Probe Z - Different Results Each Time

Accessories Touch Probe
1

I’m working on a project that I’ve cut several times. The past few times, I’ve had an issue that the Z height when I go from my 1/4" down cut to my 1/8" down cut are different. I’ve previously just ran one of the cuts again, but I’d like to figure out why.

To test, I just probed for Z on the 1/4" bit and then swapped to the 1/8" bit and probed Z again. The Offset for the 1/4" bit was -4.159 and for the 1/8" bit it was -4.29. That’s a big difference. So I’ve kept swapping the bits to see how much the results change. I’ve also just moved the bit to a slightly different location on the probe base. Below are my results. Both bits appear to be clean, and the board is flat, and I’m testing from the same general location each time. I’m not new to Onefinity, but I’m at a loss. Am I wrong to expect the Offset to be pretty darn close each time I test the same bit and another bit on the same piece of material?

1/4" Bit Z Results:
-4.159
-4.029 (Changed bit between tests)
-4.031 (Moved bit slightly and retested)
-4.028(Changed bit between tests)
-3.994(Moved)
-3.995(Changed - Bit inserted all the way in collet)
-4.152 (Changed - Bit sticking out more than I’d normally have it out)
-3.604

1/8" Bit Z Results:
-4.29
-4.288
-4.299 (Changed bit)
-4.299 (Moved)
-4.035 (Changed - Sticking out of collet more than normal)
-4.506 (Changed - Pushed all the way into collet)

3

The offset will likely be different each time you change a bit. That’s why you probe, so it can figure out how far the bit is sticking out of the collet.

1 Like
4

I thought the offset for the Z would be the top surface of my material. Is that not the case? To be honest, in the years I’ve been using my Onefinity, I’ve probbed, cut, and given the probing very little thought. If it wasn’t for my depth of cut being different between my 1/4" pass and my 1/8" pass, I still wouldn’t be giving it much thought.

I’ve recorded the Offset values on the X and Y before to make sure I can always return to the lower left hand corner of my project when I’ve had to Probe to a different part of my CNC bed for a different project while I was in the middle of another project. That’s always stayed constant for that given project.

5

The offset is just that - the offset from z zero due to variable bit length.

1 Like
6

If that’s the case, is there any way of looking at the UI on the controller to confirm that both my 1/4" bit and 1/8" bit are going to be cutting starting at the same height (Z level)? I know my design will control the depth, but I’d like a visual way of knowing that two bits will end up bottoming out at the same depth.

7

Could use mdi to move to z zero to confirm. Command is “Z0”

2 Likes
8

I’ve never used the “Z0” in the MDI. It looks like that lowers my bit to what should be the top of my material. To be sure I’m understanding, are you saying that I could do this with the 1/4" bit and then with the 1/8" bit to make sure both are going to be starting from the same height after I swap out bits?

9

It will move to wherever you have set your zero height. Yes you can do between bits to confirm consistent height.

2 Likes
10

Thanks for the tip, I’ve never known an easy way to accomplish this. And using the MDI and “Z0” is about as easy as it gets.

I just did that and both bits appear to be visually at the same height. However, when I did a quick test cut, I can still tell the difference between the first clearing pass with the 1/4" and then the pass with the 1/8" bit. So I still have something going on. I’ve used clearing passes before, and on this same project, so I’m not sure why they’re not cutting at the same depth.

1 Like
11

Is your clearing pass set to leave a little material for the final pass to clear?

1 Like
12

How can you tell the difference?

The difference it probably negligible, in the range of a few hundreds of a mm.

It could for example if some dust get under the probe or the wastboard is not perfectly straight and you don’t probe in exactly the same spot.

A toolsetter should be more precise.

13

Here’s a picture of my test. If you look along the edge of the maze, you’ll see where the 1/8" bit runs and in the middle of the maze, you’ll see where the 1/4" bit is cutting a little less deep.

image
image896×936 140 KB

And here are my settings from VCarve for this pass:

image
image404×946 87.7 KB

14

Just wanted to throw this out, where I think there may be some confusion between the terms “offset,” “Z height,” and the “zero point.”

When you “home” your machine at startup, you’re not only setting its absolute travel limits for all axes, but technically, establishing a reference point known as the “G53 offset” in GCode.

When you use the touch probe to find the left, right, and top surfaces of your material, you’re creating a new offset, named “G54.” From this point on, this becomes the active offset for all machine movements, whether they come from your exported GCode (e.g., Vectric) or manual jogging.

After changing a bit, you re-zero the Z-axis using the touch probe on the top of the workpiece. This updates only the Z-axis component of the G54 offset, just as you did for the first bit after homing.

If/When you incorporate a tool setter to your workflow, it simplifies bit changes. You still use the XYZ touch probe for the first bit to establish the material location, however, for subsequent bit changes, the machine uses the tool setter to automatically measure the height difference of the new bit. This process is quick, reduces error, and happens automatically when you start the job.

Tip for Z Probing
Since I don’t yet have a tool setter, I’m mindful of where I probe for Z-height after a bit change by avoiding probing an area that has already been cut. For example, if you initially zeroed at the center of the workpiece but cut into that spot, subsequent probing there will yield inaccurate results. Instead, choose a consistent, untouched reference point—like near a clamp or the edge of the material for all Z-height measurements. Or, you could always zero your Z-axis from your machine bed instead of the workpiece. Just make sure you update this reference in Vectric!

We can go deeper into the differences of moving the machine within G53 or G54 coordinates, including an example of how and why I do so, but to answer the OP question, the reason why your values change when probing after bit changes is because your new bit has physically changed position in the spindle in reference to the previous bit.

4 Likes
15

You’ve reminded me of a problem I had that is very similar. When changing the bits I was not getting the exact depth of the first bit. Turns out that the wood had shifted a bit upward and my z-probes were now off by the amount of the shit of the material. Something to look for too.

16

I found the same thing when using the 1/8" to get a smaller radius in the corners.
So… I want to pocket a 2" x 4" x .300 slot.
I use the .250 as rough and .125 as finish but… I will use an offset of .003 and finish depth of .297.
Then I will do another pocket with the .125 ( it is already in the chuck… DO NOT CHANGE ANYTHING.) Now I will use .000 offset and finish depth .300. I have found that running it at 500 IPM, step down of .010 (it really doesn’t matter) and step over of .012, equals zero sanding. Sometimes I may run the finish twice. Depending on the wood I may use a .005 offset and -.005 depth with the first poclet.
PS The start depth of the second pocket will be .002 above the the finish depth of the first pocket

17

@GeraldSmith Thanks for passing along that tip. I’ve never thought about doing it that way, but this sounds perfect. I ended up chaning my project to use the 1/8" bit for the entire cut. It took a lot longer, and I’m always worried when I use an 1/8" bit to clear that much material, but it fixed my problem. Next time I cut that project, I’ll be borrowing your suggestion. Even if that were to take the same amount of time, it would be worth it just to protect my 1/8" bit.

1 Like
19

Thanks Jeremy

The time will be a lot less than using an 1/8" for the whole thing. I found that the savings of the sanding was huge, especially when it is inside surfaces.

Have fun my friend.

1 Like
20

I have found that probing off of the wasteboard instead of the workpiece helps alot.