Just started using my new shapeoko, with carbide create. When I run my job I am getting all pockets and outside cuts coming undersize by approximately .075" If I ask for a pocket .75" wide by 4" long I get .725 by 3.925
Is there some setting that I need to adjust? I get similar results when I try to cut outside or inside of a line. I am using carbide’s tools and the Dewalt router
Here’s a short exercise demonstrating how to calibrate your machine:
The GRBL defaults get you in the ballpark.
3 Likes
I tried this method to calibrate, instead of a triangle I used a 1" square pocket. After several test runs and tweeking the numbers I got a near perfect 1" pocket .25 deep. Then I ran a test program for a rectangle 4" x 1"
The 1" remained perfect but the 4" was way over size .054" So I changed the settings till I got a perfect 4"
Then I go back and run my program for the 1" square and the width is way under.
Am I doing something wrong here?
2 Likes
I don’t see how you can use a pocket to measure same edge to same edge.
The 4" pocket vs. 1" pocket is probably only including the runout once over the 4" span, hence the discrepancy — you could use math (regression?) to determine what the runout is, but the point to drilling holes and measuring one side of one hole to the same side of the other hole is to eliminate runout from consideration.
Calculate runout/effective endmill diameter by cutting a slot and measuring it.
Calculate how far the machine moves per revolution(s) of the motor shaft by measuring edge-to-edge.
Use the former in your CAM app, the latter to adjust your steps/mm.
1 Like
I just killed a reply that was way too long, so short answer here:
Start with a differential measurement so you are only looking at the machine travel, and cancelling tool size and runout. The holes @WillAdams refers to are for this. I prefer to cut a stepped block for final checks. The last one I did was 8 steps, each step 25mm square, 1mm tall per step. Then I measured each from the same end. The differences should be 25mm. I don’t care about the absolute, only the differences (IIRC, the first step was about 24.4-ish, but from the reference edge to the end of the last was 199.4ish, right what is should be) Just be sure all finish cuts are consistent in cut depth.
Then worry about tool size. I don’t recommend plowing a groove unless hat is what the job will be. Any free play will affect the width of the groove, and I have even seen grooves done this way MEASURE smaller the than the tool (due to the measurement getting the peaks in the surface) on a sloppy machine. Either cut a wider pocket with a moderate finish pass, or cut to leave an island, again with a moderate finish pass. I tend towards an island (usually surface the ends of a block) since outside measurements are a bit easier and outside measuring tools tend to be more accurate in the absolute sense (unless you calibrate with gauge rings). I will go as far as to say that inexpensive calipers (digital, dial, and vernier) are rarely correct for inside measurements. You can directly zero for outside (the faces are clean and touching, it is zero), but for inside, you need a standard. For many reasons, another caliper is not suitable.
2 Likes
Thank you for your reply. I will go back and use the hole method.
So I went back and used the holes at right angles at a distance of 250 mm. It is very hard to take measurements from the outside of a hole to the inside of the hole with my digital calliper but did the best I could. Within .05 mm
Then I went back and ran my test program for a 1" x 1" pocket . Again it was undersized. Then I went and ran my test program for a pocket .76 inches x 3" again it was undersized By .022
Is this the software that is in adequate and does not calibrate property with the equipment ?
I would think that if I am using carbide create with carbide motion with the recommended tool bits from Carbide I should not have to calculate run out on my tool bits
I can achieve the size pocket or hole l want by telling carbide create to give me a bigger hole but if the software is good I should not have to do that! I have the same problem when I want to cut out an outside cut. It will be undersize
Unfortunately, it is not possible for us to order endmills which are guaranteed to be spot on — there’s a specification for an allowed variance.
Similarly, it is not possible to know how true your collet or your router are — that runout has to determined and allowed for.
And of course, there’s the question of how plumb the spindle is mounted relative to the balance of the machine.
Please:
- cut a set of slots along a triangle
- along X-axis
- along Y-axis
- at a 45 degree angle — arguably that should be repeated along both diagonals
and measure them to determine runout
Then pocket three holes and measure them:
- left-edge to left-edge
- front-edge to front-edge
calibrate for steps/mm based on that
Then try cutting pockets using the diameter which includes runout — if you don’t want to do it this way, then work up some other technique, but you have to calibrate for these variations somehow.
This may be left field but if you are using Inkscape and MakerCam there is a requirement to adjust the MakerCam preferences every time you set up a new page.
1 Like
Thanks again Will for replying. When I determine the run out of the tool how do I adjust it in the software? Or do I add or subtract it manually each time I layout a design? For example I want a 1" x 1’’ pocket , I know the tool is undersize by .01"( it is supposed to be a .25" end mill but only carves a hole .24" wide) do I have to Tell Carbide create to carve a hole 1.01" x 1.01" to get a 1" cube? Or do I create a custom size endmill .24" add it to the library? Or some thing else?
2 Likes
Create a custom endmill in Carbide Create.