Contact Point - Milling 4 Axis 1

[laurent90]

Hello

Here is my first post in this website.

On one machine 4 axis contineous, I must manufacture a cylinder with a milling cutter 2 sizes. I have a problem with the contact point. It is always in the center of my tool. And in my new process, i would like that the reference axis either out of alignment .

I don't know how to configure this switch into my operation : variable_contour. ( is this a good method ? )

find attached with post a screenprint to understand my problem. ( TC8.5/NX 7.5 )

Thanks for your help.

Laurent

 

[markrief]

You should be able to get this be setting a small lead angle on the tool axis.

Mark Rief
NX CAM Customer Success
Siemens PLM Software

 

[laurent90]

I would like that my tool stays normal to the guide.

 

[markrief]

In NX 9.0.3 and newer, in Surface Contouring, Curve/Point drive method, this parameter is available - it is called "Tool Contact Shift"

Mark Rief
NX CAM Customer Success
Siemens PLM Software

 

[laurent90]

Thank , for your help. Can you tell me if is it possible to configure this method for a surface ? (helical milling )

Laurent

 

[markrief]

If you are using streamline, you need to do this with tool axis lead and/or tilt.

Mark Rief
NX CAM Customer Success
Siemens PLM Software

 

[laurent90]

Hello

I can't reproduce the same result with function streamline ( than surface method ) and i don't find the parameters : lead or tilt . I attached with this post a file *.prt to have a better understanding of my problem.

 

[markrief]

Change your tool axis from "Normal to Part" to "Relative to Part" and enter a small Lead Angle. I tried .5 degrees.

Mark Rief
NX CAM Customer Success
Siemens PLM Software

 

[laurent90]

Thanks a lot for your Help. I have configured my operation with your informations and it's OK.

Laurent