I am trying to create a post processor and simulation in NX 11 using the OOTB sim15_millturn_9ax_sinumerik_mm. The machine actually has no lower turret, but two B-axis heads (each on one channel.) This means two 5 axis kinematic chains. Can someone answer right off the bat, will I need Machine Configurator in order to create this? I don't think there are enough axis addresses in the sim15_millturn_9ax_sinumerik_mm MCF file.
We have almost everything working on the first channel except the b-axis compensation in the simulation. We still have the simulation driving the b-axis center of rotation, not the spindle nose. I think this is an issue with our Sinumerik code that we are posting, but I'm struggling to get this correct. The machine manufacturer has a special sub prog for B-rotation that is too complex, so we are trying to simplify it just to make the simulation work. It is TURN(b angle, tool angle, traori on/off, spindle number). I tried to copy the TC.spf sub program to start, but it still drives the center of rotation. Does anyone have any suggestions? So far we are just simulating turning operations.
Thanks in advance.
about set up the kinematic model with all the axis you do not need the Machine Configurator. Axis definition and channel as well as chain assignment can and should be comply done inside the NX MTB Machine Tool Builder application.
To fully customize your machine tool simulate correctly, I strongly suggest you will need to do mollification inside the MCF file and for this the Machine Configurator (Advanced License) is needed. Especially for complex mill turn machine tools it will mostly not work by "simply" copy MCF/CCF files form an OOTB machine tool.
About B axis head compensation what you mention is exactly one point you need to dive into. Inside the tool change program and maybe an additional subprogram TURN specific settings are done which are essential for doing a correct simulation and compensation. The TC.spf from sim15 is one example how that can be done, but each machine tool vendor does it differently. At the end all using Sinumerik code like M6 CUTMOD TCARR and others. From my experience it is needed to understand what is really happening inside the subprogram if you will not use it as it is and re-engineer it inside your own tool change program.
We already post some videos about handling offsets here:
Hope that helps
I think I have a bit of a strange scenario with this machine in that at B=0 the tool tip is actually pointing along the X- direction for this machine rather than the Z- direction. I believe I should be able to accomodate this by modifying the GMe_Activate_Tool_Correction in the MCF file, but I am struggling to determine which items to edit. Any suggestions?
the files PMAC and PGUD are part of the encrypted *cyc file and they get executed from an ini file during initialization of CSE. Many different definitions are handles. That are files form the Sinumeirk controller.
first update the KIM model with your B axis origination.
Make sure initial value is correct, then try moving with CSE to e.g. G53 G90 X0 Y0 Z0.
Try first without tool mounted and correction activated.
As a second step mount tool and activate tool length correction- but without B axis change.
At last to the more complex one, the method you mention is the one which maps the tool length values to the axis of the machine tool.
my B-axis center of rotation moves to 0,0,0 when G53 G90 X0 Y0 Z0 is programmed. This is correct when D0 is programmed on the actual machine tool. When I do this with Sim15 it moves the spindle nose to 0,0,0. I'm trying to understand which of the TC_CARR values I need to change in order to compensate for the length of the head during GMe_ActivateToolCorrection.
Thanks very much for the help so far.
do you have the basic stuff running in your machine tool environment? In particular I meant if this:
"my B-axis center of rotation moves to 0,0,0 when G53 G90 X0 Y0 Z0 is programmed"
is working correct in ISV?
That will be achieved by setting the initial values inside the KIM.
Are you saying in your machine tool the D1 only will compensate the tool length plus the length from spindle nose to center of rotation? Is there no other code responsible for that?
At TCARR=0 D0 G53 X0 Y0 Z0, the machine should have axis of rotation of B axis at 0,0,0. (this works)
At TCARR=1 D0 G53 X0 Y0 Z0, the machine should have spindle nose at 0,0,0.
The TCARR.DEF is the same as the machine. Now I get different behavior depending on what I make the initial B angle and what is the Zero B angle in the KIM. This is progress, but for some reason it's compensating in both X and Y when I call TCARR=1 D0 G53 X0 Y0 Z0.
I am trying to understand where this compensation is driven in the MCF. Does the MCF look only at the TCARR table or does it consider the junctions in the KIM? Any hints on where to make this work correctly before I dive into the tool correction?
Hi Jeff, I hadn't much time today, but does the description of TCARR give you same answers already?
You find it inside the Machine Configurator on the button.