Dimensional Issues with Velox CNC

We just started cutting more precision parts on our Velox a few weeks back. In particular gearbox side plates. Bearings that were designed to be press fit would not fit. A quick measure showed the holes were undersized to the CAD. We then did a few test cuts and found all cuts to be undersized.

Not sure if we are doing something wrong or if there is something wrong with the CNC. Any suggestions are appreciated.

A few more details:

We are using the 4mm endmills from WCP.

Cutting 1/4" aluminum plate

Depth of cut is 0.0625"

G Code is seems to be correct.

We were having the same problems with our 5050. We got this machine a few weeks back. The Z axis seemed to cut twice as much than the values in the Gcode. No idea what happened, but we tuned the steps per rotation and it seemed to work.

I thought velox was supposed to calibrate the machines the moment you got them.

We (5190) are right there along with you-- we bought a Velox VR-5050 and are in the process of calibrating the axis. I will admit disappointment that the machine wasn’t even close to calibrated from the factory. The Z-axis was off by more than a factor of 2. What’s more frustrating is that there doesn’t seem to be any real instructions on how to check/calibrate the machine.

Are you all making a finishing pass? Is it possible that tool deflection can account for the difference? What diameter bit are you using?

This is definitely interesting, it seems people who have bought a Velox recently have been having nothing but issues. Around the time when my team got our’s it didn’t really seem like a lot of people had issues with the 5050.

As for your specific issue, try drilling some holes in a plate and measure if the hole locations are off at all. If your axes are not calibrated then those dimensions should be off as well.

We are using the 4mm endmills from WCP. We are not doing a finish pass and could try that.

I’ve had a few people now suggest tuning the steps per rotation. I guess we can look into that although a lack of instructions from Velox makes that a more difficult thing to do.

FWIW, our Z axis seems correct however we have not tested it as closely as the XY. We are certainly not seeing a 2x issue though.

I’m not familiar with that particular CNC, but I would check the anti-backlash feature on the lead screws nuts. Some are implemented with a nut which compresses to hold the lead screw nut tight against the lead screw. If that gets loose, you can experience backlash. Backlash is when the screw turns a bit before actually moving the carriage. This will result in small, inconsistent undercuts like you are seeing

Drilling holes (first with a centering bit) is a good idea. That will remove any tool flex from the equation. If you drill a line of three or holes with a tool path that progresses from one to the next, backlash should also be eliminated.

I can’t speak to any velox specific things to look at, but particularly on a not very rigid machine I would examine your finishing strategy.

You should be taking a finish pass of 0.005"-0.015" (radial depth of cut). Probably on the lower end of that since this is not a rigid machine. I would also follow that up with a “spring pass” which is repeating the finishing pass at the final dimension to help clean up any material that is remaining due to cutter deflection.

1 Like

My team has the same machine, and we also ran into this issue. We ran a series of calibration tests that showed all of our cuts were off by a fixed value.

We solved this by changing the value of the tool diameter in CAD. We cut with a 1/8th router bit, but in CAM we enter it as a .120" tool. The .005" difference accounts for the error of the machine and gets us accurate parts. This took a few nights of trial and error to determine.

The variance in your error makes me think there may be something else going on, but it might be worth adjusting that value to see if you can get consistent cuts at the dimensions you are calling for in CAD.

We’re a bit new to this so I’m trying to apply what you are saying to HSM. Is this a correct interpretation:

This is pretty much what we started doing on our router, it works very well. The “spring pass” made a big difference.

The team bought a Velox VR-3636 11 months ago. We machined several bearing pockets for 1.125" OB bearings and they were a snug fit using a 0.244" diameter HomeDepot router bit. To get the correct size hole we increased the diameter of the bit to 0.246". Setting 6000 rpm, 15 IPM, 0.035 DOC. We have not tested the linearity of the lead screws which we will need to do before making gearboxes. Overall the team has been happy with machine and we pushed more than 50 parts through the machine last year.

Sort of. You can change from 2 finishing passes to 1 finishing pass. But you do want to leave “repeat finishing pass” checked.

Not sure I agree with Cory’s assertion that the Velox machines are not rigid machines. Sure, they aren’t HAAS Mini Mills, but for a gantry-style router table, I think they are pretty solid.

