NX6 CAM: difference between MCS, WCS & RCS

[dreamstar]

HI guys,

I'm still learning the manufacturing side of NX6, and making strong progress... thanks to all of you.

According to what I read, I believe the "part zero" is called MSC in NX6, am I correct?

Assuming that I am, I want to do the following:

I am trying to make 1 program with 3 different set-ups in it. I was hoping I could do that by including optional M1 stops between each set-up so the operator can rotate the part and relocate its zero. So I made this little block (attached) with 3 sides to machine. I created 3 different MSC of where I wanted the part-zero to be for each set-up. So far so good.
I have then proceeded to insert operations for each sides, and everything is still fine. When I verify each operation separetly and watch it really slowly, I see that the numbers are correct for my X,Y,Z axis. However, When I verify the entire program, the numbers are no longer correct. Instead of using each MSC as reference for its toolpaths, NX6 using the WSC instead of the MSC....

I was hoping one of you guys could open the file attached and look at what I am doing wrong.

Also I was also wondering this. I want to make 2 of the same part on the same blank... How do you do that with NX6? Right now I am using the autoblock but i cant find anything about creating your own blank and assigning it after..

THANK YOU ALL.
ps: What about RCS?
MAx

 

[wmalan]

Just off hand, under Details in the MCS menu set the first MCS to 1, the next to 2, and the last to 3. Make sure your post has the G - MCS_fixture_offset in your motion block set. It defaults to G53 so the 1,2, and 3 values increment it to G54,55, and 56. I never use RCS so...

--
Bill

 

[Jaydenn]

Have you actually post processed your file yet?
I cannot see your file as I only use NX5, but the way you describe your file should work without issue.

If you create a unique Machine Coordinate System(MCS) and put operations into that MCS, your output will be related to that MCS.

If you are refering to the built in NX verify command then pay no attention to the XYZ numbers displayed in the status bar. I tried this on a few of my programs and like you describe, as soon as the MCS changes, the numbers are no longer correct.

The bottom line is, you must post process your file and examine the output. I suspect you will get what you want once you do that.

As far as defining a blank, it is created in a similar fashion to the MCS.
You choose the "create geometry" in the manufacturing create toolbar, and select "workpiece". There you can choose part, blank, and check geometry. Any operations you create under that parent will use that blank.
Also, you can find the "blank" button inside many of the operations.
It's all covered in CAST.

 

[looslib]

WCS - Work Coordinate System
used for geometry construction

MCS - Machine Coordinate System
used for tool path construction

RCS - Reference Coordinate system
Used for machining transformations, it has been a while since I did NC on UG/NX - like 7 years.

AbsCS - Absolute Coordinate System
UG/NX center of its universe!

If you are having the operator rotate the part, then I would use a M00, not a M01 to stop the machine. You don'ty want the machine to go to the second face machining on the first face. Using the three MCSs for each face is correct, but the post will put in rotary moves to get to the next face. Use the RCS to redefine the 2nd and 3rd MCS to tell the post that they all have the same physical origin. I hope I have that right!


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[dreamstar]

Thanks guys, it's a big help.

Bill, I didn't know about the details window where the 1,2 3 increments makes it g54, 55, 56 so thanks. Under the same window, what is the difference between LOCAL and MAIN in the PURPOSE field? What about right underneath for the RCS... should I "link RCS to MCS" always?

One more thing... how do you get NX to output optional stop like M01 or M00?

Jaydenn, you are absolutely right. Once I posted my programs, the coordinates were right even if it was displaying the wrong ones on the toolbar.

Thank you for all your help.
Max

 

[miner49]

Max,

To output code to the post processor you need to add the command to the operations. On the Machine dialog ther are start of path and end of path commands.
The optional stop will output a M01
The stop command will give you an M00

These and many other commands can be customized with post builder.

You may want to check out

http://bbsnotes.ugs.com/

This has an entire thread for CAM it is free to licensed customers.