Fusion360 Cutter Comp

Can anyone who is running Fusion360 share how you are doing cutter comp? I would love to hear about how you have the actual CAM set up as well as your tool table in LinuxCNC. We messed with it a bit and we were getting parts that were oversized by the endmill diameter. I attached the settings in Fusion we were running. In LinuxCNC we just entered the endmill diameter in the tool table.

We're running a completely custom 4x4 router with a Mesa 6I24-25, among other goodies. I can get the LinuxCNC version on Wednesday.

- Nick
 

andypugh wrote:

I believe that is an option at the postprocessing stage, but I can't remember exactly where it lives.

 

@Andypugh
I haven't used it either with LCNC, but it's an option for each operation under Passes tab.  Nothing in the standard LCNC PP about cutter comp.

I think you're on the right track...sounds like a radius vs. diameter issue.  If the part is exactly one tool diameter larger in X/Y, then each side is oversized by 1/2 the diameter.

When cutter comp is accidentally turned off (or the diameter in the tool table is 0) the parts should come out undersized by the tool diameter since each side of the part gets a haircut by 1/2 the tool diameter.

@ndp

• LCNC tool table must be in diameter - check this first.
• Program a simple square toolpath in F360 with a simple tool.
  • Use 2D contour, no lead-ins, nothing swoopy (plunge in)
  • Make sure the part dimensions to be 'cut' is an easy number (like 1", or 100mm) when compared to the tool diameter.
• Output two versions - one with cutter comp "in control" and one produced by F360
  • The "in control" version should have X/Y values which follow your part dimensions
    • G1 X0 Y0 Z1 Fnnn (or something similar)
    • Z0
    • X0 Y1
    • X1 Y1
    • etc. 
  • The F360 version should be your part dimensions, plus the tool radius.  So for a 1"x1" part and 1/2" dia tool:
    • G1 X-0.250 Y-0.250 Z1 Fnnn
    • Z0
    • X-0.250 Y1.25
    • X1.25 Y1.25
    • etc, as it walks around a square that's 1/4" larger in X/Y than your part.
• If the gcode looks good, the final thing to do is see what LCNC actually does with the code.
  • Put a pen in the spindle and a piece of cardboard on the table
  • Define the pen as the tool from the program, and make sure the tool table diameter matches what you had in F360
  • Run the program (after the usual touch-off in Z and so forth.  No need to smash a pen.)
    • You should, if everything is right, have see both versions follow the same exact toolpath.
• If not, something is actually wonky in LCNC's cutter comp - some additional offset or setting somewhere is biting you.  Report back if this is the case and we can see what the deal is.

Hello,

if there is no "G41" or "G42" at the start of your contur and no "G40" at the end of your contur then there is no compensation in your program and the control will ignore the diameter in your tooltable!!

Martin

I looked at this the other day. If you check the F360 docs, when doing in control compensation, the tool  diameter in the tool table should be set to zero for no compensation because this field is used for the amount of compensation to apply. This explains why you offset by the tool diameter

In the end, I changed the F360 tool diameter before i found this.

i think this is also a big how do you use the machine,
do you program by the part size and then put in a tool size in the table comp to get the right size part? ie enter 5mm to use a 5mm cutter.. ( the + to this is you can swop a cutter to 6mm and change comp and away you go, no reprograming)

or program including the cutter size which tends to be how most of us program out of a CAM system i would think?
or any of the other ways?
this is the very reason fusion has so many comp options.

for my self now days i leave comp off on operations and only set it to on if i know its a feature that i need to keep in tolerance on part life. some times i use D value same as tool number, other times in linuxcnc i setup extra tool slots as some times you do need mutipal D comps for a tool.

the option i use for comp in fusion is set type to wear
and set the value to 0

then the D value comp will offset the cutter by the value you enter for the D term (+ or -) ammount, and use this a "trimmer" type function
so can enter in a small number like 0.1mm and your cutter would stand off by 0.1mm from programed path..