Work Offset Question

[Cartierusm]

I've read the Mach3 manual and I'm a little confused. I have a permanent laser center finder attached next to my router and I have the x and y coordinates from center of the router bit to the center finder. I want to be able to just use the laser and then zero out and run a program and have it know that 0,0 is actually x-1.2 and y2.3. Do all I have to do is put those coordinates into the G55 box in work offset, then when I run a program it will automatically compensate? Also do I need to set that G55 code in my CAM program or will Mach automatically add that part in?

[ger21]

You put those numbers in the G55 offsets for your laser. If you zero the coordinates for your spindle, when you call G55 in your g-code, then move to 0,0, the laser should be where the spindle was. G54 will reset the coordinates to match the spindle. Is that what you're trying to do?

[Cartierusm]

Actually I want to do the reverse, the laser is a laser center finder. So I find the edges of the piece with the laser and then zero out and have the offset compensate.

So I don't have to program it in when I'm using CAM? How does Mach 3 know which to use G54 G55, where does it get set. Thanks.

[neilw20]

Reference the machine.
Move to where you want. with you laser, etc.
Manually using MDI will do to select an offset table.
Say 30 by G59 P30

You can also do this from the MDI screen by manually entering the offset number, and also the offsets screen.

Hit the X and Y zero.

Now the P30 table has that co-ord as X0 Y0.

In the start of your porgram put G59 P30.

Use different offsets for different jobs. You can store more than 240.

Make sure in the setup screen that Mach3 is setup to save the offsets when it exits.

[ger21]

So I don't have to program it in when I'm using CAM? How does Mach 3 know which to use G54 G55, where does it get set. Thanks.

The G54 and G55 need to be in your g-code. If you can get your CAM program to do it correctly, that would work.

[Greolt]

This will not suit everybody but it's what I would do if I had a laser set up as you do.

Position the machine by jogging until the laser is on the feature I want then press a button on screen that moves the spindle to take up that exact position and zero the X and Y axis.

Easy matter to make a screen button to do this. Call it "Laser Zero" or whatever you like. Assign it a VB script to do the business.

If this idea appeals I can help with the script if needed.

Greg


EDIT: Here is a simple script that would do the job. Enter the values as needed in the "G0" line

DoOEMButton (1008) 'zero the X axis so the move will start from here
DoOEMButton (1009) 'zero the Y axis so the move will start from here
Code "G4 P0.25" 'pause for DRO to update
Code "G0 X-2 Y-1.5" 'here is where you enter the moves required to shift spindle to where laser was
While IsMoving () 'wait while it moves
Wend
DoOEMButton (1008) 'zero the X axis
DoOEMButton (1009) 'zero the Y axis

Lots of ways to skin a cat and this is one.

.

[Cartierusm]

Greolt, cool thanks. I appreciate it. Since I just built a killer Pendent control maybe I'll incorporate that button into it, then I don't have to go over to the computer or worry about the CAM or Mach dealing with it.

[Cartierusm]

Greolt, I need a little assistance in incorporating your script into my app. So I open Mach Screens 4 and load my .set file and create a button. What do I do next to make the button use the script you wrote? Thanks in advance.

[Greolt]

You need to assign the button control to "VB Script function in Mach3". See the pic.

Then in Mach go to Operator / Edit Button Script, then your new button will be winking. Press it.

This will bring up the VB Script Editor. Paste the script in there and save and close.

Simple as that.

Greg

.

[Cartierusm]

Greg, thanks for everything. That worked perfect, and now I don't have to worry about setting it in my actual G code, which I would be lost at anyway. Luckily I have the standard shift and control buttons for fast jog and step job already on my pendent control so I just asigned the control/Goto Zero combination to that new button.

[Greolt]

Glad to help.

I ordered off ebay a cheap laser that puts out a cross pattern. Thought I might give this idea a go myself.

Greg

[Cartierusm]

Cross pattern interesting. Can you give me a link? I use a Laser Center Finder from http://www.lasercenteredgefinder.com/ . When I made my Router Mounts I just put a 1/4" hole for the laser and then on the side drilled a #7 hole and tapped it 1/4"-20 and then made a little aluminum slug so when I tightened the set screw it didn't damage the Laser Center Finder shaft. I just made sure the bottom of the laser body was at the same height as the bottom of the collet of the router. Then I drilled a small indentation with a 60 degree V bit, a very small peck, zeroed out the DRO, moved the gantry until the laser was in the hole, wrote down the Coordinates. Then I jogged around the table and keep Manually inputting the data until it returned to the right spot every time. Now when I go to mill something I just align the laser with the x edge of the work piece, zero out, align with y edge of work piece, zero out, and then run the script you wrote me. No more changing to center finders or any of that crap.

On my table I also milled a 1/2" channel .175 deep x 29" long and then inserted a true piece of aluminum 1/2" x 3/8" x 28"stock. With a rubber mallet tap it into the recess and you have a perfectly parallel and perpendicular work stop to butt your pieces up against, I also did the same with x axis. So setup is a breeze. Make sure though that you mill the channels once the table is bolted to the router and make a straight cut using one of Mach 3 wizards. This way it doesn't matter if the wood top of the table is square to the table, the cut will be square to the cutting part of the machine.