Creating a consistent Zero Point when doing repetitive carving with Easel

Good morning. I am new to carving and could not find a match for this question. Perhaps someone can help or point me to an area where I can find a clear and concise answer.

I have a drawer front which I am carving on a consistent and repeatable basis. I have created a jig for the X-Carve to give me consistent placement of the part each time I place the stock in the machine. After homing the X-Carve, I need to move the spindle to a specific location to carve the material. Since the material is always in the same location on the carving bed, is there a method in which I can specify the X/Y axis points as the zero point for the carving rather than eyeball the carving point? Ultimately, these are simple, rectangular cutouts inside of Easel and I am bringing the images into Easel as SVG files which were originally developed with Adobe Illustrator (not really an important point, just extra information). I am using the probe for the Z axis and it is working fine.

I could edit the G-Code, but would need to know how the G-Code points would need to be defined.

I thank you in advance for any assistance you can give me on this topic.

Randy

When you do the first one, you’ll jog the machine to the X/Y position and set that as the X/Y home/zero position.

Every other carve, you’ll just select “Use last X/Y position”. As long as you home the machine, the X/Y spot will be the same.

Thank you for the reply Justin.

I am aware that I can use the last X/Y position. Rather, I was asking if there is a method to input a X/Y zero position in the setup for this operation. The subsequent carvings in the batch could use the last X/Y position.

An alternate which I could use, would be to have a a G Code which I could import for this carving, but, if the test carving is off, then the G Code offsets would be incorrect.

Your thoughts?

Provided you have limit switches installed you can Home your machine. (Not Easel Home position which = work zero)
If you can Home your machine you have a consistent machine reference point.
With a reference point you use parking spots G28 and G30 to give you a consistent offset from that reference.

I’m confused and I think Haldor might have described it better.

There’s two zero points. Machine zero is set by homing. Work zero (what I was referring to albeit poorly) is a zero position using an offset from the machine zero position, which persists during power cycles as long as you home first.

@RandallBishop I have done a couple of videos on this topic

https://youtu.be/XnZhGkmXQtE

Hope this helps you

Thank you for sharing this Phillip. This was useful as I will not be starting from 0,0 on the waste board… I think the real key is being able to manually plug in an X/Y coordinate as the base for work zero. I will be reviewing your other videos as time permits.

Thank you Haldor for the reply. I’m thinking that, once I find the “sweet spot” for the work zero of the jig/fixture, I will set the value and export the G code for future use. This will ensure consistency from setup to setup.

Thank you Justin. This has been a great discussion and I think you have got me thinking out of the box on this. I would still like to know if there is a way to manually set the X/Y work zero. From what I am hearing, there does not appear to be a way to do so.

I will play with this tomorrow to see where this takes me.

Thank you again.

I wonder if this is what you are looking for:

G10 L20 P1 X0 Y0 Z0

This command will set the workpiece x y and z zero to wherever the spindle is located at the time of the command.

You could then do this:

home the machine

manually set the x0 y0 z0 to the desired spot.

send a G28.1 or G30.1 to memorize that location.

send the G10 L20 P1 X0 Y0 Z0 command.

On subsequent carvings, you could then do this:

Power on the machine, and connect.

home the machine

send a G28 or G30 to return the spindle to the previously memorized location.

send the G10 L20 P1 X0 Y0 Z0 command to reset the work zero to that location.

Is that kind of what you are looking for?