Help. Levil FMV-F400 with FANUC Oi-MF controller....

[dcompton]

Hi All,
I am trying to learn our new Levil FMV-F400 milling education certification cart running a FANUC Oi-MF controller. When I set up and load a program, the machine moves to a random point not associated with the workpiece origins set in Fusion 360. I did some playing around and have found that the machine will still move to the appropriate machine zero location, but the RELATIVE and ABSOLUTE positions reflect this arbitrary position out in space. The documentation that we got with the machine is spartan at best and I cannot for the life of me figure out how to set the work origin position so that it matches the XYZ zeros for the part. Or at a minimum set all the zeros to machine zero so I can start over. I have manual milling experience using 3 axis DRO, and other non-FANUC CNC experience where I can simply move the spindle to the zero point, and zero the XYZ. Can anyone help me wrap my head around this? I simply want to be able to set the work zero to match the origin in FUSION 360 which should be in the gcode. Any help would be greatly appreciated. Thanks!

DC

 

[sinha]

There is a manual method for WCS datum setting. Another way involves manipulating the associated system variables. If you place the spindle at the desired XY datum of the WCS, and run the following program, it will shift the current-WCS datum to the current tool position.
The program was written for model C, but I believe, it would work on model F also.

O9000 (CURR WCS DATUM SHIFT ON MILL);

#1 = #4014; (If, for example, the current WCS is G56, 56 would get stored in #1)

#1 = #1 − 53; (This would store 1 in #1, if the current WCS is G54. Similarly, corresponding to G55, G56, G57, G58, and G59, the stored values would be 2, 3, 4, 5, and 6, respectively. In our example, #1 would store 3)

#1 = #1 ∗ 20; (#1 would store 20. 40. 60, 80, 100 and 120, corresponding to G54, G55, G56, G57, G58 and G59, respectively. In our example, #1 would store 60)

#1 = #1 + 5201; (#1 would store 5221, 5241, 5261, 5281, 5301, and 5321, corresponding to G54, G55, G56, G57, G58, and G59, respectively, depending on which one is the current coordinate system. The stored value would be the variable number corresponding to the X axis work offset value for the current coordinate system. In our example, #1 would store 5261)

#[#1] = #5021 − #5201; (#5021 contains the tool’s current X coordinate in MCS, and #5201 contains the X external offset. The control follows the logic that when the difference in their values is stored in the system variable corresponding to the X offset of a WCS, the current position of the tool becomes the new X datum for that WCS, that is, the current tool position gets redefined as X0 in that WCS. In our example, #5261 would get appropriately modified, which would shift the X datum for G56 to the current X position of the tool)

#[#1 + 1] = #5022 − #5202; (Shifts datum for the Y axis to the current Y position of the tool. In our example, #5262 would get appropriately modified, which would shift the Y datum of G56)

M30;