Centroid issue: Entering tool height offset library changes the Z value of my WCS

[PhoenixMetal]

I recently purchased a used bed mill with a Centroid control, and I am having an oddball issue that I'm hoping someone can help with.

When I enter the tool height offset library, the Z height of my WCS (G54) changes on its own to some seemingly random negative number.

Here are the steps that reproduce the problem:
1. Enter Part Setup, get to the Z axis step, and set the top of my workpiece as Z 0.
2. Bring the Z axis all the way up to home. The Z readout now shows some positive value (for example +7.4226"). All good so far.
3. Enter tool height offset library. The Z value shown at the top of the screen (for my WCS) suddenly changes from 7.4226" to some negative number (for example -4.9495"). The Z Ref value on the bottom of the screen also shows this same number (and since this is a bed mill and I'm not using a reference tool, the ZRef should be 0). Please note that I have not moved the Z axis - it is still all the way up in its home position, nor have I changed the tool or active tool number.

I made a video showing the issue: https://photos.app.goo.gl/UR1X8YAuORYqAe4E3 . The mystery Z number change is around the 2:35 mark.

The unexplained negative Z number is somewhat consistent by the way. If I repeat the process starting with my WCS Z origin on the top of a tall object (for example the 9" high surface plate shown in the video), the Z home value changes to -4.9495, and it will come up with that number consistently. But, if I start the process with my WCS Z origin at a much lower level (for example the bed of the vises in the video which is around 2.5" high), the Z home value changes to around -1.74", and again it will come up with that number consistently. So while it is consistent, notice that the difference between the starting Z origins (6.5" difference) is way different from the difference between the mystery negative numbers that it comes up with (approximately 3.2" difference). I can't explain it.

I've only been using the machine for about a week, and it worked fine last week, but now I have this issue. Any ideas?

Thanks in advance.

Similar Threads:

• Haimer Tool Offset and Z Height Problem
• Tool library offset question
• sprutcam 9 tool library issue, waterline issue, was working fine
• Solved Partmaster V13.5 - Centroid OS & hardware- Tool heights offset - post proc. fix.

[cncsnw]

Note the active height offset (H number) displayed in the status window next to the tool (T) number.

When you set the Z axis Part Zero, the control activates the height offset for that tool, and applies whatever offset is currently in the Offset Library under that H number. For this reason, you should go to the offset library and measure your tools first, so that the height offset which is applied (e.g the value in H1 when you set Z zero using tool #1) is correct.

The reason for the "issue" you describe is that, by default, when you enter the Offset Library screen, the control cancels any active tool height offset. Note again the H value shown in the status window.

Suppose that your probe measures about -12.37" (the distance the head needs to move down from home in order to touch the probe to the tool-measuring block). As is normal practice with a bed mill, you are measuring tool in comparison with an imaginary Reference Tool. Your imaginary Reference Tool is 12.37" longer than the probe (T1/H1), because your Reference Tool just touches the tool measuring block when the head is at Z Reference (which is at Home).

After you set Z zero on the part, and return the head to Home, the control shows that Z is at +7.42" (on the DRO) and that H1 is active (in the status window).

When you enter the Offset Library, the Height offset is cancelled (see the status window). It is as if you just removed T1 and inserted the (imaginary) Reference Tool. Therefore the tool tip is no longer 7.42" above the surface; it is 4.95" below the surface (which, by strange coincidence, is the distance down from your part surface to your tool measuring block).

In short, nothing is wrong. Just measure your tools before you set part zero, and pay attention to the active H offset number in the status window.

See Mill Training Notes and Mill Tool Length Offsets Explained.

[PhoenixMetal]

Hi cncsnw - I think you may have hit the nail on the head - having to do with the height offset being cancelled when I enter the offset library. I haven't had a chance to get in front of the machine again to test this out though.

Maybe the previous times that I used the mill (in which I didn't have an issue), I happened to measure tools first, and then measured my work surface.

I can in general do as you say, and measure my tools first, and then measure the part zero afterwards, however there will be situations in which it has to go the other way around: I keep a library of standard tools that get used on multiple jobs (and the tools are referenced to a tool-measuring block, not the part), so frequently all I need to do to run a new job is measure the workpiece location and start running. BUT, let's say that in the middle of a job (after I've already set the part Z zero), a tool breaks and needs to be replaced, or I need to make a change which requires a new tool to be measured. What to do then?

By the way, your website was a great help to me in identifying the various components in my system - thank you!

[cncsnw]

"Measure your tools first, then set Z part zero" is the simplified, easy-to-understand advice.

The reality is: only set Z part zero with a tool which already has a correctly-measured height offset.

If you have a tool that you measured last week, and you have not done anything to change the length of that tool, and you have not changed your tool-measuring procedure, then you can go straight to setting part zero with that tool.