Zero Z axis before cutting?

General software related questions should be posted here.
Post Reply
RAD
2 Star Member
2 Star Member
Posts: 81
Joined: Fri Aug 28, 2015 3:17 pm

Zero Z axis before cutting?

Post by RAD »

Do you guys normally zero your z axis before cutting? I zero mine about 1/2" above the material if I don't the z axis would ignore the float head switch and continue driving the torch into the material, this sometimes happens when doing my dry run before actual cutting. Is it standard procedure to zero your z axis? (Along with x & y axis) I'm using sheetcam and mach3. Thanks
D.I.Y 4x4 CNC Plasma Table with water tray
60 Gal. A/C + D.I.Y Aftercooler + Water/Oil seperator + Desicant air dryer
45XP (CPC with hand torch)
MiniTHC
UCCNC + Sheetcam + Inkscape / AutoCAD
AdrianH
2 Star Member
2 Star Member
Posts: 87
Joined: Tue Dec 27, 2016 1:08 pm

Re: Zero Z axis before cutting?

Post by AdrianH »

I know that my set-up is only a small home made hobby one, but I zero X and Y not Z, but I zero Z before every pierce. If the following helps?

I use a M800 macro to perform the zero, the probe switch on my set-up is mounted to the Z carriage, so I have the situation where the nozzle touches down on the metal surface and the Z carriage continues to move until the switch opens. A sort of floating head arrangement.

This is my M800 macro, it is a very slight rework of some on the Mach3 forum. But should give you an idea of how I do it.
M800.m1s
' APH
Code "G31 Z-30.0 F300" 'probe surface
' Wait for movement to complete
While (IsMoving())
' Sleep, so other threads can run while we wait
Sleep(100)
Wend
ZprobePos = GetVar(2002) 'get contact point
Code "G0 Z" &ZprobePos 'return to point to remove overshoot
' Wait For movement To complete
While (IsMoving())
' Sleep, so other threads can run While we wait
Sleep(100)
Wend
Call SetOEMDRO(802, -1.80) 'Set Z DRO = 0.00
Code "G1 Z 5.0 F300"
' Wait for movement to complete
While (IsMoving())
' Sleep, so other threads can run while we wait
Sleep(100)
Wend
' End



The 1.8mm is the difference between contact and switch opening and I found that using gauges and repeating several times.
It will probe down from current position to -30mm, I have my safe height at 10mm set elsewhere and as I have a very low pierce height at 1.5mm, the set-up comes from 10mm, finds Zero, sets the offset for the switch, goes up to 5mm and then down after this to pierce height back in Gcode.

Attached is a pic of the very basic head switch so you have an idea just how crude this is.
zeroswitch.jpg
Just wondering what your safe height is set to and if you have to be above that for your test to work?

I hope it helps in some way.

Adrian
tcaudle
4 Star Elite Contributing Member
4 Star Elite Contributing Member
Posts: 1353
Joined: Tue Feb 28, 2012 6:47 pm

Re: Zero Z axis before cutting?

Post by tcaudle »

There is a value in SheetCAM (Options/Job Options) that sets a value called Plunge Safety Clearance. If you have a POST that puts in the touch off code it should look something like: G28.1 Z.50 in the g-code That gets put in there in the SheetCAM function OnReference() so the number after the Z is the plunge safety clearance value. That defines the point at which it slows down from normal Z speed to Homing speed. Plunge safety should be at about 1/2" and rapid clearance about double that or more. You cannot set the feedrate of a homing move (G28.1. It uses the percentage in MACH for that Z homing speed. Z zero should be the top of the material The purpose of touch off is to reestablish Z zero BEFORE a pierce so its the correct height. There is a switch offset variable in SheetCAM (swtichOffset) that has to have a value to apply after the touch off switch activates, that lets the Z subtract the overrun from the Z so it should adjust the number to make Z zero the top of material. You can touch off as often as you want by setting the "refDistance" variable in MACH to a number (in mm ) where it it can move something like 100mm to factor in close pierces but touch off on ones further apart. Obviously on really warped material you may want to set that to 0 so it touchs off before every pierce
AdrianH
2 Star Member
2 Star Member
Posts: 87
Joined: Tue Dec 27, 2016 1:08 pm

Re: Zero Z axis before cutting?

Post by AdrianH »

tcaudle, I could have done with your help when trying to learn all this as I never found out any of this through the tutorials with Sheetcam. :)

Is there a written manual anywhere? in linux the program will not show the post documentation on my machine.

Adrian
RAD
2 Star Member
2 Star Member
Posts: 81
Joined: Fri Aug 28, 2015 3:17 pm

Re: Zero Z axis before cutting?

Post by RAD »

Thanks guys. My Z axis auto zeros via the float head as normal for every pierce and I have my switch offset value established and set in sheetcam (MP-1000 P/Processor edited). I am going to give refDistance a try though this would be useful in saving some time.

The problem is at the begining of a job if I don't zero my Z as I do the X and Y the Z axis basically drives the torch into the material and continues until it can't go anymore :shock: , but once I zero the Z about 0.5" above the material everything works fine thereafter, even if I reload a different job (as long as I don't close then re-open Mach)

I don't have a problem zeroing Z everytime I start Mach3, but I could not find any info on this anywhere else, which is why I ask if this is standard procedure, thanks
D.I.Y 4x4 CNC Plasma Table with water tray
60 Gal. A/C + D.I.Y Aftercooler + Water/Oil seperator + Desicant air dryer
45XP (CPC with hand torch)
MiniTHC
UCCNC + Sheetcam + Inkscape / AutoCAD
tcaudle
4 Star Elite Contributing Member
4 Star Elite Contributing Member
Posts: 1353
Joined: Tue Feb 28, 2012 6:47 pm

Re: Zero Z axis before cutting?

Post by tcaudle »

AdrianH wrote:tcaudle, I could have done with your help when trying to learn all this as I never found out any of this through the tutorials with Sheetcam. :)

Is there a written manual anywhere? in linux the program will not show the post documentation on my machine.

Adrian
The post documentation is for programming a POST using LUA It lists all of the internal variables and object names.
Some of (or a lot of) the settings and features are custom defined by the POST. So while there is a Plunge Safety Clearance value in SheetCAM its up to the POST to use that value as passed in put it in the G-Code. Generic posts don't use it . The later posts for CandCNC equipment use it and have other custom variables defined. The problem with flexibility and power in a program is its really hard to document. We cover it pretty extensively in our manuals for the DTHCIV and provide that info to our users.
Post Reply

Return to “General Discussion”