The milling basics page seems geared toward the mpcnc with the little dewalt 660 in mind. How would the advise change with the lowrider and the bigger dewalt 611 in mind? Being just plane bigger can it take bigger bites? I see the link to purchase the 1/8" collet, but what do I need to know before I start running 1/4" bits?
I’m hoping it can at least handle a larger depth of cut than 1mm so I can quickly knock out a bunch large plywood parts for an upcoming project.
I too, think the milling basics page is geared more for the mpcnc, however both machines are using the same stepper motors, pulleys etc. As a result I think it is mostly relevant anyway. Taking that into account, I have basically been following the the only variable you should be changing is the depth of cut advice from that page. @vicious1 is also fond of noting that every build is different…
My Lowrider is built on a 32"x80" inch door, so it’s probably more rigid than a full sheet machine, but…
I have been cutting ~5mm depth of cut on my Lowrider regularly for the type of cut your planning. I’ve been using a 1/4" up-cut spiral bit at 8-9 mm/s feed and 3 mm/s plunge. Cut quality has been excellent.
Including a little extra depth to ensure I cut all the way through, I’ve been cutting parts out of 1/2" ply in 3 x ~4.7mm deep passes, and 3/4" ply in 4 x ~5mm deep passes.
Hope that helps.
I think cutting deeper rather than faster is preferable for 2 reasons. One is that you use more of the cutting edge on your bits. So rather than wearing out 1-2 mm at the tip you spread the wear over ~5 mm or so. Also, the stepper motors have less torque at higher speeds, so trying to cut faster may result in missed steps even thought the load on them is lower due to a lower DOC.
[quote]
My Lowrider is built on a 32"x80" inch door, so it’s probably more rigid than a full sheet machine, but…[/quote]
Yeah, mine is about 50"x50" so if anything a little less riggid than most.
Very helpful and encouraging! Thank you.
+1
No different.
The spindle spins at the same speed, same electronics. The MPCNC at its recommended size range is the same rigidity as the LR in it’s size range. Same specs same cuts. Tons of people seem to think the LR is the better version, it is the same build for a different size range.
A LR at the size of a MPCNC well it could probably cut faster, but only if you want thin material…so if you built a short MPCNC well it would be too close to call.
To sum it up Larger more powerful spindle, steppers, power supply change nothing our limit has always been machine rigidity. Honestly any machine that is not cast iron or massive (granite/steel) can not be vastly better in terms of rigidity. I think if you looked around at other machines of similar size you will see we all run about the same speeds.
Not considering the geometry of the work and all other things being equal why choose a 1/8" 2 flute spiral upcut bit vs a 1/4" 2 flute spiral upcut bit or vise versa? I assume the 1/4" would put a bigger load on the machine, if so is it even enough to matter at 8mm/s?
Much larger load, load is proportional to material removal. Every machine is only strong enough to remove X amount oaf material it doesn’t matter what bit size you use. So if you are pocketing, use a larger diameter, if you are slotting do you want to slot 4-8x slower because you are removing all that extra material?
Flutes are a big factor as well, you need to get the material out before it comes back around to cut again, this sis determined by RPM.
This can be a very very complex subject if you keep diving deeper…flute angle, tip geometry, under cut angle for the flutes, complex or simple. You might want a larger diameter for a longer endmill so it does not flex though.
There are tons and tons of resources about all of this but it comes down to our RPM range works best with a single flute, from there anything will work but it will not make you machine more rigid so material removal rates will be very similar in the end.
There is a machine at our local makerspace that goes much faster than my Lowrider. More than twice as fast I’m sure. I found it a bit alarming to be honest. I can make mistakes plenty fast enough at 8 mm/s 8^)
This is why I’ve been using a 1/4" bit. The 1/8" is probably fine for the 1/2" ply, but just seems sketchy in 3/4". EDIT to add that the 1/4" clears chips out of a deeper kerf MUCH better than the 1/8"
I think the 5mm DOC is probably my personal comfort limit. The router starts to sound like it’s laboring that little bit too much at about 6mm. Also, the materials I’m working with are never perfect. The plywood may be bowed off the table a bit in places…perhaps a touch thicker in some spots, etc. This can already lead to cuts being a couple mm deeper than intended in some areas.
A couple of mishaps have me thinking that my Lowrider may start skipping steps at about 9mm or so DOC with this bit/feed rate/etc. and I like a little margin.
