Re: [mfg-smartcam] Toolplane Coding

[Jeff Pieper]

I have mine setup to output the Work offsets with user events each time I start a side or rotate. I also use programmable work offsets so the operators don't have to figure them. The first element with the first tool on the B0 side would be #U10=54,#V10=Xoffset,#V11=Yoffset,#V12=Zoffset,#U2=0   This is what is output. G90 G10 L2 P1 X0.0 Y0.0 Z0.0     (programmable work offset) M107                                          (built in machine macro for home position) G54 B0                                     (work offset & pallet rotation)   If I'm going to do end work on the part it would be. #U10=55,#V10=Xoffset,#V11=Yoffset,#V12=Zoffset,#U2=90 or 270   G90 G10 L2 P2 X0.0 Y0.0 Z0.0     (programmable work offset) M107                                          (built in machine macro for home position) G55 B90                                     (work offset & pallet rotation)   This lets me output what I want in the code. We machine 6 sided aluminum blocks so I want to be able to assign a different work offset for each side. Each side would also be assigned its own work plane. Your temp file will also need the correct info to assign these values.   Jeff Pieper CNC Programmer ----- Original Message ----- As i understand it, the cg is returning the correct workzone (g54 g55 g56 etc) but your xyz values are coding from table center (or wherever your origin is). When you are defining the workplane, you must ensure that the toolplane switch to match the workplane is on.  A nice way to make sure this happens is to define your workplanes by using the Process_Options_Index Planes tool. Define an arbitrary workplane name in the xy_plane at the location you desire, then go to the aforementioned dialogue box and rotate locally to get your new plane.  Don't forget to reserve the new plane. If you are manually defining your workplanes, remember to click off the "from world" button, and click on the Match Plane button. -----Original Message----- Hello all. First I would like to thank you all for the help I have received with this forum thus far.  The information found here is most benificial. On to my question:  I am new to the 3D World of FFM.  I am programming a Horizontal mill with a tombstone. i was originally creating separate programs for each face on the tombstone and merging the code together to form one program. The parts I am machining have origin located in different locations on each face of the tombstone.  I created new work/tool planes approximately in the WCS where they would correspond in space inside the machine.  I have geometry on all faces but I can't get the code to output with the XYZ coordinates relative to the new planes I created.  The code generates values from the WCS.  I have the B rotation working in code, the G codes for my work offsets and the positions have the correct xyz relative to their plane orientation. What am I missing? Any help would be greatly appreciated. Thanks in advance Derrick