Im attaching a pic of my test cuts for a mortise and tennon joint. This is just a test piece, no real world application, other than dialing in my new lowrider. It is a mortise and tenon, each of which I drew at 38mm x 19mm. Both parts came out the same dimensions.
The pic shows the target dimensions and actual cut dimensions. The white paper shows how the part is oriented on the machine.
As you can see, the overall width of the part (50mm) is on target for what I would expect with this machine. I’m happy with that.
The Y dimensions for the both the mortise and tennon is also acceptable at 18.9mm
The overall length of the part is 1mm too short (119mm) which is too much for such a small part.
Also Im concerned about the mortise and tennons.
The tennon is about 0.5mm oversize, and the mortise 0.5mm undersize, causing interference.
I would expect a tight fit between these parts, and maybe even a light sanding to get them to fit nicely, but that is too much interference.
The fact that male portion is oversized and the female part undersize by about the same amount, and that the other dimensions are acceptable, makes me wonder if this is some sort of tool size compensation problem or a software setting that Im missing.
The material is 3/4" cedar (very soft), and was cut at 2mm axial DOC (10 passes) and 400mm/min feed. Cutter is 1/8" single flute carbide, brand new. Cut quality is clean with a few tool marks on the last few passes.
I did not use roughing/finish passes. I did a simple 2D contour cut. Post processor was the fusion 360 MPCNC from flyfisher605.
Obviously I could compensate and make the parts fit together by altering the drawing, but I would like them to be closer to “as drawn” dimension, which I know is obtainable because of the other acceptable dimensions in the part.
I’m sorry if I didn’t understand your issue correctly, but I’ve been meddling with joints myself lately. My experience is that I must measure the cut, to get the correct proportions for the CAM. For example, for the strawberry arcs, the test cut showed 3.8mm for a loong 3.175mm endmill. I think the runout varies depending on the specific endmill, depth of cut, softness of wood, length away from gantry and so on…
This is a great description of the problem!
It’s common to get dimension issues: Parts Too Big and Holes Too Small
Your errors are consistent with what I’ve had in the past. Shorter in one dimension and larger in the other (with vs against grain?) but it’s also a little like “outside” cuts are larger than “inside” cuts (parts too big holes too small) which I’ve also struggled with, even to drill dog holes in the spoilboard.
I haven’t found a magic bullet yet either, sorry. I do the same as @turbinbjorn and cut test pieces/holes.
I have done a couple slot and tab fixtures with good success. I model them with zero clearance and the end up as a tight fit. Sometimes I just have to hit it with some sand paper to touch up the edges so they don’t peel on the right fit. I’m mainly using birch plywood.
I did notice my x axis(gantry) was always out more than my Y axis. I seemed to get rid of this a bit by eliminating the zap straps on the belt.
Also finishing pass is critical, try it again with a .3mm finishing pass
I don’t think I would ever adjust the design to meet the inaccuracies of the machine. I would go through all of the typical mechanical checks (belts, bearings, mounting screws, grub screws, skate wheels, etc) first. Then I would test again. Dealing with runout is not so simple and not usually the issue. Two weeks ago if I saw a consistent error I probably would not have seriously considered an electronics issue, but a friend’s recent issue turned out to be defective external stepper drivers. After that I would do what you are doing. See if anyone in the community knows of any unusual things to look for. After making my best effort to adjust my machine (and a final test), I would adjust the toolpaths to compensate for my machine’s inaccuracies.
First, I’ll check for mechanical problems. Slack in the belts will have some error, which will look like backlash. It can also produce wandering cuts.
Loose grub screws make everything look like crap, and can do some really weird stuff.
Bearings not making proper contact with the rails can also do some weird stuff. Basically, make sure the machine is mechanically sound first.
Then I cut inside and outside squares. If you round the corners to a radius greater than the tool radius, it helps.
I then adjust the tool diameter until both inside and outside squares are the same dimension (Typically, I fit the one into the other, and adjust until I get a tight fit.) I try both conventional and climb milling to make sure that it’s not tool deflection that I’m measuring. FWIW, my nominal 1/8" (3.175mm) bits seem to come to this when I adjust them to 3.02mm. This definitely gets my “holes too small, parts too big” and means that my finger jointed boxes did not fit together at all. They do now.
When both inside and outside get me the same dimension, then I would look to steps/mm on the machine… But mine were as close to dead on as I can measure with my caliper. (<0.1mm error over 100mm.)
Interested to see what would happen if you tried this test with a more stable material like MDF. There are simply too many variations in hardness, density and grain patterns in solid wood. Really soft wood like Cedar might compress when your milling it as well. Using a stable, engineered material would probably give you a better read on accuracy.
I know this was just a test but if you wanted to use the CNC for solid wood joinery I’d oversize your tenons and pare them down with a sharp chisel so you get a perfect, tight fit.
Well I made some progress by adjusting the tool diameter as suggested by Dan. Turns out my 3.175mm end mill was actually 3mm in diameter.
I ended up making the tool diameter 2.7mm to compensate for runout and machine flex, and that got my first test cut within acceptable tolerances.
I havent had much time lately to do more testing, but I think I got it.
Thanks for the replies
