Angle head programming on a 5-axis mill

[JTHESLAMMAN]

Hi everyone.

I am trying to figure out how to program a right-angle head for a umc-750. A lot of the info I can find seems to be for 3 axis machines. I defined the angle head as an aggerate to my tool spindle and added a tool. When I try to chain the geometry in the top view, I get errors and if I chain it in the front view the back plot looks good, but it wants to tilt my b axis to 90 degrees which is not what I want. I need to machine features within a cylinder from the top view. Any help would be greatly appreciated. I attached a file showing what I am trying to do.

Thanks

MOCK PROGRAM.mcam

[crazy^millman]

Who supplied the post? What process did they say needed to be used for using the RAH? If the post builder didn't build the post to support a RAH then you are not going to get it to work like you're thinking. Might can lie to it to get it to work, but if you want to go about it the correct way then need to have your post builder add this logic to the post.

[amw]

Dont mean to hijack the thread but can the Mill Default or MPmaster free posts be used with a RAH on a normal 3 axis mill?

[Chris In-House Solutions]

In-House Solutions sets up their posts with an Axis combination for RAH support.  If you got the post from another developer they might do it differently (misc. value perhaps)?  The post has the kinematics in it so adding an aggregate to your tool page wont work.  As said above you need likely need to add logic to the post to support RAH.

@amwno Mill Default and mpmaster do not support RAH's

[amw]

24 minutes ago, Chris In-House Solutions said:

In-House Solutions sets up their posts with an Axis combination for RAH support.  If you got the post from another developer they might do it differently (misc. value perhaps)?  The post has the kinematics in it so adding an aggregate to your tool page wont work.  As said above you need likely need to add logic to the post to support RAH.

@amwno Mill Default and mpmaster do not support RAH's

How about the IKE Posts? IKE Mill Fanuc? Are there any free posts that will run a RAH? 

This is not something we do much at all, but we are a job shop so never know when a job could come in. Even if the start/end code isnt right might still be able to work with it for an occasional job once every couple years or so. 

[crazy^millman]

3 hours ago, amw said:

Dont mean to hijack the thread but can the Mill Default or MPmaster free posts be used with a RAH on a normal 3 axis mill?

Generic Mastercam Posts will support them in a 3 axis process.

[#Rekd™]

I thought the router posts supported the aggregate heads? 

[Jake L]

My custom RAH post is made from the MPRouter post. Made the modifications a few months ago.

The tutorial videos I watched said the MPFan or MPMaster posts don't have the logic for RAH out of the box.

[nperry]

1 hour ago, Jake L said:

My custom RAH post is made from the MPRouter post. Made the modifications a few months ago.

The tutorial videos I watched said the MPFan or MPMaster posts don't have the logic for RAH out of the box.

The right angle head post we have is based on Fanuc 4x Router. 

OP - your setup looks mostly correct to me. When we use the right angle head to machine features on the 5 axis we need to plug in the B/C, A/B rotational values manually.

[Chris In-House Solutions]

19 hours ago, amw said:

How about the IKE Posts? IKE Mill Fanuc? Are there any free posts that will run a RAH? 

@amwOur free IKE posts do not support RAH heads out of the box.  If you want a quote please reach out to your Mastercam reseller for one.  

[JTHESLAMMAN]

Thanks for the input! After a lot of messing around I got the angle head to work the default mill post and my 5 axis post. The key piece of information I was missing was a setting in the control definition under work offsets called translate NCI coordinates to machine view with aggregate. Once selected Mastercam posted out the proper code.