Hole size less than wanted, what to check?

Hi,
I did a first run with my primo (skrpro2209dual fw509) to make holes in spoilboard, to fit some t-nut
image
20 holes
image

like this:
image

T-nut largest part is about 19 mm
so top hole 20mm wide should be good…
No, I get less than 20mm, and need to redrill at 20mm to make the t-nut fit

I’m running this 6mm dual flute ( https://www.amazon.fr/gp/product/B07DBC6DKP/ ) into 18mm MDF
after run, I checked the bit, it’s really 6mm

any idea of something to check ?

I had the same.problem running to fast slow down? You could try a finishing pass also

1 Like

Imo first thing to check is that when you command 20mm you get 20mm. @dkj4linux uses a BBQ skewer or toothpick pointing at a ruler for some of his machines, i clamp a dial indicator on mine. Use the largest implement you have that measures to the accuracy you want. The key is to do this under no load.
Stepper motor angle, pulley diameter, belt tooth pitch…these are all well defined so it should be really really close. If not, you could have other issues. There was a discussion not long ago about the belts stretching and maybe the pitch isn’t exactly right. If you have a small error, this could be it. Might warrant messing with the steps/mm, might not. Personal choice.
Sounds like you’re confident the mill is actually 6mm.
Could be the stock is deforming a little. I think mdf pushes back a little, but it might just be me. When you cut a slot, it’s it 6mm wide?
The last thing is deflection from the tool mount, core, and tubes. That problem you fix with extra finishing passes (as already mentioned), the other ones you fix with “stock to leave” settings.
I generally have to remove an extra 5-10thou depending on the cut direction and material. Good luck!

2 Likes

Thanks for your idea,
I did a quick test with a V-bit (with spindle off) and a school paper sheet

  • homing x0 y0 and get Z low enough to mark paper, then rise it
  • send G0 X550, mark paper
    The same with Y axis
    As I mesure I get approximatively:
    X : 549.5 mm (for 550 asked)
    Y : 520 mm (for 520 asked)

I’d be happy with that! I guess the rest must be some combination of material ‘springiness’ and machine flex.

2 Likes

Quick questions… just how much smaller is the hole? …and is it at all tapered top to bottom?

Since your hole is undersized, the runout/etc is probably OK, but the bit/machine is flexing too much. The endmill you are using is the kind with a smaller shaft (not 1/4" shaft). You might try an endmill with a 1/4 shaft… or slow it down… or give it more finishing passes. Also, verify your core bearings are snugged up properly… they can have a habit of sneaking loose and causing problems like this.

1 Like

What tool path did you use to make your holes? Did you use a Bore or something else?

1 Like

Hi Kev, thanks for your ideas,
I’ll check core bearings
I use a old Bosch POF50 small router which needs a 6mm tool shaft
I also noticed a little burned side in the wall hole,
Maybe mdf has overcooked and shrinked … :slight_smile:
Later this day, I will try to mill a pine board with many holes, and to do precise measurements.

Hi Robert,
I’m using fusion 360 like this:

Hi there!
While head scratching how to make a test pattern board,
I think I found the reason in fusion :slight_smile:image
I’ll try this soon and let you know

seems to be called “stock to leave” in english

3 Likes

Ah yes hehe, that setting defaults to on and drives me crazy all the time. Good job finding your solution, and good luck on the cuts.

1 Like

Yeah, we talked about using that to fix the problem, but I didn’t guess that it WAS the problem!
I think the fusion default is to leave stock on roughing strategies like pocket and Adaptive. Finishing strategies like contour and parallel usually don’t.
Glad you’re on the right path now!

3 Likes