Gerry,

Working on the tool change as designed with a fixed position and moveable plate and got the following error:

"Tool Change Z Position can NOT be above Z=0 System going to E-Stop"

The initial tool setup seemed to work fine, the top of stock was identified and then the fixed position was identified. It then went back to its originating position and waited for me to turn on the spindle. It ran the test pattern then went to I believe the Change position of "4", not sure? It waited for the tool change, after which "Cycle Start" generated the error.

Does that have to do with the Z Pos for the Change Position?

see attached

The tool change position is in machine coordinates.
When using the auto zero functions of the 2010 Screenset, Z zero in machine coordinates must be the top of your Z travel. So you can not have any machine coordinates greater than 0.
Your tool change Z axis position must be a negative value.

So my z works in the negative - Z zero is the top of my z axis.

Does that mean if I want to change bits at 4" above the table and my total z is 0 to -7 so my tool change z will be -3?

Yes, set your tool change Z position to -3.

Are you homing the machine to the top of the Z axis?

Yes, Z homes to the top.

Is there a different way to home Z since all of my work is done in the negative -Z?? Just curious what the standard practice is...

Adam,

No, that is correct. Just remember that the positions are in machine coordinates.

OK, great I'll give it a shot this evening.

One last question about the "Clearance Plane" is that based upon the work surface? So, if the work surface is on a 1" piece of stock and I want a clearance of 3" and my Z travel is 0 to -7, will I set this number to 3" regardless or do I need to do the math to calculate it based on the Z axis ( -7 + 1 = -6 + 3 = -3 )?

Thanks,

Your travel really has nothing to do with it.
The Clearance Plane is specified in work coordinates.
When you zero to the top of the part, your setting the work coordinate zero to the top of your part. If you want the clearance plane 3" above your part, then it's 0+3 = 3.
So you set it to 3. But you don't calculate it based on travel.

I'm pretty close to having this going but noticed when cutting some demo circles and calling for 2 tool changes that MasterCam output some GCode that I don't need.

I assume that lines N282 - N288 is standard on some machines but since I don't have a tool changer is there a way to eliminate the GCode from being generated? I think those lines were interrupting the flow of the change in the Macro's in the screenset.

Isn't the M6 the only line needed and the Macro should take care of the rest, Clearance Plane and Tool Change position?

N278 G1 Z.203 F30.
N280 G0 Z.25
N282 M5                 -- Spindle stop
N284 G91 G28 Z0.   -- not sure why this is here
N286 A0.                -- not sure why this is here
N288 M01               -- temporary stop
N290 T235 M6        -- Tool change  
N292 G0 G90 G54 X1.875 Y6.7025 A0. S12224 M3
N294 G43 H235 Z.25
N296 Z.2

You need to edit your post processor to remove those lines.
You do want to keep the M5 to stop your spindle.