Sign in to follow this  
Corey Hampshire

Planes when Milling in a Lathe/Mill Turn

Recommended Posts

I am working in our mill turn and ran into an issue yesterday. I am doing some milling and  I have my part oriented in Mastercam (2022) just like I do when I program our Vertical Mill. Top Plane is looking down from the spindle onto the part. When I posted  the code (Post from In House Solutions) the part is off 90°.It was like it needed oriented so that you are looking at the part through the door. I figured this out pretty quickly and switched my WCS for my ops to Front. This fixed my issue.

My question is why? Why is it off 90°? Is there something that is different when Milling in a lathe? This is in a Mori 2500MT. This isn't in the Mastercam MT software for the record, they do not support this machine, so it is just Milling and Lathe combined in the standard Mastercam suite.

Second question, when I go to do 5 axis tool paths will I run into issues since my planes are not Top/Top/Top and are now Front/Front/Front? I thought I read on here somewhere that Mastercam made it so you can use whatever planes you need to for 5 axis now. I was taught that it had to be Top/Top/Top and the post would handle it.

Share this post


Link to post
Share on other sites
1 hour ago, Corey Hampshire said:

I am working in our mill turn and ran into an issue yesterday. I am doing some milling and  I have my part oriented in Mastercam (2022) just like I do when I program our Vertical Mill. Top Plane is looking down from the spindle onto the part. When I posted  the code (Post from In House Solutions) the part is off 90°.It was like it needed oriented so that you are looking at the part through the door. I figured this out pretty quickly and switched my WCS for my ops to Front. This fixed my issue.

My question is why? Why is it off 90°? Is there something that is different when Milling in a lathe? This is in a Mori 2500MT. This isn't in the Mastercam MT software for the record, they do not support this machine, so it is just Milling and Lathe combined in the standard Mastercam suite.

Second question, when I go to do 5 axis tool paths will I run into issues since my planes are not Top/Top/Top and are now Front/Front/Front? I thought I read on here somewhere that Mastercam made it so you can use whatever planes you need to for 5 axis now. I was taught that it had to be Top/Top/Top and the post would handle it.

C Axis Zero is the issue and Back Plane is what Mastercam normally considers C0 for Mill/Turn programming using a MP Post. Your machine must have C0 facing to the front of the machine and In-House configured the post to support that process for getting the output to work correctly. The issues you run into are the Polar Coordinate output when things are not aligned like Mastercam needs. In-House is aware of this issue and has configured the post to give you an output to support all the needs the machine has. Sometimes little unforeseen things will pop up and that is when you get a hold of your dealer or them and make them aware and they address them.

Yes Front/Front/Front for all the 5 Axis will be no issue these kind of issues were address many versions ago. Again where the post does all the heavy lifting.

  • Thanks 1

Share this post


Link to post
Share on other sites
15 hours ago, Corey Hampshire said:

I am working in our mill turn and ran into an issue yesterday. I

Have you played with the C axis utility? I got used to it, but the thing I like is that if you give it a C angle it will show you the cutter orientation. i used the CNC Multi axis lathe post as a base.

Share this post


Link to post
Share on other sites

Have you tried orientating your part and setting your WCS on the D+Z+ plane.  Then depending on the Mill ops you can either select the Right Cplane (axial) or the Back Cplane (Radial)

image.thumb.png.b7756d7c834ded89b6e0b6ccd51512c2.png

  • Like 1

Share this post


Link to post
Share on other sites

Live tooling facing the Main spindle ...right side plane... C0 is at 3 o'clock

Live tooling pointed to the chip pan, cross drilling...Back side plane ... from the back side view, hold the ALT key down,

press the arrow key down rotates C axis 5 degrees with every depress of the the arrow key.....

 

 

  • Like 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us