Hello! I want to work with a Cylinder as Clearance Option:
My part looks like this, I have four holes on a cylindric surface, I'm working with holemaking:
The part is clamped in the middle of a roundtable. Unfortunatelly the Post interpretes the clearance-pathes. I don't want this:
This is from a standard-post from NX11.0.2
Am I wrong with my idea, only to output the Z-axis but not the toolpathes, which really does the round-table? This toolpathes should end in a B-axis command in post.
ofcourse code you showed is strange and funny, but maybe it is working.
- clearence paths are single lines, accept it like a spline, not rotary move
- if your machine works with TRAORI you should get XYZ (B) C for example.
and then the new plane has to be set (cycle 800) , *
N720 X112. Y71.225 Z36.427 A-62.875 C+0.
N730 X112. Y73.037 Z32.644 A-65.881 C+0.
N740 X112. Y74.647 Z28.771 A-68.888 C+0.
N750 X112. Y76.053 Z24.818 A-71.895 C+0.
N760 X112. Y77.249 Z20.798 A-74.901 C+0.
N770 X112. Y78.233 Z16.72 A-77.908 C+0.
with this logic any of clearence geometry will be succes.
(if your mcs is in the axis rotation it is complicated to do such "rotary" move in one block in TRAORI mode with CAM. Stuff I told you is universal - doesnt matter where you put mcs/part on the table)
- If your machine has not Traori etc, you can get output with rotating table - multiple C (you can avoid multiple C output with combine rotary cmd) - I think this is not your case.
For me any of template posts does not works good, you need to edit it, and maybe you wont bend it like you want because of deeper code logic. hard work.
Better is to start with generic template (almost empty) and build your own logic. hard work too but you can get beautiful result.
(* check cycle 800 par 57, I dont agree with that in case multiple using in operation.)
Cylinder Clearance option will not get you a B rotation in this case.
Please take a look at tool path list, there should be a bounch of rapid motions between two holes like below.
NX CAM tool path is machine independent. Imagine a head-head 5-axis machine is used to cut this part. Rapid motion on cylinder surface has to be interpolated to a few small linear motions as listed tool path.
To get a single rapid motion between holes, please use other options of NCM like "Automatic Plane" which will result to a direct rapid move from one hole to another.
To get rid of strange cycle800 output for each rapid position, please switch below option "Use Standard Path between Rotary Motion" to "ON" in Post Configurator.