Avid Support is working with me to fix this issue, but I’m wondering if anyone else has experienced it. Very uneven flattening in the Z axis. Anytime I do a pocket like this, especially with raised lettering, I get very uneven lines in Z. I’m using VCarve.
(Material is not moving. I’m only cutting into it maybe .05 per attempt.)
(Using a double flute 1.25" flattening bit, and a .25 straight flute.)
(Machine was trammed properly a while back.)
(I have decreased acceleration.)
(Have upgraded software per Avid to newest and reset profile.)
(Laptop is dedicated and exceeds all specs.)
(Collet tight with no slippage, also tried new collet and nut.)
Some ideas based on the photos:
-
Can the metal be rising up off the table a bit, maybe by being pulled up into the bit?
-
Grab the collet (while it’s in the spindle) and try to wiggle it, in case something has come loose.
-
Check for vertical backlash in the Z axis. Might need its internals tightened up. If so, the collet would “wiggle” up and down.
-
Make sure both bits are properly tightened into the collet. You could measure their stickout with calipers before/after to see if one is, for example, slowly getting pulled out of the collet.
You could also go to a specific X,Y,Z location on your machine and manually measure the height of the spindle, before and after, to see if the machine is losing steps. Similarly, touching off the bit before/after and comparing the results would show any collet problems.
I’m interested in what you find out as my most recent sign project did the same thing for the first time but not quite as obvious. I tried various travel speeds as well as spindle speeds making sure my chips appeared appropriately sized.
Hey. Thanks.
- Material held down well, no lift.
- Collet tight.
- Unaware of any vertical backlash.
- Bits tight.
I’m going to do the “air test” you mentioned.
Have you tested it with a dial indicator? I would wonder if that would cause this type of issue.
I get the same thing but not to the same degree.
1 Like
This is very common when pocketing, and there’s some debate over the root cause. There are also a lot of variables involved - the most common being the method used for setting Z zero after a tool change. If you’re not using a touch plate to set Z zero, it’s very easy to be off by a few thousandths of an inch (hundredths of a mm) in Z zero. Even if you do use a touch plate, you have to then account for the accuracy and repeatability of the Z zero routine and the touch plate you used. The geometry of the bits, machining strategy (raster vs. offset,) machine backlash, and a ton of other variables are involved as well. In other words, it’s quite possible (and quite likely) that your machine is fine, and you’re not really doing anything wrong.
Frankly, about the only sure-fire cure I’ve found for this type of issue is to add a textured background to the pocketed areas. Carving the texture into the background removes those tool marks. I know that’s not always an option, depending on the client/customer’s wants. In that case, we’re pretty much stuck either carving the entire pocket with one bit, or doing a lot of sanding.
Thanks for the response.
No tool changes have been done in these examples.
This level of inconsistency in CNC is totally unacceptable, even in flimsy machines. I’ve used multiple CNC routers and never had anything close to this level of inconsistency. CNC should, and generally does give extremely flat pocketing with very minimal tool marking and minimal sanding required, like my previous machines.
I think we all agree with you. In my case, I’ve done large pockets in red oak with near-mirror-finish results, on a 5x10 machine, and that was before I finished tuning and tweaking the machine. It can be done.
There’s something wrong with your machine, setup, or process. Keep checking things and eventually you’ll find it.
Thanks for the response. These cuts were done on an Avid?
Yes, I have an Avid Pro 5x10 with a CNCDepot 3HP ATC spindle.
In your original post you said the pocket was done “Using a double flute 1.25” flattening bit, and a .25 straight flute." There’s a tool change involved there. Hence my comment on resetting the Z zero after the tool change.
I’ll agree with djdelorie that there may very well be a problem with the machine (backlash, etc…) or the setup, or the process. That was my overall point. This is very common, and that there are a ton of variables that could each contribute to the result you got. I too would keep checking things off the list as you go through them.
