I'm making a lathe machining simulation in NX10 and I have some troubles with the different coordinate systems. Before I apply this to my own lathe I tried to do it with the OOTB sim11 sinumerik 2 axis turn, but I can't figure it out either.
What I'm trying to do is to define a machine zero like my actual lathe has, positioned around this area:
I'm trying to do this such as when NX reads G53 from an external machine code file it positions the tool regarding this origin, and when a G54 shows up the tool is again positioned regarding the tip of my piece (like my actual lathe does and like my colleague in Vericut).
Right now I have the kinematic model of the sim11 lathe unchanged and my MCS/RCS configured like this:
I tried to change almost every coordinate system by trial and error (MCS/RCS and the junctions from the kinematic model) but nothing changes, when I have either G53 or G54 the tool is always positioned regarding the tip of my piece...
If someone could explain to me how it works I would be very grateful.
you need to define the machien zero NOT in CAM, but inside the kinematic model of hte machine tool.
Use the Axis initial Value if the CAD model is not at teh machien zero already. You can test it with preview motion.
Thanks, this helped me for setting the machine zero, I changed the X and Z axes.
But now my simulation does everyting regarding the machine zero. If I try to simulate a simple test code:
G53 G0 X0 Z0
G54 X0 Z0
I don't have any motion on the G54-line, NX doesn't make any difference between G53 and G54. How can I manage this?
How to define offset is the next step. Also not complicated.
You can have a look into the CAM setups in our OOTB Example.
Usually we define a local MCS Fixture Offest Number 1 -> G54 and OOTB post and Simulation will handle it.
May also this doc give you helpful information.
Hello, this is indeed what I tried to do, and I also started to look in that documentation.
For more clarity I attached my files in a zip with all my configurations.
Thanks for the help.
The Sinumerik CCF implementation of G54 G55 etc. expect the definition of the offset upfront like e.g.
The OOTB post is creating and to_ini.ini file with data for offsets and tools.
In your case the G54 offset is simply 0/0/0
You can change that behavior inside the MCF with setting a global variable
GV_bUseLoadOffset and GV_bUseSetToolCorrection
More details check the PDF Docs.
In MY_TURN_03_sinumerik-Main.ini, add line below:
(^ using your machine specific home x/z coordinates)
For Sinumerik, program like this:
N160 G500 N170 T0 N180 G0 X=0 D0 N190 G0 Z=0 N200 M30
Not sure if this will work with the G53. As Thomas mentioned, you may have to tweak the MCF
Hope this helps