Lately I've been machining some bigger parts on my 5 axis where the travel is skewed. The machine has 16" of x travel and 20" of y travel with the trunion located at a0c0.
I want to rotate the part so I can work in the upper Y quadrant, machine, rotate 90, machine, rotate 90, machine.
I can not for the life of me get my post to let me do this. It always leaves me at a0c0.
The tool axis is up so there is theortically 4 solutions to do the position that it could use....
Not sure what you mean by "Which tool do you address?"
Original tool path. MCS location a0 c0. Very hard to manage engage/retract with 2" shell mill since part is very close to the X axis limits.
So I create a new MCS A0 C90
Exactly what I want it to do. Machine using the Y axis travels instead of X since I have more room there.
However post defaults it back to A0C0 . Notice CYCLE800 output code and X/Y cordinates. I've tried to force it with a UDE Rotate but it still puts out the cycle800 a0c0 rotation .
I can't be sure of this because I do not see your Geometry tree but consider this in case it applies to your situation.
There should be a "parent" MCS to your rotated MCS (the "child"). The parent will likely be parallel to the Machine Tool base coordinate system. The child will have the same origin and be rotated the way you want it. The parent will be "Local" with "Fixture Offset" # <your choice>. the child will be "Local" with "CSYS Rotion" and the "Fixture Offset" will be the same number as in the parent. This may help your cause but without the whole story I'm just speculating.
Maybe try the Rotate UDE?
CAxis/Absolute/90 (or whatever)/Reference only
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled
I also ran into this. Our machine tools by default don't move rotary axes when cycle800 rotation is only about Z axis, only coordinate rotation is performed (I guess because technically tool axis is already correct?). I ended up using TRAORI to get around this. I programmed everything as if was at C0 using one MCS but broke tool paths into quadrants. Then made a UDE that inserted the C move and TRAORI. Might not be the approach you are looking for but it worked great for me when I was machining large parts and dealing with this same situation.
@Dstryr: you adress the postprocessor. This is what I meant with "tool". As @Not-Yet-Retired said, check the parent and child MCS settings. In regular the ootb postprocessor should output the angle, when there is a rotation only around Z axis.
@smoffat: you mentioned: "Our machine tools by default don't move rotary axes when cycle800 rotation is only about Z axis" I´m interested on that comment. Do you mean the real machine tool or the cse modeled machine tools? I ask because there was problem in the CSE-Driver (S840D & TNC) in that case. I´ve fixed it for NX1003.
I was talking about the physical machine tool. There is a command to change this behavior on our machine:
This was a while ago so I don't remember if I tried this in CSE but I think I did. We are using NX 18.104.22.168 so I guess it's good I went with TRAORI. Machine behavior and simulation match.
Played around with this a little more as curiosity got the better of me. Our post is developed from sim09 post and will output a cycle800 rotation just around Z but CSE simulation won't rotate the C axis. I think this is why I went the route that I did with TRAORI. Geometry tree setup is as follows:
MCS_MILL: MAIN, 0
G54: LOCAL, FIXTURE OFFSET, 1
G54_C180: LOCAL, CSYS ROTATION, 1