What would cause my x-carve to jog during tab plunges?

For some reason my x-carve tends to jog (very slightly) the x and y axis during plunge operations such as tabs, ruining the outer profile cut of projects. I’ve taken to just not using tabs at all because of this. What exactly causes this problem? I’m wondering if it may be a voltage issue for the stepper controllers. I would seem to be indicative of runout, but I’ve put a dial indicator on the collet and that’s not the issue. Has anyone encountered this before?

I will preface this with the fact my machine has been fairly meticulously calibrated and my Z axis has been trammed to nearly perfect. I have searched other posts and it seems some have encountered this with slowing down the z axis. Is this just a limitation of the factory Z?

That sounds either like something is loose, or bent.

Unfortunately it is all very tight. All of my calibration cuts are spot on in every direction. My V-wheels have no play and my belts are all tightened to the same tension.

Does this happen with Gcode as well? It would be easy enough to rule out any sort of issue with that by checking the code.

no the gcode doesn’t have anything but a z axis movement during the time I’m getting the cuts in the profile. Basically, it encounters a tab, z axis plunge down, grazes the outer profile, z axis moves up, machine transitions the other side of tab, plunges down, grazes outer profile, moves up, continues. It seems to be in both directions up and down, but only when the z axis is moving. I was concerned if it may be something relating to the steppers having a sudden stop and start between the plunge. Just a theory, I do not know.

Could it be noise from the stepping signal to Z that is picked up by X/Y?

That sounds logical to me, and is also a concern. Another thought is since tab plunges are a fairly violent movement in the scheme of things (machine transitions across the profile, instantly stops, plunges, instantly accelerates) could I possibly be losing steps? I may try to just slow down the z axis or do some tests with lower feed rates. It just seems kind of silly to account for such a very basic toolpath. The machine is 3d carving hardwood for a few hours flawlessly with the Z in constant motion, and then screws up on a simple vertical plunge, quite odd.

I had a problem with flex along the Y axis when doing plunge cuts which would make them oval in the Y direction. I added stiffeners on the Y axis rails which improved that a great deal. Do you have the wide makerslide X axis? What physical mods (if any) have you done to the machine?

An aggressive plunge (like when the cuts for the tabs are done) can cause the bit to deflect leaving scarring on the profile cut…usually a vertical line at the beginning and end of the tab. Having the least amount of the bit sticking out of the router can help as can slowing the plunge rate.

You mentioned 3D…are you using Vcarve? If so, use 3D tabs and see if that helps any.

Also, is it always the same axis or just the axis not moving? For instance, if you’re going from top to bottom, is the movement left to right? And if going left to right, is the movement top to bottom?

If so, it might be auto torque reduction showing it’s drawback of the axis not in motion having significantly less torque.

I’m assuming you’re using an Xcontroller. If so, search for how to disable auto torque reduction.

You could try a run with rapid feed rate at 70% of current value and set acceleration to 50% of current.
In case the rates are a little too high.

However, it may also be coming from flex - or lack of sideway force during Z plunge/retract, causing a “dimple” at the plunge position.

Okay, so that is what I suspected is the issue - runout. I haven’t run by bits all the way into the chuck just because I know that can induce more runout depending on the chuck style. I guess you’re saying the sudden plunge can transfer lateral energy into the bit? I could see that causing a momentary oscillation possibly, and it only needs to occur for a split second - enough for it to kiss the profile of a work piece.

I use aspire and fusion 360. I probably should try the 3d tabs, that’s a good idea. I think I used them once and dismissed them as being a gimmick. I haven’t been able to tell if the jog is a particular axis or aggravated by a particular moment in relation to another. The only correlation I’ve drawn is when the bit is plunging on a straight Z axis movement. I’ll do some tests and see. I did just swap out to a Makita spindle, so it’s a good opportunity to test just the spindle before messing with some settings.

yes I have the newer machine with the single extrusion gantry. I don’t have any stiffening mods done, but I can’t imagine that should be necessary to get the thing to plunge without flailing around 1/16th of an inch. :slight_smile:

1 Like

So, I found this thread by changing around keywords:

that is just about the same issue I’m having, the OP never confirms if or how he fixed it, but it does seem like the consensus is deflection and possible solution in 3d tabs. I’ll give that a shot, it makes sense.

3D tabs. It’s not a gimmick, they are better.

Your carve will slow down to move the Z axis (like it does for a 3D carve) but its much better than creating those witness marks.

If you’ve got a linear Z axis and messed with the Z acceleration at all, you’ll barely notice the motion.

yeah now that you mention it, it makes perfect sense. I’ll give it a go.

The beefiest bit you can use for the profile cut helps with deflection as well. I try to use a 1/4" endmill for profile cuts if the design allows it as it less prone to deflection.

also a good idea. I had just gotten accustomed to using my 1/8" straight cut two flute, but since it’s a profile cut I might as well be using my 1/4", there’s no reason not to.

1 Like