It may be something to do with cutter compensation and /or the tool diameter data in either Fusion, or your Tormach’s tool diameter offset table.
I work mostly with mastercam, so have little experience with Fusion, but most CAM software have a place in their contour tool path parameters where you can enter the cutter diameter, and select left, right, or no cutter comp. This tells Fusion which contour’s geometry the cutter is on, or if the cutters center is on the geometry.
For example: if we are climb milling, clockwise around of the geometry of a 2" square box, with a 0.500 diameter endmill - left cutter comp will give us a 2" sq box. riaght comp will take 0.500 off each side, leaving a 1" square box. and no comp will remove 0.250 off all sides, leaving a 1.5" sq box.
Also, if the cutter actuall measures less than 0.500", it will leave a larger sq.
If the cutter diameter is not listed accurately in CAD/CAM and Tormach tool table, the work piece dimension will be off.
Generally 3 areas need the correct data for the G-code to post properly:
- the correct cutter diameter must be entered in your CAD/CAM software (Fusion)n
- the correct cutter compensation selected
- the correct cutter diameter offset entered in the Tormach tool table.
You can also open the G-code editor, and take a look at the posted X & y move co-ordinates to help you determine what is going on. Cutter comp is usually set with a G41 or G42
For example, if the front corner is the work piece’s X=0 y=0 position, with a 1/4" cutter, starting at this corner, without any lead-in or lead out, climb milling CW, with left cutter comp , the cutter’s starting position, in your G-code, should be X -.125 Y 0.00 . Some (most?) CAM software also lets you selct how the cutter moves around a contour’s corner (with or with out rolling. - either will produce a ‘sharp’ corner) …With “none” selected the next cutter moves would be something like this:
G1 Z0. F18.
Y2.125
X2.125
Y-.125
X-.125
With “roll” the next moves would look something like this:
G1 Z0. F18.
Y2.
G2 X0. Y2.125 R.125 F5.
G1 X2. F18.
G2 X2.125 Y2. R.125 F5.
G1 Y0. F18.
G2 X2. Y-.125 R.125 F5.
G1 X0. F18.
G2 X-.125 Y0. R.125 F5.
Depending on what the difference in programmed size, vs. cut size, I’d check the Tormach tool offset table first, then Fusion’s cutter diameter, and then cutter comp selection.
I’m sure others more versed in fusion will chime in to give more specific help.
