Workpiece Offsets

This section is for useful tips and tricks for Aspire
Post Reply
User avatar
TReischl
Vectric Wizard
Posts: 4589
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Workpiece Offsets

Post by TReischl »

I added a small laser module to my machine some time ago. It is mounted offset of the spindle.

The issue is running jobs that use both the router and the laser in addition to setting zero for the laser. I use Ger21's Screenset 2010 which allows the use of a laser pointer (this is not the laser cutter) to set a zero and adjust for the offsets between it and the spindle.

By running the spindle and then jogging around I finally figured out the relationship between the router spindle and the laser beam.

What I had been doing was to set zero for the router and then move the laser over to that zero and reset zero. Back and forth, too much fiddling around.

I would bet that most of us rarely used work piece offsets. Well, we did, but just the default one, G54. That is what I was doing. It finally occurred to me that all I really needed to do was enter the zero for the laser beam into G55. After setting zero for the router I just use windows calculator to get the new numbers for the G55 position.

The next step was to modify the post processors. The router post has a G54 call in it at the very beginning. It looks like this:

+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------

begin HEADER

"M5"
"G00G20G17G90G40G49G80"
"G70G91.1"
"G94"
"G54"
"G0X0Y0"
"M3"


I did the same thing with the laser post but entered G55 instead of G54.

Now the machine adjusts the zero automatically for the laser. If I go back to routing no need to fiddle around selecting G54, the code does it for me.

This was a little different than what work piece offsets are normally used for so I thought I would post it. Hope it helps other folks out!
"If you see a good fight, get in it." Dr. Vernon Johns

User avatar
highpockets
Vectric Wizard
Posts: 3667
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Workpiece Offsets

Post by highpockets »

WOW! Great tip Ted!!!

Thanks for sharing....
John
Maker of Chips

User avatar
rscrawford
Vectric Wizard
Posts: 1102
Joined: Mon Jan 17, 2011 6:49 pm
Model of CNC Machine: CAMaster Cobra 408 ATC, ShopSabre IS408
Location: Wetaskiwin, Alberta
Contact:

Re: Workpiece Offsets

Post by rscrawford »

Great idea Ted!
Russell Crawford
http://www.cherryleaf-rustle.com

Mobius
Vectric Wizard
Posts: 413
Joined: Wed Jul 09, 2014 1:19 am
Model of CNC Machine: CRP Pro 4848 Custom Build
Location: Drumheller, Alberta, Canada
Contact:

Re: Workpiece Offsets

Post by Mobius »

Awesome. I've got a laser enroute for my CNC right now, so this will come in handy!
Connor Bredin
Distinctive Dimensional Concepts Ltd.
www.distinctive-concepts.ca

chri879
Posts: 23
Joined: Tue May 10, 2011 5:33 am
Model of CNC Machine: CNCRP PRO48X48
Location: Redlands, CA
Contact:

Re: Workpiece Offsets

Post by chri879 »

Great tip, thank you for sharing!

User avatar
dwilli9013
Vectric Wizard
Posts: 1237
Joined: Mon Sep 30, 2013 12:45 am
Model of CNC Machine: 3 axis Self Designed Self Built
Location: Machesney Park Illinois

Re: Workpiece Offsets

Post by dwilli9013 »

Always thinking Ted. Thanks for the tip. :lol: :lol: :lol:
D-Dub
Dwayne
Dwilli

MAXJ
Posts: 35
Joined: Wed Aug 08, 2012 3:06 am
Model of CNC Machine: KRMx02

Re: Workpiece Offsets

Post by MAXJ »

Hi Guys,

Sorry if I ask the obvious question here, but I would like to understand Teds solution better. I still have lots to learn.

In Mach3 on the Offset tab, do you set the G54 value (the router position, relative to the workpiece Zero) as X = 0, Y = 0 and Z = 0 and then include the G54 command in the post processor, as stated.
Then Mach3 again, on the Offset tab, do you set the G55 value (the laser position, relative to the router bit) as eg, X = +65, Y = +35 and no Z, and again include the G54 command in the post processor as stated?
This way the post processor G55 command will compensate for this offset between router bit and laser focus point, so that router bit zero point lines up exactly with the laser zero focus point?

Cheers

Max

User avatar
TReischl
Vectric Wizard
Posts: 4589
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: Workpiece Offsets

Post by TReischl »

MAXJ wrote:
Tue Jun 23, 2020 1:52 am
Hi Guys,

Sorry if I ask the obvious question here, but I would like to understand Teds solution better. I still have lots to learn.

In Mach3 on the Offset tab, do you set the G54 value (the router position, relative to the workpiece Zero) as X = 0, Y = 0 and Z = 0 and then include the G54 command in the post processor, as stated.

The G54 values are set when you press the X,Y,Z zero buttons in Mach. If you set those values to 0,0,0 then your workpiece zero will be at machine zero. G54 is a special case in that the values can be set by pressing the Zero buttons in Mach.

Then Mach3 again, on the Offset tab, do you set the G55 value (the laser position, relative to the router bit) as eg, X = +65, Y = +35 and no Z, and again include the G54 command in the post processor as stated?

No. Doing so will put your workpiece zero at X65 and Y35. Remember, these values are all relative to where you homed the machine. G54, G55 are registers that are used to add values to machine zero. Then when the program is run these values are added to coordinates in the program.

This way the post processor G55 command will compensate for this offset between router bit and laser focus point, so that router bit zero point lines up exactly with the laser zero focus point?

Nope, the machine only reads the register in the gcode. It does not add up the G54 register and the G55 register.

What you wrote WILL work if you are using the centerline of the spindle to set X,Y zero. But it is still not adding the values in G54, G55 up.


Cheers

Max
"If you see a good fight, get in it." Dr. Vernon Johns

Post Reply