Parts that are to mate do not match after cutting parts

I am trying to cut two parts that are to be mated via a scarf joint.
The material is 3mm poplar ply (liteplay in the hobby industry) and I am cutting the parts with a 1mm serrated bit.
The parts are drawn in AutoCAD exported as a DXF and Imported into Estlecam.
The parts match together in AutoCAD and in the Estlecam program (the joining faces (scarf line) line is common to both parts).
In estlecam the parts are then traced as a “part” with the cut being on the outside of the DXF line.
After the parts are saved as the CNC file and run through the MPCNC the scarf faces do not match.

I have tried tightening the belts, loosening the belts, the gantry has no play in it.
It is imperative that these parts match accurately.

Kinda lost her as to a solution on why the joining faces do not match

Thanks for the help

You’re cutting these out of two different pieces right? I assume you run the red line on one piece and then the yellow line on a new piece of wood?

It looks like you are off by a bit diameter. If you put your bit between the two pieces to act as a spacer does everything line up properly? ( Besides the fact that the gap is too big)

Yes, two different pieces
Both with a common mating line
Both parts are generated via estlecam as separate pieces, with separate cutting paths
The picture of the estlecam program (red and yellow lines) is just to show that the parts “indicate” correctly in estlecam with the correct 1mm tool path.
The actual parts in the picture if I was to press them together will have a large gap on the diagonal line.
See the new picture I have

Are you cutting on the right side of the line? The upper piece should be cutting on the lower side of the line, and the bottom piece should be cutting on the top of the line.

1 Like

yup
both parts are being cut as a “part” and not a “hole”
so that has the cnc path being generated around the exterior of the parts outline

The job looks correctly set uo, but are you using a 1mm tool? If you are using one that is thicker, say 3.18mm (1/8") then the tool path will be too wide, and your part will be too small, resulting in a gap between the two parts that fit.

it appears that the cnc path is not correct when cutting on the diagonal path

In all of these kinds of problems that I have seen on the forum, none have been traced back to bad g-code generated by the CAM. All have been traced to CAM settings, or bit diameter mismatches, or some sort of mechanical issue with the machine like runout or deflection. That doesn’t mean it cannot happen, but it is not where I would start if I was troubleshooting.

My suggestion is to model a square connection between two parts (single finger joint), then take a look at the g-code. With a known bit diameter and this simple geometry, you can easily evaluate the g-code to make sure it is correct, and you can do a test cut on scrap to see the match. This will tell you a lot about your issue.

1 Like

1mm is a pretty thin bit. I would guess that the bit is bending/wobbling as it moves through the workpiece causing the cut to be inaccurate. In the picture, it looks like there is a slight bevel on the edges of the pointy part. Just a guess though.

Use a finishing pass for accuracy.

Runout or vibration or other magic can make the tool behave like an oversize bit.

Cut some rectangular holes and parts and check whether the net effective dimensions match the intended size. Use a finishing pass so it is a realistic model of your final job.

If the parts are undersize and the holes are oversize by the same amount, your bit is acting like a larger bit.
Adjust the bit diameter in CAM to reflect what your bit is actually doing.

1 Like

Ok a little more information to go on.
Material is 2.7mm +/- .003mm thick
3 passes are made (1mm/1mm/.71mm) with a travels speed of 12mm/sec due to the small 1mm bit
The cut line is 1mm in width when the last pass is completed (I have mic’d it on occasion)
The bits mic out to 1mm exactly
I have been using this method for a few years now with successful routering (lack of better words) of parts (giant scale aircraft parts).
Here are a few more pictures of what I have just cut and these cuts are perfect and are all tabbed together and are holing together without any glue.
The tab slots are cut to 2.6mm (.1mm less than the thickness of the ply material) so they fit snugly together.
Any item that is tabbed with a 90 degree tab to fit into a slot for the tab works perfectly.

The only time I have had trouble is when I have 2 pieces that have to mate with a curve or an angle cut.






4 Likes

I’ll run some test shapes and see what the results are

Thank you for the help
It is greatly appreciated

On a side note…

Those bits are the up/down “grinder style” cutter. They have poor chip clearing performance, and are best for abrasive stuff and composites, like milling PCBs etc. A spiral upcut is going to give the best performance for general purpose wood work like this.

Also, 1mm does not seem like a requirement for that particular part. Maybe try a larger tool? I usually use the largest tool that will get the job done. Eyeballing that tapered fit… looks like a 1/4" upcut might work? As others have mentioned, CAM errors and machine flex are more common, and your feeds look conservative to me… but a thicker bit would eliminate flex from the troubleshooting list.

BTW… been an RC builder/pilot for over 30years now… love what you’re doing with the cnc! Custom planes was my primary purpose for building my cnc… just need time from life/work to start enjoying it all. Honestly, looking at your glue ups… if I was milling those I’d mostly use a 1/4" upcut, and finish up the tight inside corners with a small bit if there was a bunch… or just hand razor them if just a few.

1 Like

That’s impressive work and it sounds like you’re doing everything right.

The only other thing I can think is if a small amount of deflection is occurring in the corners. Climb milling and conventional milling can leave slight (but different) defects on corners because of how the cutting action pushes the bit. I would be curious if conventional milling produces the same parts or if the errors are reversed.

If conventional milling reverses the error then it is from deflection of the bit, which is exacerbated in corners or tight curves. A very slow, thin, full depth finishing pass might still be in order, to have the least possible load on the tool. Then it should be almost as good as a laser. Then crank up the speed to see how much you can get away with, so you don’t have to wait forever.

Reason for the 1mm bit is that there are hundreds of corners for the 90 degree locking tabs and slots. If I was to use a larger bit each one of the cornrrs would have to be cleaned out.
oh BTW there is no glue on those wings yet, they are all just indexed and tabbed together for now.
they will be disassembled and reassembled with glue

1 Like

In estlcam you can overcut the corners to compensate for bit diameter and eliminate the cleanup. If your group all your slots together you just click on the corners to over cut them. It works fantastic.

Also, out of curiosity, plunge that bit straight down into some material and then shut the machine off and see if the bit is a tight fit into the hole. This would determine runout if it’s a loose fit. On my Makita router with stock collet I’m seeing about 0.003" of runout. Cheap reducing collet adapters brought that to about 0.006" Might be an issue but it might be nothing, just another thing to check. I think angles would magnify any error like that

Also your projects look awesome! Nice work

1 Like

I have had the same problem on occasion my problem was tracking. At much over 500 mm/min the cutter flexed enough to be a problem on circular cuts but not on straight the finish cut may help also. I was using a regular 1mm single.flut end mill

Have you measured the actual parts that you cut?
Is only one part too small, or are they both too small? If the gap is 1mm, that would be only 0.5mm off each part.
If only one part is smaller by 1mm, then you are cutting the wrong side of the line.
Double check tool paths and offsets, verify measurements of the cut parts

2 Likes