Calibrating holes more accurately

I cut these holes in .0284 aluminum. They are supposed to be 18/64” or .281 inches. As you can see they are oval. The shorter side is on the x axis (left to right) .279. I calibrated my machine to .003 inches using the calibration method that AVIDCNC recommends. Can someone help me make thes more round please? I think that the feed speed for the x/y movement seemed a little fast. I haven’t tried slowing it down yet.

  1. What was the CAM package used?
  2. What was the feed rate and speed of the spindle?
  3. How thick was the aluminum?
  4. End mill specs?

I used Vectric Vcarve pro 11.5 to generate the Gcode

18000 rpm 100in/minute

Aluminum thickness is .0274 inches

Amana #51478-Z SC up cut spiralO aluminum 3/16” bit, single flute. I took a photo of the endmill specs. They are highlighted in yellow

Thank you.

1 Like

What is your workholding? The speed and feeds are ok. Is it lifting?

Which size steppers are you using?

While down cut end mills are rare in metal they are actually used extensively in sheet processing just for this very reason. The holes are so large and close together you would need a high CFM flow-through fixture but that is hard to get in our budget range. Use the blue painter tape stuck to the sheet and then to the spoilboard with the sandwiched of superglue is best option.

1 Like

Slow your feed rate about 25% -50% and lower your spindle RPM.


Nema 34. It is lifting. The stock is 12” round. It is held in place in six locations on the perimeter with screws and washers. I was going to use double sided tape. I felt that it would gunk up the aluminum scraps and make a mess. I am using a fog buster with denatured alcohol.

1 Like

NEMA 34 are the way to go. I am completely convinced the money you save by going NEMA 23 is lost on the frustration of the shortcomings.

Ok, it looked like lifting but you can never be sure from photos. You can try the down cut and that might help.

That is why I never use the double sided tape. The blue painters tape seems less gooey. Its twice as much tape and then you got to super glue it but it works really well in place of flow-through fixturing.

I don’t know your CAM package but what I do is I set my Z 0 at the top of the spoilboard in Fusion 360. That way I am cutting in the positive as oppose to going into the negative. It saves your spoilboard but in this case, glue buildup on the end mill.

I touch off to a double painter tape on the spoilboard, Then I am barely nicking the tape and my end mill stays clean.

I have a flow-through fixture table for most of my sheet processing though. As soon as the tool carousel is done I will publish the plans to build one. They aren’t complicated to build and keeping a few rules in mind they almost always work better than tape and super glue.


I am going to try the tape and cyano combo. I ordered the downcut bits. I appreciate the help. I will let you know how it goes. All the best.

1 Like

Yes, please do follow up. As much as I would like everyone to think I am always right :disappointed: I am only right about 1% of the time… :rofl:

And, if that does help you please do mark my post as the solution. It helps other diagnose their issues. Of course, if I am wrong… well. My glasses where dirty or something :wink:

1 Like

Another thing to look at is how you are setting up the ramps in VCarve and your plunge rate. If you are using a plunge rate that is really slow compared to your feed rate and a smooth ramp distance that is less than the circumference then there will be a sudden increase in feed rate during the cut that may cause what you are seeing. I usually set my plunge rate equal to the feed rate (about 60 IPM for aluminum) and use the spiral ramp function in Vectric. You will have to select the advanced settings option in the Profile Toolpath settings to see the spiral ramp option. It will take longer to cut because it will require and extra pass but I get a very smooth and accurate result in both aluminum and brass.

1 Like

If this were my situation, I’d start at the machine.

  1. How good is my backlash and calibration? Jim Neebs has a good video on setting backlash and calibration of the Avid using Mach4.

  2. Is the machine square, I used the Avid method, but increased it to a 40” square using a 1/4”x1” aluminum bar with drilled and reamed hole and a test indicator mounted along with using steel dowel pins.

If the machine is relatively square. I set the backlash then calibrate (so I don’t introduce any backlash into squaring the machine), then square the machine. My holes are round and in the correct positions within reason. If any changes are made, verify the preceding and also verify multiple times for repeatability (aka piece of mind).

With the machine all up to par, you can now look at the programming and speeds and feeds.


I really like the idea about the 40" square. I will do that and check out that video as well.

I ordered some downcut aluminum cutting bits. I will give them a try.

I also feel like the feed speed and the ramping is key. I do have to cut 470 holes so I know that its going to triple the time for sure So I will try ramping last last because the holes were really smooth without ramping.

I think the upcut aluminum bit is the real culprit but after I run a few tests, I will post the results.

Many thanks to all!

1 Like

They look more wavy than nice ovals, so I doubt if its X-Y calibration. More likely deflection or backlash/something loose. If you cut the same toolpath in MDF or particle board, is it round? What if you slow it down 25% or so? To me it seems a bit fast for that small of a circle if it were cutting wood, so I would think it would be even worse for metal (but then again, I rarely cut metal).

In wood there is no issue. I agree it is a combination of the speed and using the upcut bit. I ordered a downcut bit for aluminum and I will post the results. Thank you