Hello Guest it is December 07, 2019, 11:07:54 AM

Author Topic: Use probing for tool zeroing  (Read 10501 times)

0 Members and 1 Guest are viewing this topic.

Offline DazTheGas

*
  •  750 750
  • DazTheGas
    • View Profile
Re: Use probing for tool zeroing
« Reply #10 on: December 01, 2015, 11:04:23 AM »
The probing screen does work, i will be doing a video over the coming weekend, i have just been too busy later on other stuff, pedio if you go into the video section and have a look at the m6 command i did you will find a bit of code there that can be customised to do an autozero.

Daz
Theres always time for a choccy biccy

Offline DazTheGas

*
  •  750 750
  • DazTheGas
    • View Profile
Re: Use probing for tool zeroing
« Reply #11 on: December 02, 2015, 11:23:06 AM »
OMG your right although the probing screen does work I cant see a way of using a toolsetter to zero the z, not too worry heres what i use.

Create a button and in the script put

Code: [Select]
local ToolSetter = 15.7 -- change to your toolsetter hight
mc.mcCntlGcodeExecuteWait(0,"G91 G31 Z-15 F40") -- change feedrate and depth to suit
mc.mcCntlGcodeExecuteWait(0,"G91 Z2 F40") -- change feedrate and retract to suit
mc.mcCntlGcodeExecuteWait(0,"G91 G31 Z-3 F10") -- change feedrate to suit
mc.mcCntlGcodeExecuteWait(0,"G91 Z5 F40") -- change feedrate and retract to suit, use this Z rectract value for line 7
wx.wxMessageBox("Remove ToolSetter") -- remove if needed
mc.mcCntlGcodeExecuteWait(0,"G91 Z-"..ToolSetter +5 .." F50") -- change feedrate and retract to suit
mc.mcAxisSetPos(0,mc.Z_AXIS,0) -- set Z axis to 0

Daz
Theres always time for a choccy biccy

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Use probing for tool zeroing
« Reply #12 on: December 02, 2015, 11:42:54 AM »
I don't know much about Lua, but I see you probe twice, retract, and THEN zero the Z axis? Am I missing something? It looks like you're setting Z zero above your touch plate?
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline DazTheGas

*
  •  750 750
  • DazTheGas
    • View Profile
Re: Use probing for tool zeroing
« Reply #13 on: December 02, 2015, 01:01:33 PM »
line by line, I us metric

1. Sets the toolsetter height
2. Probes down a maximum of 15mm at a feedrate of 40
3. moves back up 2mm
4. Probes back down at a slow feedrate of 10 for more accuracy
5. Retracts a small amount to remove toolsetter as ive seen some with a small lip around them
6. inform operator to move toolsetter
7. moves back down the toolsetter height + the 5mm we raised on line 5, this leaves the tool on top of stock
8. set z dro to 0

if that helps

Daz
« Last Edit: December 02, 2015, 01:03:41 PM by DazTheGas »
Theres always time for a choccy biccy

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Use probing for tool zeroing
« Reply #14 on: December 02, 2015, 02:04:42 PM »
OK, I misread line #7.

However, In Mach3, we set Z zero at the trip point, which is stored in a variable.

Your method sets z zero where the tool stops, after decelerating. Not quite as accurate.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline DazTheGas

*
  •  750 750
  • DazTheGas
    • View Profile
Re: Use probing for tool zeroing
« Reply #15 on: December 02, 2015, 02:23:25 PM »
we set Z zero at the trip point, which is stored in a variable.

Good point, I will have a change and perhaps send the value to a pound value

Daz
Theres always time for a choccy biccy

Offline DazTheGas

*
  •  750 750
  • DazTheGas
    • View Profile
Re: Use probing for tool zeroing
« Reply #16 on: December 02, 2015, 03:30:37 PM »
ok updated to set z axis on probe touch

Code: [Select]
local ToolSetter = 15.7 -- change to your toolsetter height
mc.mcCntlGcodeExecuteWait(0,"G91 G31 Z-15 F40") -- change feedrate and depth to suit
mc.mcCntlGcodeExecuteWait(0,"G91 Z2 F40") -- change feedrate and retract to suit
mc.mcCntlGcodeExecuteWait(0,"G91 G31 Z-3 F10") -- change feedrate to suit
mc.mcAxisSetPos(0, mc.Z_AXIS, ToolSetter) -- set dro to height of toolsetter
mc.mcCntlGcodeExecuteWait(0,"G91 Z5 F40") -- change feedrate and retract to suit, use this Z rectract value for line 7
wx.wxMessageBox("Remove ToolSetter") -- remove if needed
mc.mcCntlGcodeExecuteWait(0,"G90 Z0 F50") -- move tool to zero,  change feedrate to suit

Daz
Theres always time for a choccy biccy
Re: Use probing for tool zeroing
« Reply #17 on: December 03, 2015, 03:28:06 PM »
Tool Zeroing is apparently going to be part of the next release. I have a "sequence" that is supposed to work with the current probe screen but I haven't tried it yet. I will try when I'm home tonight and if it works I will post it here.
Re: Use probing for tool zeroing
« Reply #18 on: December 03, 2015, 05:58:45 PM »
It works. It's not ideal but it'll do until they release the version including tool zeroing.
Here's what you do.
Set your block on top of your material.
Move the z down to a close distance from the end of the tool.
Zero your Z axis DRO.
Go to the "probing" screen.
Set the Z position to a negative amount that will result in contact with your plate.
Set "Measure Type" to "set Fixture".
Press the measure Z button.
It'll go through it's sequence, when done, the number in your Z DRO is the amount it is above your block.
Remove your block, do a G0 Z-(distance in z DRO + Block thickness)
the tool tip will be at the top of your material, set your DRO to 0.
Or you can just add the thickness of your block to the "end result" DRO number and set the Z DRO to that sum. I'm sure you get the picture with that.

Now, the reason I found that this was not working for me was the soft limits. With Soft Limits enabled, I Get an immediate error saying "NO Contact With Probe".
And if I keep trying the measure Z button it eventually goes to a PMDX error 7.

With soft limits disabled, it has worked every time I've tried it.

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Use probing for tool zeroing
« Reply #19 on: December 03, 2015, 06:58:26 PM »
Sounds like a bug in the PMDX plugin. Be sure to report this to them.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html