EstlCAM tool change without probe?

Software / Firmware EstlCAM
1

I’m using EstlCAM and doing some pen plotting. I have a change to a different pen in the job. The thing is that the pen is a rollerball gel pen and thus doesn’t have a continous conductive path from the ball of the pen to the body, so I can’t use the touchplate. I set 0 by manually lowering Z in FluidNC until the pen is touching where I want it to be.

The EstlCAM tool change script includes a G38 line to probe. When it does this, the Z gantry crashes into the workpiece since there’s nothing to probe. Is there some gcode I can use to have the job pause, let me swap the pen, then resume and have it return exactly where it left off?

2

You have some options. You can either have separate gcode for each pen, or you would need some way to manually set the pen to the correct height without being able to jog. You could do something like set the pen height in the holder so it touches a piece of wood and then set that thickness as the offset. Then when you have to change pens, it can pause, you replace the pen and set it the same height using that wood and resume.

I’m assuming you are using a Jackpot. If that’s not true, this changes a bit but the general idea is the same.

I think that would change the starting gcode to this (assuming you use a wood block that is 25mm thick - I set it to 24.5 so it lowers the pen a bit extra, might have to mess with that). It assumes you set the position prior to running the job.

G21
G90
G94
G92 X0 Y0 Z24.5
G1 Z10 F900
M62 P1 (If used start spindle pin27 )

And the tool change gcode would change to something like this:

M63 P1 (turn off pin 27)
G91
G0 Z10
G90
G0 X0 Y10 Z25 F2520 
M0 (MSG change tool, remove spacer)
M62 P1 (turn on pin27)

I didn’t actually test this but it makes sense in my head. :rubberduck:

3

My start gcode assumes that I’ve already dropped the pen to exactly the level it needs to be. I set the cut depth in Estlcam to something like .5mm so that I can move Z to get the pen just touching a feeler gauge, then start the job.

That said, my start gcode is presently this:

G21
G90
G94
G92 X0 Y0 Z0
G1 Z5 F900

With that start gcode, should the tool change gcode then become this?

M63 P1 (turn off pin 27)
G91
G0 Z10
G90
G0 X0 Y10 Z25 F0 
M0 (MSG change tool, remove spacer)
M62 P1 (turn on pin27)
4

I think at that point, for the tool change, you would want to go to the tool change position. The normal Z of 10 is probably fine. Pause, remove the pen, and resume. Have it move to Z0. Pause, insert the pen so it’s just touching the feeler gauge, and resume.

M63 P1 (turn off pin 27)
G91
G0 Z10
G90
G0 X0 Y10
M0 (MSG remove pen)
G0 Z0
M0 (MSG insert pen touching feeler gauge)
G0 Z10 (add clearance so pen does not draw moving back to position)
M62 P1 (turn on pin27)

Does that make sense?

1 Like
5

Makes sense and even better, it works exactly as intended in testing. Thank you so much!

2 Likes