5 Axis Fanuc Generic post question: Primary axis does not reset on Top Plane

[Giang-TT]

Hello, 

I'm working on the Fanuc 5-axis generic post to use it on an rotary table BC (C is the primary axis and B is the secondary axis).

I have 2 toolpaths: #1 and #2 using the same tool:

#1 toolpath: is a 2D toolpath, takes place on a user-defined tool plane - which requires both B anc C axis to rotate (e.g. B30. C30.)

#2 toolpath: is a 2D toolpath on the Top Plane.

When I post only #2 toolpath: I get B0 & C0 output on my NC program.

But when I post both #1 & #2 toolpaths, after finished #1 toolpath on the user defined plane (e.g. B30. C30.), the tool goes back to the Top Plane for #2 toolpath. But only the B axis changes back to 0, the C axis is unchanged (still kept at C30.). So the part is no longer aligned along the X and Y axis, and the 2D contour along the edges now take place on both X and Y (instead of X or Y). That is my problem, I'm not sure if can call it a problem.

My question is: Is the any quick way, or is there a "switch" that allows us to force the primary axis to reset (C0.) if the toolpath is using Top Plane? 

Thanks for reading.

 

[crazy^millman]

Force A tool change between each operation.

[Aaron Eberhard]

One way that would absolutely work would be to put a manual entry op between the two operations, that was just G0 C0. B0. to index it that way. 

Without your specific post it's hard to test if this would work, but you could try playing with these misc values

You'd edit the second op and set these to a value.   What they're supposed to do is tell the post processor "start thinking about this toolpath as if the B & C are already at X degrees.   In your case, you can try putting a 1 in both of them and see if that adjusts your output.    It may not be hooked up correctly for your use case, though.

I've used it when I wanted it to do the opposite of whatever it was doing, i.e., it wants to go C+90, when I wanted it to go to C-270.

[Craig-B]

If you are using an updated copy of the Generic Fanuc 5X Mill from CNC Software, it has new switch that might help if you set it to yes$.
use_tool_plane_as_bias : no$  # Use the tool plane XY orientation as a bias when tool is vertical?
                                                     # When set to 'yes$' the operations' tool plane will be use to calculate
                                                      # the primary axis angle.

Link to Tech Exchange:
https://community.mastercam.com/TechExchange/Parts/3544#partTitle

[MIL-TFP-41]

There is a switch for that in the generic 5 axis post.

frc_cinit    : 1

 

[Giang-TT]

Thank you all for the replies, I tried them all and here is some updates:

 

On 1/17/2024 at 9:46 PM, crazy^millman said:

Force A tool change between each operation.

Yes, this helps - but it also outputs some tool change codes in the program, which I want to hide.

 

On 1/17/2024 at 11:11 PM, Aaron Eberhard said:

One way that would absolutely work would be to put a manual entry op between the two operations, that was just G0 C0. B0. to index it that way. 

Without your specific post it's hard to test if this would work, but you could try playing with these misc values

You'd edit the second op and set these to a value.   What they're supposed to do is tell the post processor "start thinking about this toolpath as if the B & C are already at X degrees.   In your case, you can try putting a 1 in both of them and see if that adjusts your output.    It may not be hooked up correctly for your use case, though.

I've used it when I wanted it to do the opposite of whatever it was doing, i.e., it wants to go C+90, when I wanted it to go to C-270.

I tried this, it didn't help in this case

 

On 1/25/2024 at 2:32 AM, Craig-B said:

If you are using an updated copy of the Generic Fanuc 5X Mill from CNC Software, it has new switch that might help if you set it to yes$.
use_tool_plane_as_bias : no$  # Use the tool plane XY orientation as a bias when tool is vertical?
                                                     # When set to 'yes$' the operations' tool plane will be use to calculate
                                                      # the primary axis angle.

Link to Tech Exchange:
https://community.mastercam.com/TechExchange/Parts/3544#partTitle

I'm using an older version of the generic 5X post so it doesn't come with this switch, I will try out this new one, it looks giving me what I want. 

 

 

On 1/27/2024 at 12:59 AM, MIL-TFP-41 said:

There is a switch for that in the generic 5 axis post.

frc_cinit    : 1

 

I tried this switch, it didn't work with a null tool change, it only works when I have a real tool change.

[crazy^millman]

Will have to get a custom post from your dealer. The generic is just that not customized for each users wants. It is made to make good code with some understanding you get what you get.