No tolerance for the tolerances!


(Shawn Swan) #1

First let me start by saying I LOVE my shapeoko! I’ve had it for a year and a half and I’m on it most nights. I’m having a problem and I’m getting tired I’ve my work around, wondering if anyone can help. I’m using vcarve pro to make my files and save them using the shapeoko mm processor.
My issue is when I cut a specified width it always comes out smaller than I wanted. Like tonight I’m trying to cut a slot to slide over a board that is .45 inches thick. I made the slot .46 inches wide. When it cuts it comes out .43 inches wide.
Any ideas??
I’ve been working around it by using the allowance offset found in the create profile toolpath menu. This is not fun when im trying to do inlays.
Any help would be greatly appreciated.
Thanks.
Shawn


(mikep) #2

Already calibrated against belt stretch?


(Shawn Swan) #3

I never thought of belt stretch. Would temperature affect this? It’s cold in the shop right now, between 5 to 10 degrees Celsius


(William Adams) #4

We have a bit on this at:

The biggest thing to check is effective vice nominal endmill diameter.


(Shawn Swan) #5

Endmill diameter .125". Confirmed with digital caliper


(mikep) #6

Will is pointing to how to calibrate for belt stretch. When you tighten the belts, the stretch. How tight they are is very difficult to control, and the number of steps per mm is therefore a little different on each machine. There’s a procedure to correct the controller’s steps per mm to compensate. If you need maximum accuracy, you need to do this any time to change belt tension. I haven’t found temperature to make a big difference, but over time the belts get loose and need to be retightened.


(Phil Thien) #7

.03 over a half inch is likely bit deflection.

Check for belt stretch, yes, but…

Change form a climb to normal cut and the bit will deflect in the opposite direction. Or consider a small full-depth last-pass.


(Shawn Swan) #8

YOU WERE RIGHT!! I used conventional and it cut it bigger. I wanted the slot at .46 and I got .48.
This will help for inlays, I can do the outer cut in conventional and the inner cut in climb. Just tested and it worked perfect! Thanks for your help!


(mikep) #9

What this is really telling you is that your feed rate is too high. .015" in deflection (x2, one for each side of the slot) - is a LOT of deflection and going to break tools. Gwizard recommends less than .001".

There are some materials that cut better with climb, some that cut better conventional. Depending on that difference to get things to fit is going to cause a lot of tail chasing as you touch different materials (even different hardness woods) and the fit changes.


(Phil Thien) #10

So it is a .125 bit. Spiral or straight? What are your depth of cut, plunge speed, and feed speed?


(Shawn Swan) #11

Spiral .125 ballnose
Depth .125
Speed 16000 rpm
Feed 50 inches/min
Material MDF


(Phil Thien) #12

What instrument are you using in order to measure the slots you’re cutting?

And how deep are these slots and why are you using a ballnose instead of a straight cutter?

I ask because anything in the hundreths (.003 would be nearly 1/32") seems like pretty extreme over .5" or so wide, I wonder if you’re getting an accurate measurement.


(Bryan Haring) #13

I agree with much that has been said but i have also found that finishing passes are very important and for the high tolerance areas. Say i am cutting a slot i will leave .040" and do the final pass with ramps to reduce any bit deflection. Hope this helps!


(Shawn Swan) #14

Using a digital caliper to measure
The slots I’m making (trying to make) are .46" wide x .5" deep. Cutting all the way through .5" mdf so cutting .6" deep to clear the ball. I could be using a straight cutter but I’ve got a ton of ballnose.
Even if the measurement wasn’t accurate, it’s not close to fitting when I try to fit it.


(Phil Thien) #15

Yeah but “not close to fitting” also doesn’t provide much help, as a part that is .001" too large will feel miles apart when it comes time for assembly.

I only bring it up because you indicate you cut .46 climb and got .43, then you cut .46 conventional and got .48, a difference of .05, a difference approaching 1/16th, which would be causing all sorts of problems.

Sounds like things are working to your satisfaction though.


(Tim Foreman) #16

If you are getting major size differences in climb vs. conventional cutting then you need to work on your machine. Something is loose.

Make sure your belts are all tight.

Make sure there is no play in the wheels - adjust the eccentric nuts so there is no wiggle.

Especially look at the Z axis and make sure there is no play anywhere.


(Shawn Swan) #17

I finally got back out to the shop to run some more tests… and it’s fixed.
The wheels were a little loose on the underside of the Z tram so I tightened those up against the aluminum rail (not too tight though). Then I raised my dewalt router up as I had it hanging all the way down, now it sits mid way up. Ran a test And it worked PERFECT!
Thanks for eveybodys help. Greatly appreciated. Now, back to playing!