Z Randomly Raises During Job Run

[jimwilde1]

When running a sign, the machine will randomly change the Z setting such that it raises it. It starts out cutting a letter, then the one next to it only gets lightly cut (not deep enough). When I cancel the job and return to XYZ zero point, I find that the cutting bit is now about 1/8” above the material surface. Am I bottoming out the machine somehow? Settings ? What am I doing wrong? Sometimes the machine cuts perfectly. Not sure what’s going on. Any help is greatly appreciated. I also have a note into the helpdesk. Thanks. Jim.

[ohiolyons]

So the raising up issue is the way this software just works. There are 100's of posts where people complain about this. There are ways to minimize raising and lowering, but you are the mercy of Vectric's optimization algorithms. I quit worry about it, bigger fish to fry.

The bit being off in the Z by an 1/8" is not software related.

1 You didn't tighten the collect nut enough.

2 Slippage is the machine itself, belts not tight enough, screws loose, etc.

3 Stock not flat. (Letters not cutting same depth next to each other.)

4 Pushing your machine too fast in X and Y.

5 Etc (anything else involved with the process)

Edit 1

6 Static electricity, is your machine grounded properly?

Edit 2

7 Are you turning your dust collector on and off during a cut? Grounding issue.

8 Do you lean on your spoil board while watching the cut?

These may seem silly, but we all know a guy who has done at least one of these.

[martin54]

As ohiolyons has said there are a lot of different reasons for lost steps & it is really a process of elimination to work out what it is, work your way through the list given to see if that helps. This is a subject that comes up quite often so a search on the forum for lost steps will bring up a lot of posts which will contain info on what you should check

[TReischl]

As others have mentioned, lost steps. From what you describe it sounds like Z axis.

Here is something to consider:

The type of bit itself. Typically "end mills" come in three flavors. The first is a true router bit, not an endmill, but it sure looks like it will do the same job. Then there are the true "end mills" which may or may not be "END" mills. Some are end cutting, some are not. So why is this important?

If you attempt to plunge a non end cutting bit straight into the work you will put a heckuva load on the Z axis. This can result in lost steps.

I use the zig zag option to plunge all my end mill type tools. Yea, it is terrible, takes longer. Like a few seconds. But that sure beats spending hours trying to figure out what is going wrong. If I am doing profile cuts I always use the spiral ramp option. Yup, that effectively lengthens the time somewhat.

If you are using straight router bits it is almost guaranteed that they are not end cutting.

Soooo, since I am incredibly lazy by nature, I would start trouble shooting this issue by altering the cutting technique. Failing that, I would then move on to slowing down a bit. If your axis is "bottoming out" then the problem will continue no matter what you do to fix it in programming.

[adze_cnc]

It starts out cutting a letter, then the one next to it only gets lightly cut (not deep enough). When I cancel the job and return to XYZ zero point, I find that the cutting bit is now about 1/8” above the material surface.

Let me verify: the first letter (A) is cut properly. One part is not noticeably deeper than any other (i.e. it doesn't "fade" out)? The second letter (B) is similarly consistent only shallower? At the end the Z axis has gained 1/8".

So, somewhere between moving from letter A to letter B there is a loss (or gain if you like) of 1/8" ?

[GEdward]

I'm guessing that your HD520 is fairly new and that you got the spindle option. If that is the case then the spindle comes with either a ER16 or ER20 collet and along with the package you likely got two collets. Z axis shifting upwards is not very common and I suspect one of two things. Either TReischl's suggestion that you are using a bit that is not designed for plunging or ohiolyons suggestion that your collet is not tight enough (or you are using the wrong size collet, like maybe a 6mm tool in a 1/4in collet) are the two most likely culprits.

It looks like the Z axis motor couples directly to the lead screw on your machine so belt slippage is not an issue. I believe the HD520 has homing capability. If so, you can check for lost steps by homing the Z and follow up by checking Z zero on your project. If after homing, the Z is correct, then you have lost steps. If the Z is still above the part then the tool slipped up into the collet OR the spindle motor slipped up in the mounting bracket.

Hope this helps.

Ed