Spring pass has little to do with rigidity-- the “spring” pass is to allow for the spring/flex in the tooling. Cutters/endmills (especially 1/4" and less) will flex when lateral (side) force is applied. The spring pass is meant to allow the cutter to “spring back” and remove the material that wasn’t removed because of the flex. That’s why I suggested that drilling holes was such a good idea-- no lateral force means no flex and no wondering.

It’s also always a good idea to reduce tool stick-out-- the distance from the bottom of the collet to the end /tip of the tool. A good rule of thumb is less than 4x the diameter and far less if possible. That reduces tool flex, which improves precision and extends tool life.

Here’s a decent article:

1 Like

Running finishing passes is certainly important if you need exact finished dimensions. I have to tune values on my Haas VF-0 at work if I want bearing holes and what not to come out perfect. But I just plan on using a reamer most of the time to clean it up. 1678 sizes ALL our CNC parts with bearing holes to 1.115 in CAD and post ream everything.

Now if it’s drilling holes in the wrong position that is a tuning issue for sure. But you should also drill a large square and check that the gantry is not out of square. A parallelogram could account for this with a little tool deflection and is one of the worst possible issues you can have if you are running mirrored parts.

Many moons ago (early 2000’s), my employer was looking for a new entry level bed mill; something in the $15k range. I found a few and advised the dealers that I would be doing a test cut to check TIR. …they had time to ensure maximal accuracy for the sale.

Using a 3/4" endmill, I programmed (interpolated) a 1.50" round hole in a 3/8 Al plate held in a Kurt vise. The program also made two dead pasess to eliminate any tool deflection. Speeds and feeds were very conservative.
Without removing the part from the vise, I then set up a test indicator to check the circularity.

I didn’t care much what the final hole diameter was as I could compensate for that, but without exception, every hole was not round. Every hole was “egg” shaped by up to about .004" …not 4 tenths!, 4 thousanths. The dealers were all amazed. It’s understood the install tech didn’t dial in the mill (obviously) at a customer’s site and it was a new mill sitting in the showroom.

So, with that in mind. There is no way a gantry router is going to be more rigid than a cheap bed mill, and I doubt the repeatability and accuracy would be any better either. But for most FRC applications, a gantry router (or cheap bed mill) will work just fine.
Perhaps review how well the Velox was initially set up.

IMO, bearing holes are another matter. With non round or off size bearing holes, I think your team may run into other problems that will surface from such holes (alignment issues, premature wear, additional motor load…) If you’re holes are undersized, is there not a tool wear compensation component in either the machine control or your CAD program?

Depending on the software hes’s using, that might turn into 0 finishing passes. HSMworks for Solidworks needs 2 or greater to actually do a discrete finishing pass.
I recommend doing 3 passes: the roughing pass, the .005"-0.01" finishing pass, and finally a spring pass. We’ve been doing 2 passes on our Tormach but I’ve been thinking about switching to 3 to avoid the undersizing issue.
The fix that I’ve used in the pass is to cut 1.125" bearing holes, and mark the endmill as smaller than its actual diameter in the CAM program. For example, the 4mm (0.157") endmill on 115’s router is marked as 0.151" when I use it, to make it try to cut a slightly larger hole. This method works well if you don’t need as good accuracy and want to save time on finishing passes.

The head of the machine will flex as well. That may not be what’s happening, but the spring pass will account for that too.

The Velox may or may not be rigid for what it is, but that’s not really relevant here. Whether it’s rigid enough for the Z axis to not be deflecting due to forces involved in cutting is the issue.

Whether it’s tool deflection or the entire axis deflecting, a spring pass isn’t going to make the problem worse, but it may make it better.

Thanks for bringing up this topic. I hadn’t realized how much deflection there is in a typical gantry router until i tried adding that final zero cut profiling pass (spring pass?) and it removed another .007".

Also trying to learn some new video editing software so here’s a short PSA on the subject:
Adding a finishing pass

What’s interesting to point out is that on our Velox we have never had to run finishing passes or adjust tool diameters to get dimensions to match CAD. We get exactly 1.130" bearing holes (matching the cad) which are pressfit for our Thunderhex bearings (When we got our stockpile of thunderhex bearings the the OD of the bearing was all oversized for some reason-hex bearings will end up having a loose fit in the same hole). I’m no machining expert but I think it may possibly have to do with running 2D Contour (which is what we use for 90% of our parts) over 2D Adaptive since the endmill has material pushing on it from 2 sides instead of only one. When running 2D Adaptive I also tend to see a bit more chatter from the tool too. (I could be completely wrong about this though)