Touching off

I'm struggling with process here. I have my origin set right and the gcode loads properly into linuxcnc. I take the tool to the top corner of the work piece (not the table) and touch off.

At this point the z rises for a tool change which is fine but then when it drops down it hovers about 3/4 of an inch above the work piece and starts its run.

How do I properly touch off the Z axis so that it properly plunges into the workpiece? I've read the docs and can't seem to make sense of how to touch off in the GUI and start the gcode properly.

This is a 3 axis cnc router setup.

Thanks!

I don't use tool tables or do tool changes. I use one tool per gcode file.

To touch off Z I have the tool I'm going to use in the collet, lower the tool towards the work piece until it
A: Just touches the work piece and touch off Z at Zero
B: I can just slide a block of a known height under the tool and touch off Z at the height of the block. ie I would enter the height of the block in the touch off dialogue.

In the near future I will get a Z Axis tool height setter to get the height a little more accurate.

It is basically the same concept as setting X & Y.
Use a edge finder to find the edge of your stock in the X & Y directions and either touch off entering half the diameter of the edge finder or move the edge finder half the diameter of the edge finder and touch for zero.

so if I take the tool and touch the top of the 1/2' work piece do I enter P0 Current or P0 Current -.5?

Bearfood wrote: I have my origin set right and the gcode loads properly into linuxcnc. I take the tool to the top corner of the work piece (not the table) and touch off.

The image is found here --> www.linuxcnc.org/docs/html/gui/axis.html#_manual_control
The tool can be touched off the top of the work and entered as zero like the image above. If a block was placed on top of the work for measuring purposes the entry in the 'blue box' above would be equal to the thickness of the block. I use a 0.020" feeler gauge to touch-off so the entry is 0.020". This assumes you are working as BeagleBrainz describes. Delete any G43 in the program (best idea) or at least have 0's in the tool table.

Post your GCode.

Depends on what you have set in CAM - zero on top of workpiece? Zero on bottom of workpiece? (Or something else even)

I usually have zero on top of workpiece in CAM.
Bring tool down until just touching the top of the workpiece
Touch off Z = 0

What direction do the numbers go when you move Z?
As you move Z down, Z value should decrease.
My machine ini has 0 at the top of Z (Max value) and -185 (minus185) as bottom of Z.

Yikes, I must have been half asleep. Leave the tool touch-off button alone and use this.

Continuing on Pippen's thoughts, if the program has Z=0 at the bottom of a 0.5" work piece and the tool touch-off is the top of the work piece, the value to enter is +0.5".
I program Z zero at the top of the work 99% of the time but some software, like Vectric, wants to work the opposite way.

The original post sounds like there might be a tool-length in the tool table, but he is touching-ff without a tool + g43 in effect.

I had a similar problem once and it turned out that I had a length value in the tool table that I didn't know was there. I think it got there by me clicking on Tool Touch Off rather than Touch Off. I cleared all length values from the tool table and it solved the problem.

Thanks, looking through this and the suggestions I went back into CAM and found that my origin was on the bottom left corner of the workpiece not the top. With the origin on the bottom I believe I touch off with a .5 offset whereas if the origin was on the bottom I'd touch off to the top of the workpiece with a 0.0 offset.

in Vectric, edit the post-processor and change the Z variables:

VAR Z_POSITION = [Z|C|Z|1.3|-1.0]
VAR Z_HOME_POSITION = [ZH|A|Z|1.3|-1.0]
VAR SAFE_Z_HEIGHT = [SAFEZ|A|Z|1.3|-1.0]

now works like expected...