Hey. Thanks for your response. I should have been more clear. There are 4 pics, 2 each of different cuts. One cut was used using 1.25 only. The other cut using .25 only. I was just seeing how differently they’d look with different diameters.
I’m glad to see other people getting very nice cuts with Avid machines. My experiences using several other CNC’s have lead me to believe this issue is machine specific. I’m used to getting extremely flat pockets and hope to be able to again with this machine. Thanks again.
When I was experiencing this issue. It came down to the spoilboard. To correct I torqued down all the bolts with large thick fender washers to the same spec. Then I added a second layer glued to the first. Surface that and I have been good ever since. The only time I have it now is on tool change. I am sure then it is my setting the height at fault. Thanks again Mark Lyndsay for the torque and washer advice.
1 Like
I know this post is old but I’m wondering if you were able to figure anything out. I am experiencing the same thing in hardwoods and have exhausted Avid’s support assistance in the matter. I used to have an Axiom and it was capable of making nearly mirror pockets so I believe it is the Avid and not me at this point….
This is a key piece of advice, along with recognizing that heat/humidity can shrink/swell your work and your spoilboard. Additionally sometimes when taking huge pockets out of wood can release tension in it and get it to change shape as you pocket.
You can mitigate a lot of this stuff by clever toolpathing… Often times I’ve found that taking a big chunk out of a pocket, and them coming back later and doing a finishing pass can really help.
I have double checked the spoilboard (which is bottom layer of 3/4 HDF - secured to machine frame with spring nuts, middle layer 3/4 birch, top layer 3/4 HDF - screwed together with 2” #10 screws). The issue is occuring on a piece of hard maple measuring 4.5” wide and 13” long. Using a 1/4 endmill with a 0.03” final pass depth. Piece is held in place on 4 sides with stock that is screwed to the spoilboard with 2 hold down clamps on each end preventing vertical movement
I have definitely witnessed this. Usually my material, which seems flat and stable and well secured, will develop a slight bow upwards after I begin cutting. The best way I can think to combat this is a vacuum hold down. Also, if that is foam being cut and/or pocketed, because its so soft, is it possible un evacuated chips are getting ground in to the material to cause marring/gouging?
Here’s my checklist, based on things I’ve experienced:
If you have a toolsetter, make sure it’s parallel to the bed, else different diameter bits will measure different lengths relative to “correct”
Make sure nothing is loose in your machine. Grab the spindle nose and try to move it. If you can move it despite the motors holding it, something is loose.
Try reducing the Z acceleration. Too much accel can cause “dig” when the spindle tries to stop faster than it can.
Clean your router bits and collets before putting them together, and tighten them a LOT. Shipping grease and slipping bits have ruined a few of my jobs.
Check your spindle for tilt and nod. It doesn’t matter if the bit is the right height if it cuts deeper on one side than the other.
If you’re using a toolsetter, try slowing down the probe speed.
If you’re using servo motors, the Z tuning might be off.
The two things that cause this the most for me are (assuming your machine doesn’t have a mechanical problem like backlash or a loose/weak spoilboard):
Pushing too hard on the last pass. An upcut bit will lift the material, and down cut will push it down. This effect can be dramatically different in different parts of your cut. For example, your first cut is the full width of the bit, but your next adjacent cut may be much less (depending on your stepover setting). Straight vs. curves will be different too. When you want a really flat bottom, adjust your toolpath so that the final cut is like 0.030” or something, i.e. just enough to clean up the toolmarks. This is also a good time to ignore chipload and run a little slower feedrate and/or higher rpm.
Material bowing as you remove material. Wood is not stable. Just like when you rip something on the table saw and see the stress being relieved in the two halves, you can get the same thing on a big pocket. Believe it or not, MDF is even worse. It is very hard at the surface and soft in the middle, so if you cut off one surface, it can bow significantly. A vacuum table or two sided tape hold down can help with this, but generally the same advice works as the first item, take a very light finishing pass on the bottom of the pocket.