I am attempting to cut a precise hexagonal slot, approximately 6.5 mm wide on all sides, 1/4 inch deep in plywood. The issue I am experiencing is I am getting 3 pairs of varying widths for the six sides. Two are perfect, two are slightly off, and two are off by a decent amount.
The CAD/CAM is being done in Fusion360 and it is being carved on my Xcarve 1000mm with an Inventables 1/8" Downcut bit. I have checked all the measurements in the CAD to make sure it all of the slots are equal. I have a basic 2D pocket set as the operation. For what its worth, the CAM is set to tool on center, and there is no rest machining enabled.
I’ve been reading this post here for information
[SOLVED] 2D pocket cut about 1mm off even after multiple passes
I am going to try the following:
- Adjusting some tolerances and settings in Fusion
- Remeasure end mill
but given the perfectly symmetrical nature of the issue, does anyone have any specific ideas of what I’m dealing with?
Thanks everyone in advance
I strongly think this is a flex/backlash issue, which is different on X and Y axis.
In combination with path direction vs router rotation and wood fibers.
A nominal Xcarve will have a tolerance < 0.13mm but variations must be expected.
What kind of tolerance do you get if you machine the same part 10x larger?
Are the offsets the same? If so => backlash/flex
I was thinking it’s a particular axis also, but what had me wondering is that the two perfect sides are essentially just a mirror of the two sides that are slightly off.
For what its worth, the toolpaths start in the upper right hand corner and run the perimeter clockwise and counter clockwise.
When you say they are off by 5mm do you mean too wide or too narrow? Also is the 5mm error measuring face to face across the hex? And finally is the 5mm on the left and right a cumulative 5mm or is it per face?
Since the diagonals have better tolerance than the two vertical sides, it may be that combined force of both X and Y steppers is able to better push through your material. Diagonal tool paths are popular in many CAM programs because you get more force from both steppers stepping at once.
I also agree with Niel, in that it is likely a belt tension issue since the tolerances fall back in line as you complete the perimeter.
Last of all, you may also need to adjust steps per inch on the X and Y axes.
Sorry, I should have specified. They are too narrow. The measurements are the width of each individual side, they aren’t cumulative.
How does one adjust steps per inch on X and Y?
I have some work to do for sure on the hardware side of things. Do you think there’s any possibility the issue lies within the software?
If its not clear in the image, I am referring to the distance across the dark gray channels on each particular side
Just an update- I test jogged the X and Y axis like crazy, everything came back with perfect accuracy.
Also, I checked the diameter of the bit, it came back roughly .124 at the top of the bit (above the flutes). I’m finding it difficult to get a good reading on the flutes.
I tightened all the belts and wheels, gave them a good cleaning too. I did find one noticeably loose wheel on the Y2. Will run another carve tomorrow and see if that’s improved things.
Starting to feel like maybe it is a tolerance issue in Fusion. Soon to find out.
To get an actual read on the bit you need to carve a slot and measure the width of the slot. If for instance the Dewalt have a run-out this will only show in the slot.
Note that the Xcarve, tight and tuned, nominal precision is regarded to be around 0.07-0.15mm (0.003-0.006")
Hello Just wanted to post an update on this issue I was having. After squaring up all the axes, tensioning the belts, and getting everything squeaky clean, I was able to get even gaps on horizontal, vertical, and diagonal drops.
That being said- the width of the slots are all 0.5mm short. So now I’m looking at backlash and/or the diameter of the bit. Two questions if anyone can help
How does one compensate for backlash?
And what is the best way to carve a test slot for measuring bit width using the X-Carve?
Can you share the Fusion file?
You might just need to run a finish pass. Could be deflection.
Quarter Inch Slot Test v2.f3d (155.3 KB)
Here is the test file I used. Just 3 quarter inch slots- horizontal, vertical, and diagonal. All slots measure 0.23.
Wheels tightened correctly
Just following up- I increased the slot width to 0.27 and got 0.25 slots. So as in the previous test, off by .02.
Should I just compensate for this when setting up CAM operations? Use a finishing pass?
I would try the following…
- use Easel to create a rectangle 2 inches on the X and 1 inch on the Y
- tell Easel to cut ON the line of that rectangle and not outside or inside.
- use calipers and measure the dimensions of the rectangle that was cut out.
Regardless of your bit diameter, the X measurement minus the Y measurement should be one inch. If it isn’t there may be play in your setup or you may need to adjust the number steps per inch.
Two inches minus the X measurement will be your bit’s cutting diameter. This may be larger than you measure on the bit with calipers. This is because there is runout in the router and bit, there is flexing of the bit, there is stretching of your belts etc. All in all, it should be close to the expected diameter.
Measure the diagonal both ways and this will tell your machine is square with regard to X and Y. If it isn’t, you may need to adjust your machine for square.
Thanks for the response @HarryC.Ragland
To finish this topic up- I think what this amounts to is the following: I have a specific cut which needs fairly accurate precision. The machine is as tuned as I can possibly get it. If a predictable 0.02" is a result of runout, flexing, stretching, deflecting, etc.- I think it’s probably best to just compensate in the CAM for this particular cut and call it for now.
Though I am curious @NeilFerreri1 - regarding Fusion- do you think leaving stock and then doing another finishing pass would have similar results?
If you’re consistently having an issue with undersized pockets, the most likely cause is either an undersized endmill or deflection. Leaving a very small radial stock to leave, and running a full depth finish pass is the way to go.
Would you recommend conventional vs climb?
What material? In wood? Climb for rough and finish. Sometimes I’ll use a conventional finishing pass in aluminum, but I’m not convinced I gain anything. I’ll also sometimes mill both ways on adaptive toolpaths in aluminum.
I am new here and the whole carving experience. With that said, have you tried rotating the work piece and see if the discrepancies stay in the same segments? This may help eliminate tolerances issues in the writing program or even the machine. I come from experience with other types of mechanical troubleshooting. I look forward to finding out more on what to look for on these issues and how to resolve them. The messages I have read have been by some very savvy folks!
For what its worth, I tried segments going in all 8 directions all with similar results. The bit I had been using for testing was rather long and I think the flex of it probably accounted for the .02.