My goal is to contour out a shape/insert that fits inside of a pocket using Fusion 360 and my Shapeoko XL running on Carbide Motion. Similar to how a guitar neck would fit into the neck pocket. Photo below:
I enlarged the pocket to be 0.5 mm larger on all sides as compared to the insert to make sure the insert would fit. No success.
Consistently when I try to mill out an object to fit inside of another object, the pocket cut is too small and the contoured shape is too big. “Stock to Leave” is left unchecked on both the pocket cut and the contour. I’ve calibrated and recalibrated the X/Y step movements before, they always seem to be accurate.
Here are my results from my latest machining using a #201 .25 inch flat cutter:
Thank you Will - It looks like you’re using Carbide Create in those tutorials, which I have not had a chance to experiment with yet. Can you explain how Carbide Create fits into the workflow if I’m modeling using Fusion 360? Or are the techniques you show in Carbide Create something I can implement in Fusion 360’s Manufacture workflow?
I use Fusion 360 for this exact thing. I draw them exact and usually cut them exact and they usually fit very tight. If not, then I do a negative stock to leave of say .010" on one or the other. I want them tight so that I can sand/scrape them down to the correct fit.
Depending on the tool path, the divot is tool path staring point. It should be outside on the perimeter cut and inside on the pocket cut. So let’s make sure you are using the correct 2D tool paths. (pocket and perimeter)
Also if you are drawing a specific size in Fusion, and its not cutting that, then the step motors probably are not perfectly adjusted. This can be tested by drawing a 100mm square and cutting it part of the way through (no need to cut all the way). Then measure it to see if it is in fact 100mm in both directions. If not, there is a cheatsheet that helps determine how much to adjust the steps/in in Gcode (I think its $100 and $101 but would need to check). We can help once you do the test.
If you attached the Fd3 file, I will take a look (or PM me and I will give you my email)
My suggestion would be to make a simple, equivalent cut to one of your Fusion 360 project using Carbide Create — if it works, you know the machine is sound and the problem is w/ Fusion 360/your understanding of it/how you are setting up toolpaths/tooling — if it doesn’t, then the problem is w/ the machine and you can contact us at support@carbide3d.com and we’ll get that sorted out.
Thank you Joe - Here is a link to the Fusion project: Fusion
I am currently using the “for personal use” version which does not allow me to make the share link downloadable, let me know if there is a better way to get you the file.
You should be able to export to F3d from the file tab. File tab is the folder looking icon on the top left. Open dropdown a select export. Export file type as f3D to your laptop. Then attach it here or send it to me. I just want to look at the tool paths etc.
As we discussed Matt, the file and tool paths look fine. Next will be to look at the mechanical aspects of the machine. Not just the belt tension, though that is important, but also the V wheels, squareness of machine, accuracy etc. There are several good threads on this board, but we can also discuss more here in this thread.
@AmateurHour Matt, check out ncviewer.com. You can load your files there and check your gcode. Both files look good as far as I can see, nothing in the gcode telling it to do something weird. Cut depths look reasonable.
Dull bits or overly aggressive feeds can create extra drag and missed steps (mentioning because your cuts don’t look very clean, but that might be the wood more than the bit)
As @WillAdams mentions, all of these issues will be exacerbated when you have a deep narrow slot. Play in your system will cause it to grab into the material.
An easy check is to power on the machine which locks all your motors. Now push on each axis. ANY movement at all is bad, it should feel solid. Grab the z axis, rock back and forth, front to back. Any movement there is bad. Check each v-wheel, it should be tight against the frame.
I went through this last fall, after a long period of deferred maintenance. My belts were stretched, some missing teeth. My v-wheels were loose. Router bearings were shot. Handful of other problems. Spent some time repairing those issues and everything is tight and working probably better than new.
Test Number 2
I did further testing today, results below. Still no luck.
This was all one file created in Carbide Create, converted to .nc on the Carbide 3d site, and ran through Carbide Motion. I used the #201 1/4 inch bit. Oddly enough, the pocket was closer to the design but the insert piece was still way off (over 3.5mm off).
Afterwards, I jogged the machine left to right and bottom to top to measure distance as recorded by Carbide Motion versus the actual movement. It was quite accurate (results below).
Looks like it is a machine-specific issue, so I will take Will’s advice and reach out to support. Thanks everyone for looking into this and offering suggestions.
Dan - ncviewer looks like an excellent resource, thanks for the tip! I’ll do some digging into the belts, pulleys, and wheels to see if there is any looseness there and run the push check you suggested.
@dandangerous - You were right, belts were way too loose. Like embarrassingly loose. I tightened them up, recalibrated my $100 and $101 and had improved results:
Glad you figured it out! If your belts were that stretched, time to replace. They are a wear item. I picked up this one from AliExpress.
The SO3 is GT2-9mm, not sure on other machines. I picked up 10 meters which is enough for two full belt changes. I went with the aramid (which is kevlar) because the stretch/strength is very similar or even better to steel but it is supposed to handle the tight radius bends over the drive pulley better. So far been happy with it.
Check those drive pulleys too, multiple similar issues in the forums related to those slipping, and it can be hard to diagnose.
Last, on squaring the Y axis movement. Before you you turn on the power, push the Y axis gantry all the way to the back of the machine until it hits the stops. Hold it there when you turn on the machine, this will lock it to the very back with both Y axis motors locked in the same position. When you home the machine it may fail the first time, home it again. Now both Y axis motors will be the exact same distance from the back of the CNC frame (assuming that is square…).
I wouldn’t bother with any serious squaring and adjustments until you replace those belts (and maybe some v-wheels).
One other thought - you can de-complicate your test pattern. All you need is a square to test all three axes movements. For my XXL I use a 12” square so I can use my 18” line gauge for these 6 measurements:
I set zero as the center of the square and cut this in the center of my machine. Those six measurements tell you everything you need to know. I also check depth in all 4 corners. You can make this pattern larger, but really no need.
Your bit and router bearings can make a difference too if you’re getting bad runout out or your bit size is fractionally different than spec. If it cuts a perfect rectangle (diagonals measure the same) and your bit and runout are good, then adjust your steps in grbl. If it’s not a perfect rectangle, you have other mechanical work to address first.
)
