G19 arcs on 3 axis Haas Vertival Mill

[Terrance Kell]

I have a Right angle Drive mounted on my mill that I need to use to thread mill in the Y,Z (g19) plane. How do I configure MasterCam to ouput Arc on on he G19 Plane

[jlw™]

this was just focussed about 3 threads down the list. go in your mach def and build an aggregate. program as normal.

[Terry Kell]

I don't see how this helps Me Mill  a thread parallel to the X Axis. I've taken code generated on the G17 Axis and modified it by hand but, it seems like there is a better way.

[jlw™]

There is a better way, go into the machine definition manager.  Add the aggregate head in the proper orientation then program the threaded hole as you normally would.

 

[jlw™]

Only difference is that my mill posts work with it.

[Terry Kell]

Perfect ! I think I'm on the correct path now thanks.

 

 Great Help !!!!!!!!!!!!!!!

[Colin Gilchrist]

All Mill Post Processors will support a Fixed Angle Head, by using the functions in the Machine and Control Definition files. You don't need to convert a Router post, unless you want a "programmable" rotary axis.

 

The coordinates get offset (rotated and translated) in the NCI data, before it goes to the Post Processor.

 

You just need to add and configure the Aggregate Head component in the Machine Definition, enable the checkbox in the Control Definition to translate the NCI coordinates, and program in either the Front, Right, Back, or Left Toolplane.

 

So to machine in YZ, using G19, you'd be programming from the Right Toolplane. On the Tool Parameters page of the Thread Milling dialog, you right-click and select "get angled head" to load the aggregate. Make sure the Filter is turned on, and that the G19 plane support is turned on, to make sure you get Arc output. (Also, support for XZ and YZ planes should be enabled in the Control Definition.)