

I am zero-ing in the CNC on the little + on the bridge-like structure with the three holes, which has also been set as my origin here.

[vaishnavinambiarr]

@serge.quiblier 

Hey, thanks for replying!

Could you please tell me how I can change the TCP settings for the post? I have attached the used post for reference.  I'd edited the post-processor slightly to give B and C outputs as A and B respectively instead, as the CNC responds to those axes. 

[serge.quiblier]

Hi @vaishnavinambiarr 

it will be done in two locations, the first one is the axis definition:

var cAxis = createAxis({coordinate:1, table:true, axis:[0, 0, 1], range:[-360, 360], cyclic:true, offset:[0, 0, 0], tcp:false});

And the second one is the angle optimization settings

optimizeMachineAngles2(0); // TCP mode

must be changed to another settings.

optimizeMachineAngles2(OPTIMIZE_TABLE); // for non RTCP table table machine

another settings possible, but with the same result if the definition is correctly telling us it's a table table machine

optimizeMachineAngles2(OPTIMIZE_AXIS); // for non RTCP , checking the setting for each axis and configuration

If there is no rotary axis on the head, it should be sufficient. (or else we would have to either drive a virtual tooltip, and or compensate the tool lenght in calculation)

But if, as the subject imply, there is an axis on the head, then the axis definition is incorrect (one of the axis must be table:false)

Regards.

______________________________________________________________

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

[vaishnavinambiarr]

@serge.quiblier 

Hi, thanks for replying!

I made the mentioned changes to the post-processor code.

For 

optimizeMachineAngles2(OPTIMIZE_TABLE); // for non RTCP table table machine

 the output code had an error and was not generated.

For

optimizeMachineAngles2(OPTIMIZE_AXIS); // for non RTCP , checking the setting for each axis and configuration

A code was generated but the output was similar to the one before, where the tool head (XYZ) is cutting at a different location in the XY plane, instead of the part.

It does look like it has something to do with TCP, but this did not work☹️

What else could I try?

[engineguy]

@vaishnavinambiarr 

Hmmm, if the code is correct then it should cut correctly at the machine, you say that it is out of position in the X and Y axes so can you just program of a simple square and see how far off the cut is at the mchine?

I have done this here and the code is correct so assuming that your Stock setup in Fusion is the same as the Stock setup at the machine the only other thing I can think of that would make the cut out of position might be the Calibration of the CNC in Mach3, has this been done properly ??

I know you said that the machine had been set to Zero is that what you meant? It has been Calibrated using the facility shown below ?? Found under the Settings tab in Mach3.