I’m using a 1/4" upcut flat-end mill. When cutting, it tends to grab the wood and “rip” it up. It vibrates violently and leaves edge marks where it pulled material out. Some of the chip sizes seem awfully chunky too.
What could cause this? Do I just need to slow everything down? My step height is only 1mm.
VIDEO: CNC Ripping
Cutting speed is too fast.
Too much cutting depth per blade.
Machining depth is too large.
Processing material is too hard.
Uppercut, downcut
Rotation speed
Repeat trial machining from the minimum setting to find the optimum conditions for the material.
Thanks to @Blockmodule
@bruno71 I have checked your video.
Edwin
What speed are you running at?
What type of wood?
-S
The machine is not an ideal rigid body but a real physical object with finite rigidity. When you push on an ideal rigid body it does not change shape. When you push on a real object it does; however large or small it might be, there will always be some deformation. Welcome to the real world.
You’ve got two kinds of problems, one with the machine itself, one with the material.
For the machine, it’s just not very rigid, and not just in a single way. The base plate is fairly thin. The uprights don’t have a lot of resistance to bending in either X-Z or Y-Z planes; the little brackets just aren’t very big. The bearing orientation in the linear modules are only well suited for resisting torques in the plane of the top face; for the X-axis, this is the X-Z plane. Torque from the cutting bit is in the X-Y plane. When this machine is overloaded, it’s going to move, and it’s easy to overload.
For the material, you’re pushing the capacity to cut this material with the motor in this machine. A useful thing to understand about DC motors is that they have maximum torque when stalled. If you’re putting too much load on the bit (too much or too fast), the motor will slow down, which increases its torque, which allows it to cut again, which then allows another overload, and so on. There’s a time lag here because of the elasticity of the work material, and that induces an oscillation. This is the primary source of the vibration you’re getting.
Wood prefers being cut with high feed rates, so to reduce the load on the tool you want a shallower depth of cut.
The spindle speed is 12,000 RPM.
The Cutting/Ramp/Plunge Feedrate is 350mm/min.
The Max Roughing Stepdown is 1mm.
The wood is spalted maple.
What are your suggested settings?
In addition to above recommendations, I would add: do not do cuts that engage both sides of the cutter (where slot diameter = cutter diameter). Engaging both sides (even inadvertently) will cause violently changing forces to be applied to the machine, resulting in what you see.
High efficiency trochoidal paths would be neat, although out of reach for most hobbyists using free software.
In lieu of that, shallow axial DoC using a smaller cutter than the final slot width for roughing, with a finishing pass that touches up both sides with a full depth shallow radial DoC.
Spalted maple can have unpredictable hardness - I’d plan on very shallow cuts. 1mm stepdown may be fine, but you have to get rid of the chattering where the bit is bouncing back and forth in the slot engaging alternating sides.
Just my 2 cents, from someone unqualified to be discussing machining.
Speed isn’t the problem. 350 should be fine. I tend to run at 400 cutting, with ramp at 340 and plunge at 250-300 with hardwoods, but at a .5mm step-down with a 1/4" bit. Never done spalted maple, but I’ve done plenty of maple and oak (and padauk which is probably twice as hard). I would’ve assumed the spalted would’ve been easier, but maybe it’s more of the burl/knotty area where it’s harder. I’ve had a couple of pieces of oak that have given me fits though.
A few things.
I’ve done a bunch of deep cuts like that and as @brent113 mentions one of the big problems is that it’s cutting on both sides. Anything much over 15mm cut depth starts having problems. So anything you can do to clear some material will help.
You also need to make sure you clear out chips with a vacuum. Especially with a down cut bit they’ll quickly become compressed and the bit will be unable to move them out of the way and bog down.
Lastly, you should make sure your pass direction is set to “conventional” not ‘climbing’. This will make sure that the bit isn’t pushing away from and off of the workpiece, and pulling it in to cut. It will ‘fight’ against the workpiece less.
I would double check if you have any play in your x-axis bracket. If you try to tilt it up and down or side to side is it still solid? I’m betting that either it did before and that’s part of the problem, or it does now after seeing what it was doing in your video. I would’ve stopped the machine immediately if I saw it doing that.
Listen to your machine. You’ll quickly learn to hear what it’s doing and know whether you can increase or need to decrease your cutting depths and speeds.
-S
Also, do a search on thingiverse and print out some more clamps.
Just holding that on top is prone to slipping. You need some ones on the side that lock it in place horizontally.
I like these:
I’ve printed them in a few different sizes. The original is a little big.
-S
@brent113 The “slot” it is cutting in the video is actually the final contour to remove the piece from the stock. It’s not a slot with dimensions - it’s just the outer edge of the piece. How do I make that “slot” wider so the bit doesn’t rub both sides of the wood?
@sdj544 I used most of the default settings in Fusion360, but I’ll check for the pass direction to be set to ‘conventional’.
It can be adjusted to various heights and lengths with stainless steel fittings and bolt nuts purchased from a home improvement store in Japan.
I couldn’t find the settings in Fusion360 for setting the pass direction to “conventional” or “climbing”. Where are those settings?
How do I widen the outer contour in order to remove the part from the stock without rubbing both sides?
Under 2D Contour it’s actually called “sideways compensation” (hadn’t noticed the difference in terminology before)
For most tool paths it shows up under passes.
A couple ways to widen it.
If you’re using 2D contour you can do a pass with “stock to leave” set at 2mm and do a total depth of 10mm or so and then repeat that pass with it set at 0mm. Do these until you have the depth you need.
You can use adaptive clearing and then it will just clear out everything. You can also create what I call ‘ghost’ shapes (not sure if there’s an actual term). Create a shape or shapes and then turn off visibility and you can use those to select areas to either mill or avoid. Just make sure that they don’t affect the size of your stock.
-S
My $0.02… Try vacuuming or blowing the chips as they are cut. If a chip gets caught in the cutting edge it will vibrate the cutter.
After tweaking some settings, the issue was a little better but still present. I do have a sneaking suspicion also that it may be related to chips getting caught. Or just wood density variations.