The machine rigidity factor is interesting and plays into this as well. Let’s say your wider machine flexes down 1mm at mid-span do to the weight of the router dust hose, etc. add that to the variables mentioned above and you might be pushing that limit. You may be loosing some precision as well, because now your ARE loading up the lateral axes as well and your gantry might start flexing that way too.
My bad, Similar price range and heft. Same number of zero’s which is usually tied to similar overall mass.
I hesitate to bring this one up given a recent podcast but speaking purely about sub $1k machines, the printnc videos show it chewing through material at pretty impressive speeds.
…assuming those videos aren’t sped up, idk
Yes yes yes! Material removal rate!
Larger mills do generally have more space for clearing chips and are generally stiffer, both plusses. But at the same rpm they also have much higher SFM, so if you aren’t careful you can create a lot of heat.
The printnc is also about 3X the cost of the lowrider, using way larger box tube, and nmea 23 steppers. Of course it’s going to go faster. A printnc isn’t going to be sub $1000 once it’s finished.
So what router speed setting do you run at? My understanding is that the slower the feedrate, the slower to rpm…
IDK, they advertise $700 $1000, the vids I’m referring to are using nema 17s. In the infamous podcast mentioned before the designer said he designed nema 23 mounts but has never used them.
Kind of derailing here. I’m still happy with my v1engineeing machines. I was just wondering if the bigger dewalt 611 could take a bigger bite out of the material than the 660. Sounds like the router isn’t the limiting factor here. Routing is secondary for this lowrider anyway, it’s primarily for a plasma torch which doesn’t care about cutting loads.
30k as far as I know
I’ve been running my dw611 at full tilt (~27,000 rpm, 6 on the dial) when using the 1/8" bits and dialing it back to “5” on the dial with the 1/4" bit (~24,000 rpm per the manual).
I’m pretty sure this is spinning too fast and moving too slow according to the feeds and speeds charts and calculators, but I’m not seeing any burning on the wood (which is better than I generally manage when routing by hand), and I don’t think I’ve overheated a bit (no discoloration at least), so I’m sticking with it.
I’ve ordered some V-bits to try some sign carving etc. and I expect I’ll run those a little slower rpm due to the larger diameter. 3-4 on the dial maybe? I’m open to recommendations. 8^)
Wow… when I ran around a 2 and was pushing the feedrates (12 mm/s, 30 ipm) my saw dust from the 1/8 single flute looked like chips, but when I dropped feedrate to 8 mm/s, 20 ipm, I started to see a fair amount of powder so I turned the dial down further. It still seems too high rpm for the feed rate.
Keep in mind, “milling basics” is meant for basics. It is meant to move people from crowns to sawdust without making them throw the machine out the window. Every machine is different, but I bet every machine can go deeper or faster than the basics, with some experience. The thinking is, make the docs to bootstrap the process, make the forums for more communal growth, and individuals will find their own feeds and speeds that works for them, as they advance.
Presumably, the marketing videos are going to be showing fast, deep cuts, just absolutely crushing it. But the first cut, not so much. I have seen some MPCNC videos that are far better than I could ever do, but the anecdotal video is not the same as the common experience.
I am also a big believer in 1/8" bits. Just from the perspective of cutting out parts, why spend twice the time removing twice the material? I also think that there is a good reason why table saw blades are 1/8" (ish) wide. It seems like a good balance to me.
So… I based my rpm settings on the recommendations in the DeWalt manual. It says the 4-6 settings are for small diameter bits used in softwoods, etc. I figured the 1/8" was smaller than they expected people to use, so went with 6 for it and a little less for the 1/4" All my milling has been in softwood and it seemed to work fine.
However, immediately after posting about the rpm’s I was running, I went out and started a job in some “cabinet grade” Birch veneer plywood. I don’t know whats in the core plies on this, but it WAS getting cooked. I could smell it almost immediately. I ended up backing the rpm down to 2 to eliminate it. Feed remained at 8mm/s and DOC was 4.7mm. Seemed to work fine.
Regarding making powder instead of chips…If I’m not cooking anything, why should I care if I’m making powder? Is it a problem?
I’m no expert, but my understanding is that making powder will result in heating of the bit and reducing it’s life. Powder doesn’t carry heat away like chips do… Something like that. I think if you make powder, the cutting edge is returning and cutting the chip that is made on the first pass before the chip can be evacuated… something like that.