variable contour, with 4-axis normal to part would be where I would start. Or you could use sequential mill.
You have drive geometry but no part geometry?
I believe there is "4 axis normal to drive" option
You could also try "Away from line" and pick a line at the (approx) centerline of your part.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled
I see 2 ways to cut this in 4 axis.
Do you want to cut with the side of the tool or the end of the tool?
For the end, surface contouring is the way. You need to decide on what tool axis you want (away from line should give you the smoothest rotary motion) and if you want to project the tool on to the the part (select PART), or just follow the drive geoometry blindly.
To use the side of the tool, solid profile 3D or zlevel should do it. You may need a start event to lock an axis, so the part spins around, instead of the tool going around the part.
Here's a sample.
Tool axis = 4-axis relative to part. This prevents rubing of material in the center fo the tool
The problem you have is caused by the tool size in comparison with the part size.
With a tool diameter much larger than the part details you will need to specify
part geometry. This way NX can project the drive points onto the part and prevent gauges.
Set the tool axis to 4-axis Normal or relative to part if you need 4-axis output.
I would suggest a smaller tool. If you look at the toolpath (verify) you see that the part doesn't have a greate finish, even the scallopheight was specified at .0001
A better solution -to my opinion- is to use a fixed contour operation to machine a section and use transform > instance to go around
Thank You for constant support to CNC Community.
I try to create Mill-Turn Post, but in order to do so, I need transfer some of the Variables from "Program Start Sequence"
in Lathe Post, to "Program Start Sequence" in Mill Post how I can efficiently do this?