Tool change position

[JayCNC]

I'm sure this is probably something easy but I'd like to set up my X-axis on my gantry to be centered for tool changes. All of my tools are in toolholders so no need to touch off each tool after installing it into the spindle for work. I remember doing "something" awhile back to make the X-axis centered after the job was completed and thought it was going to work for every tool change in the program but it didn't, only at program end. I can post a report tomorrow night if need be. Thanks! Should be posted in Acorn, sorry...

[Racedirector]

Isn't G28 the tool change location? I set G28 to where I wanted it to happen and it just goes there when M6 happens......

Cheers

[cnckeith]

yes.. set the G28 return point for default tool change position.

[JayCNC]

Hey Keith, I think I did that but when it calls for a tool change it only goes to Z0. Attached is my report from a few minutes ago, am I missing something maybe? My code reads as follows at the end of a tool run for a tool change-

N300 G2 X7.2 Z0.15 I0. K0.2
N305 G0 Z0.6
N310 G17
N315 G28 G91 Z0.
N320 G90
(Drill2)
N325 M9
N330 M1
N335 T14 M6
N340 T16
N345 S6500 M3
N350 G54
N355 M8
N365 G0 X2.3309 Y-2.206

[Racedirector]

N335 T14 M6
N340 T16

It wouldn't be because there are 2 tool calls and only 1x M6?

Cheers

[Dave_C]

JayCNC wrote:

N315 G28 G91 Z0.

Jay, try removing the Z0 from the line and then see if the tool change will go to all three axis of the G28 settings. If you call out just one axis I think this voids the other two!

My Fusion 360 post sometimes post only two axis and I have to edit this line as well to get my tool changes over to the point that I want.

Dave C.

[JayCNC]

So the only thing that seems to work is to add X0 after Z0. Removing Z0 brings all 3 axis where the Acorn software is telling it to, and I guess that works but it's making an additional Y move that really isn't needed. Is there a way to edit the post processor to automatically add X0 into it or do I need to manually edit the program each time? Thanks!

[Dave_C]

So the only thing that seems to work is to add X0 after Z0. Removing Z0 brings all 3 axis where the Acorn software is telling it to

My fusion 360 post just does two axis by default but I don't know how to make a post do just two. I have to add the Z axis so it returns to my tool measuring point as I don't have repeatable tool holding positions.

Dave C.

[cncsnw]

No, there is no way to modify the postprocesser of the Intercon conversational programming.

If you want this move to happen at every M6 tool change, then you could add the G28 move to a custom M6 macro file.

E.g., in mfunc6.mac:

Code: Select all

  G91 G28 X0 Z0 ; move X and Z directly to return point #1
  G90   ; restore absolute positioning
  M6    ; call default M6 action

For that to work properly, you may need to update to CNC12 v4.16 when it comes out, due to an M function recursion issue in v4.14. In the mean time you could use an M0, M200 or M225 in place of the M6.