Why does the code output from Inventor CAM not display the tool compensation code G41 or G41?

[long0212le]

When I use "Post Process" to export the code to the Fan UC machine, but the output program does not display the left tool compensation or right tool compensation command, how do I open it or is it inherently absent? ?

[serge.quiblier · Accepted solution]

Hello @long0212le 

what did you set as compensation type in the operation?

In computer won't generate G41 or G42, recalculating the toolpath instead.

See the explanations in the tooltip framed in orange.

It's probably a incorrect setting in your toolpath, as the current Fanuc library post does not have any problem outputting cutter compensation codes.

Regards

______________________________________________________________

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

[long0212le]

Thank you for your answer

I choose "In Computer"
for example when i change different tool diameter, i just need to change in tool compensation setting without editing the program, is there any way to do that without having to change the program?

[CNC_Lee]

@long0212le 

You will need to use the "In Control" compensation type to allow for this functionality.

[long0212le]

I have a lot of work to do, should I set them all to "In Control"?

[serge.quiblier]

Hello @long0212le 

yes, you need to either set to In Control, and depending on the machine configuration the tool table will contains either 2, or 4 values. (Except if it's a very old one, then it will contain only 1 value)

You have data for the length and the diameter.

When using only 2 values, it's the real-life dimension of the tool.

When using 4 values, you can have the theoretical length and diameter, plus a wear value.

If you are using wear, we will consider that the theoretical dimension is zero, and only using a wear offset on the machine, but still using G41/G42.

So, you have to alter all the operations, on which cutter compensation need to be activated.

You may want to use the Compare and Edit dialog for mass editing.

Just select several operations in the tree view, and right click to access the menu option Compare and Edit.

The toolpaths will be displayed in a table, and you will be able to see several operations at the same time.

Have a nice day.

Regards

______________________________________________________________

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

[CNC_Lee]

@long0212le 

Yes, you should set all operations to use "in Control" compensation.
* Be aware that adaptive toolpaths do not allow for any cutter compensation.

[long0212le]

@CNC_Lee  AND @serge.quiblier 

Thanks for your answers.
But I can't find "Compensation Type" in my settings. I am using the function "Adaptive of 3D Milling" and "Adaptive of 2D Milling". Is it limited and only usable in certain functions?
Sorry for asking so many "silly" things, I'm just starting out with InventorCAM so there's a lot I don't know.

[serge.quiblier · Accepted solution]

Hello @long0212le 

Cutter compensation is only available on the finishing toolpaths.

It is not avialable on roughing toolpaths.

2D Adaptative and 3DAdapatative are both roughing operations.

Regards