Offline mode changes machine coords. Isn't that dangerous ?

[JeCaWo]

Hello. I have 10-15 years practical experience as a hobbyist. And now this silly question ...

I noticed that the machine coordinates in UCCNC change while in offline mode. I routinely clamp my material somewhere on the CNC bed, then use offline mode to align the gcode with the material. But if the machine coords change during this process, wouldn't that mean the soft limits could be triggered? Or the z-probing could fail, couldn't it?

Which begs the question (after 10-15 years ) what is the official way to align gcode with the actual material location on the machine's bed? [*]
Jeff


[*] I could see how to do it if I can move the machine to the zero x/y point of the gcode. But say the gcode describes a square around (0,0) and I want to specify the top right corner of that square in my material. My past procedure was to physically jog the machine to the top right corner, go offline and move the cursor in the toolpath preview to the top right corner also. Then go online again. My soft limits would be faulty now, wouldn't they?

[JeCaWo]

There is this second use case, where the offline mode really messes with me. I almost forgot:

I cut really small pieces but with several different bits. I spent more time changing bits than cutting. So I wanted to place two pieces of material on the machine bed, and use two separate coordinate systems via G54, G55. Then for each router bit, I'd be switching between the two coordinate systems and cut each one. But if I use offline mode while physically aligning the material stock with the gcode, then I am messing up the alignment of the other. I hope I am using the right terminology here with 'alignment'. Hope you know what I mean.

What is the official way to do this ?

[JeCaWo]

Anybody? Please share: How do YOU align the gcode coordinate system with a piece of material arbitrarily mounted somewhere on the machine bed ? Thanks!

[mickecarlsson]

This is how I do it:
Start up UCCNC, do a Home to zero the coordinates for the machine.
I then clamp down the work piece, move the spindle to the start point where I want it to be, either lower left corner or in the middle of the material.
I then zero the work coordinates to 0,0 (X and y) and then zero the Z work coordinates, either to the machine bed or top ot material.

It all depends on how I set the start of my job. I use Vectric Aspire for my designs.

[JeCaWo]

Yes, I guess with the (may I say "odd" ?) behavior of the offline mode, it is important that you can find the (0,0) point with the spindle. So if you would be cutting a simple square, you'd be better off choosing a corner as your (0,0) rather than the middle. I use Vectric software myself and always felt that the zero in the middle was convenient. Gotta change my habits...

It would be nice if "offline mode" could optionally NOT change the machine coordinates. After all, the machine is not actually moving.

[Nealeb]

You have correctly identified why offline mode is dangerous - the software forgets where the machine is and soft limits can't be relied on.

So, first thing is to home the machine to the home switches and never go offline during the rest of that session. Soft limits now working, and if something goes wrong you retrieve the situation just by re-homing. One problem solved. But what about lining up the "gcode zero" with the work?

This partly why various CAM packages like Vectric allow you to specify where you want to put gcode zero. Make it a corner, any corner, or the centre, entirely to make it easy to locate on the work. A corner is often the easiest choice, especially if you cutting a component out of a larger sheet. Jog the spindle to your chosen corner on the workpiece to match the gcode zero position, set work coordinates to zero, and you are ready to cut. You can repeat for G54, G55, etc as required. If for some reason you do go offline (had to hit estop, maybe?) then you can rehome and all your work coordinates will be where they were, to the accuracy of your home switches.

However, who says that you need to align the spindle over the zero point? Say, your reference point is a mark on a partly-machined workpiece. Align the spindle with the mark, then instead of setting work coordinates to zero, set them to the coordinates of the mark. Or, let's say you already have gcode to cut a 10cm square with the gcode zero in the centre. Jog the spindle to the top-left corner, set work coordinates to X,Y to -5,5, and you are ready to go.

This whole business of work and machine coordinates is probably the area that gives users the biggest problems - you are not alone in this!