Quick question on dialing in the R7.

Quick question on dialing in the R7. I laid out a 100mm square with (4) 20mm holes, and did my cam operations in Fusion360.

After correcting my single flute mill to 6mm (I don’t know why I put it in as 6.35mm/0.25"), the 20mm holes are perfect.

However, my square is measuring 101mm on each side…

My steps per mm is the stock value (400 from memory).

I just wanted to see if anyone has had to tweak theirs.

Thanks for the help.

I had to make mine off by about .8%. I made it move 30” and measured it very carefully. Interestingly it was slightly different on all axis. By about .02%. Now that I think of it, I replaced the Z screw and did not re-measure it. I’ll have to check again.

I’ve noticed the same issue but went with it because the prices I was cutting weren’t tolerance critical. I’ll be interested to hear someone’s solution. I’m thinking it will be something to do with the 8mm per rev settings. There is possibly a 1% longer cut on the acme thread when it was cut. Most of these hobby machine parts are made in China which we all know is sloppy on quality control.

Someone correct me if I am wrong but the way I understand this is as follows…

Circles and squares put different forces on the bit. A circle has constant engagement with the workpiece so deflects your machine consistently by the same amount. When the machine changes direction when cutting a square, forces on the bit are relaxed in those corners, so the machine ‘catches up’ and cuts as far as it was driven as the bit eats away the last of the material in it’s path.

Either you have deflection in the bit (moving too fast / not spinning fast enough) or you have flex in the machine (something not tight in the axes, have you adjusted the backlash nuts correctly?).

Thanks for the tips – I’ll measure and adjust steps (it was just a sanity check to see if anyone else needed to).

6mm Single flute 6000rpm DOC 3mm 600mm/min (300mm/min plunge) in MDF

As to deflection, I did roughing passes leaving 0.2mm and then finished the holes with a helix bore and the outline with a finish pass. Holes were straight, so I’m leaning towards steps per mm.

Thanks again for all the help!

@Ben_Delarre To avoid the influence of cutter flex I only measure the actual travel of the machine plates. 8*(measured-desired+1) is the correction for Tiny G.

These screws are rolled. So any error in the machine at the factory that makes the screw becomes an accumulated error factor.

Do what @Colin_Kaminski suggested and travel as far as you can on one axis. Measure actual vs theoretical. Adjust esteps by the difference factor of actual to theoretical. Then recheck.

Now this method doesn’t account for backlash, system elasticity, etc. But it should help any compound errors.

For example I run an Azteeg X5 GT controller on my R7. My steps/mm are 803.2 (for all axis). Note I have 4A 1/32 microstep drivers on mine. At different microstep values it would change.

I believe Eric was the first to find this. It is true they are off. Believe one of mine that I recently calibrated was 398.xx, 400.xx, and 399.xx. Agreed go as big as you can accurately measure. Each machine will be a little different.

Gradus M1 – 1/16 microstepping w/ 8mm (theoretical) leadscrews
X = $100 = 395.480
Y = $101 = 396.825
Z = $102 = (didn’t measure yet, so I used Y)

Thank you all for the tips and help! Cuts are square, but a little oversized on the outside and a little undersized on the holes (0.3mm).

I think the last step on dialing in is true cutter diameter. Theoretical is 6mm, but it’s hard to measure a single flute tool.

I have some 1/8" 2 flute ends that will be here by Friday. Hopefully those should be easier to measure.

@Jeb_Campbell , Could you “peck drill” a hole with the single flute and measure the diameter?

@Corey_Perez Great idea! I’ll try in MDF, but I need to get some aluminum in as I might press the edges of the calipers in too far.

But I’ll know more than I do now. Thanks again.


I’d be leery of how soft MDF is (distorting the cut, etc). But, I figured it could be worth a try!

What about the shank, where it enters the spindle end?


@Corey_Perez Sounds like a plan…

So im having the same issue. Trying to make something fit snug but even though i used that formula for commanded distance and actual travel distance and set it up in grbl, my cuts are still a little big. Any ideas? I can carve a whole project and it look right, but when i try to cut something a specific size, its a little off. 45mm diameter pocket is 48.37. Everything is tight and square. Any ideas?