Post Processor for TRAK LPM CNC Mill with Solidworks
Working on this using UPG-2
Copy the .ctl and .lng into your Solidworks Post Folder
Use the .SRC and .LIB to edit and make changes.
- Preloading tool change ✅
- Figure out compensation (Currently must be disabled in Solidworks to avoid errors)
The following are modifications to a Fanuc 6 post-processor that are necessary for writing the ProtoTRAK post-processor.
- Beginning file format: The ProtoTRAK has no special requirements, it does not need any special characters.
- ✅ - Already good as is.
- End of file format: the ProtoTRAK requires the % to show the end of the file. Characters after the % will be ignored.
- ✅
- Beginning of an operation: the ProtoTRAK requires that the tool number, feedrate and tool comp appear before, or on the same line, as a move command. The absolute zero of the ProtoTRAK is set in a different mode and does not need to be set at the beginning of each operation. The feedrate is modal, once it is set, it remains the same until changed.
- ✅ - Already good as is.
- Coordinates: may be formatted in inch or metric. The addresses used for specifying coordinates are X, Y, Z, I, J, K. The valid ranges are:
- Inch: min -999.9999 to max +999.9999
- Mm: min -9999.99 to max +9999.999
- Integer values MUST be followed by decimal. Ok to truncate 02.0000 into 2.0
- Linear moves: G01 are formatted the same as rapid moves.
- Arcs: Arc centers are specified by the address I, J and K for the X, Y and Z axes. The number following the I, J and K are incrementally referenced from the starting point of the arc. Radius values are not allowed.
- Tool Numbers and Tool Changes: the format of the tool number is from T1 to T99. The M06 command initiates a tool change.
- ✅ - Already good as is.
- Feed rates: the ProtoTRAK is programmed in inches (or mm) per minute using the 'F' address.
- ✅ - Already good as is.
- Spindle speed: S1000 means 1000 RPM
- ✅ - Already good as is.
- Turning the Spindle on: the spindle is turned on with M03 or M04 command.
- ✅ - Already good as is.
- Tool offsets, diameters, modifiers, home positions and work offsets are defined on the ProtoTRAK control and are ignored through G code.
- G2 and G3 are not used for helix. See G06 and G07.
- You must specify an I, J and K for all arcs, even if you are doing an XY plane arc where the Z axis is not moving. In this case the K value must be defined. It will be modal from there on.
- For lead in moves where you are using G41 or G42, G41 and G42 need to be placed before the Z axis moves down to position so the tool