Holes are cutting undersized

I have a project that requires precise holes in exact locations. The holes are coming out undersized, a .250 comes out .2275 and a .50 hole is cut to .485.
This is using a 1/16 down cut bit miked at 1/16.
The holes appear to the naked eye to be round.
I have checked the X and Y movement and they are good using the ruler method and moving the gantry 10mm at a time from Easel. I have used both the inside the line and the cutout options. Same result.

Am I expecting too much in accuracy, if not any suggestions?

In order to get the maximum accuracy of the machine you will need to do two things.

  1. Calibrate the machine as precisely as possible.
  2. Physically measure the bits and use that size instead of the nominal size stated.

For instance, my 0.25" Whiteside Upcut bit is actually 0.245". That may not sound like a lot, but it makes a big difference when you are chasing accurate cuts.


Brandon Parker

Regarding fine-tuning your step/mm value in GRBL its adviced to jog/measure over a single large distance as possible because this will reduce the impact from the backlash/system flexing component.

Stated Xcarve precision is said to be +/- 0.075-0.15mm

Just asking do you have it set to cut on “Inside” of the path?

Yes on the inside.

I will go back and remeasure the Whiteside 1/16 bit.

So you are saying for example make a line cut of xxx mm and then measure it. I will try that later today.

No, not exactly.

Ideally, use a fine tipped V-bit and a ruler and measure the actual travel of a single jog command, over as large span as possible.
Doing fine-tuning of the step/mm values by doing a short jog (10mm) is not efficient.

As an extreme, say your backlash component is 1mm.
If you try to fine-tune using a 10mm factor the backlash component is large.
If you instead measure over say 300mm or 600mm then the 1mm component is less by magnetudes.

Do the following, calibrating your X-axis:

  • Jog your V-bit all the way to the left
  • Jog 5mm to the right (Reason - the remove backlash as a factor, applies any time axis change direction)
  • Place V-bit point at ruler 0 position (as precise as possible)
  • Jog with a single command the full length of your ruler grid, say 300mm

If you have discrepancy between actual travel vs commanded travel then recalculate your $100 value

Repeat for Y axis.

Ok I follow what you are saying, here it comes BUT. I am using Easel only and am limited to 10mm jogs. Would not making a shallow V-bit cut a precise length give the same results?

You do :slight_smile:
Click the green Carve button and the pane that then opens have a Custom value just below the preset jog distance values.

Here is a good video showing the V-bit/ruler approach:

Over looked that! Thanks so much for your assistance.

The “Custom Value” movement option only being on the actual Carve window and not on the Jog Window is a PITA for everyone. Most newer people to use Easel since the Jog Window’s inception are not aware of the “Custom Value” option on the Carve window which is understandable. For the life of me, and I expressed this in the thread where Inventables unveiled the Jog Window, I can not figure out why they did not add a “Custom Value” to the Jog Window. I mean everyone always wants to move 1.37456" instead of an inch, and from a software perspective it should literally just be to add that component (this coming from a software person… :slight_smile: ). One day, maybe not soon, Inventables will actually realize that people want that option on the Jog Window.


Brandon Parker

Today I went through the process as outlined in the video. Before I started I questioned the accuracy of the included caliper. So how am I going to verify it? I have a set of 50+ years old feeler gauges. I figured they would be accurate enough. The calipers were spot on! Surprise. Then the problem of reading the ruler scale with these 73 year old eyes since I did not have a really fine pointed bit. So I got the sharpest thing I own-an X-Acto knife blade. I super glued it to the dust bracket and it worked perfectly. Thanks to you guys my holes are within .006! I think that is close enough.


this could be bit (or machine deflection). Try slowing your feed way down, and see if that makes any difference.

I find that inside cuts on my machine tend to be a smidgeon small, depending on the bit and the material. It isn’t proportional to the size of the hole though–bit deflection doesn’t how big the hole is.

I just tweak the hole size in the CAD model to get what I want. I think there’s a way to do it in CAM, but I’m certainly not a CAD/CAM ninja. I use Fusion360 and CNC.js for 99% of my work and get very consistent results.

1 Like

Fusion gives you the option to specify finishing passes. Deflection from machine, v-wheels, belt strech, bit deflection can result in undersized holes. Slower speeds and multiple finishing passes helps. I use Fusion 360 to cut mostly .125" aluminum with a .125" bit.