I smoked my router bit about 25% of the way in, but left the machine running as I had never been able to complete a large job until patching my motor encoders.
Clearly I don’t know the first thing about setting up jobs despite a hint in an earlier post from @anna.
Is there a table of known good settings for router speed and axis speed for some more common materials (OSB, Pine, Sande) plywoods of common thickness (0.25", 0.5", 0.75") or their closest metric cousins?
slow down the speed the router is spinning, increase your meed rate (speed
moving through the material)
If you are getting dust, you are spinning too fast or moving too slow, you want
chips not dust
The other thing you can do is to get a router bit with fewer flutes. With the
maslow you do NOT want a 4 flute bit, a single flute bit is probably best.
I didn’t ask this as too big a step down can cause other problems, but not
likely to burn the bit (it would cause other problems, rounded corners, tilting
sleds, etc)
hmmm yes, Im wondering if you get dust instead of chips if the step down is too small which then causes the bit to heat up?
possible, and it’s also possible that you are doing multiple passes to widen
things with too small an offset.
but these would need to be reall small. With a 1/4" bit (the default and
assumed), 0.1mm would probably not be enough to cause this, but 0.01mm would be
(don’t know where the problem would be)
you want to take as big a cut with each flute on the bit (both depth and
stepover) as you can get away with without getting errors from the belts
stretching or the frame/maslow/bit flexing.
OK this is all helpful and I have been seeing problem signs that the router speed is too fast / travel speed is too slow.
I am getting dust not chips
I have 3 flute bits. I’ll order some others.
Should we try to come up with a table of best known settings? I have seen something like this for 3D printers, I’m sure it would be helpful and I assume that 90%+ people will be using the dewalt and cutting pine ply so It shouldn’t be too crazy.
@anna, @bar, perhaps you have some internal table of cut settings and router bits that you have tested that could be a basis for such a table?
I have a heap of small single flute bits and just burn them out/snap them off - and then replace.
But what I really recommend is getting a lot of cheap bits and just experiment with different feeds and speeds. Admittedly that only tells you how cheap bits will perform, but it’s a really good way of learning, getting a sense for how things sound and behave when bits are dull, feed is too slow, speed is too high, etc.
Dust = friction and therefore heat
Chips actually carry some of the heat away with them, so much more desirable
I just ordered these 1/4" upcut end mills from amazon. They are a pack of 5 for $50.
They seem to be 2 flute. I couldn’t find a cheaper pack to try during a quick search.
When they arrive I will try to do 5mm plunge depth and run the sled at 60 in/min with the router set to speed 1.5.
Hopefully the bit will not roast.
If anyone has a good suggestion for bits I’d be happy to try, cheers for the help so far everyone!
I have used that exact bit. I build my gcode with Fusion and use a library that SpeTool provides for Fusion of all their bits. This lets Fusion know the best feed rate based on your spindle speed. Since the Dewalt can not go slower than 18k RPM, it wanted to drive the Maslow at 6350mm a minute. For the cuts I made I ran the Maslow at 2000mm a min and set the Dewalt to its slowest speed. Depending on how deep you are cutting you could probably push the rate all the way up to the Maslow’s max.
gosh dang, that’s flying! and it does alright? I’ve been cutting at 1000 mm/min with the spetool compression bit, instead of the upcut, dewalt on 6. The cut depth I’ve been doing is 5mm multi pass on 20.5mm (3/4) thick wood. It’s been working, but i’ve been contemplating if I should try faster.
I have the upcut in stock, just waiting for the compression to fail.
I’ve done cuts at around 120 in/min (~3000 mm/min) that have been fine. I’ve been running most cuts around 75-100 in/min (~1900-2500 mm/min). I’ve been steadily pushing my rates up and trying to get comfortable pushing the limits higher. It’s easy to feel nervous about going too fast, but often it’s the opposite and running too slow causes bigger issues than faster. Plus going faster reduces the overall cut time.
To be clear, I have only made a couple handful of cuts so far on my M4. I’ve been trying out different bits. I’m really happy with the look of downcut bits on various material when wanting a really clean cut. To clear out material, I’ve been mostly using an upcut bit since I’m not as worried about the final appearance of those cuts. I haven’t been playing with depth that much (not trying to play with too many variables at a time). I’ve mostly been doing about 2/3 to 3/4 of the bit diameter per pass (e.g., for a 1/4" bit, depth of ~0.16"-0.1875").
Now that the other parts of my M4 seem solid, I’m trying to dial in feeds and speeds.
I am seeing varying guidance in a variety of venues as to what an appropriate step-down is. The SpeTools Spiral Router Bit chart row for 1/4 inch bits calls for a stepdown equal to bit diameter at 18,000 rpm with feeds north of 180 in/min (where does the M4 top out? Well south of 180 in/min, I assume). Elsewhere I see a thumb-rule with stepdown equal to 1/2 of bit diameter.
I am not sure where to even start my testing. I would like to begin somewhere likely to be reliable and fairly clean. I’m cutting plywood in varying thicknesses, mostly with a 1/4 inch compression bit, but will use a 1/8 inch compression bit for 1/8 inch luan.
