Hello all! Real quick question regarding LR3 cutting. My main operation on my low rider is part cutting, (2D contour on fusion 360), for cutting some shape out of a large piece of material. I believe this is known as slot cutting, and can be difficult because it is essentially 100% step over?. I also exclusively cut hardwoods like white oak, walnut and rock maple.
I was wondering if anyone had a tips, tricks, feeds/speeds, etc. for doing this kind of operation consistently. I am able to do so now with decent results, however it can go by slow and be quite loud. Also, what is the best way to remove chips from inside the slot, as they can become wedged in there pretty tight.
I would recommend getting the free trial of G-Wizard feeds and speeds calculator. You can tell it details of your machine, including RPM range, bit size, # of flutes, maximum federate, etc. Then select the type of material, and you can select feeds, speeds, DOC, etc. based on the optimum chip load for the material.
If you like it, a one year subscription is something like,$60, and at the end of the year, you get a free lifetime use license at no charge (limited to 1.5 HP, I think)
For chip evacuation, an air mist nozzle can help. You could also use trochoidal milling, which makes a wider slot. It adds a lot of time per pass, but that’s offset by the ability to cut the material in a single pass.
Make sure you’re using an upcut bit, crank up the rpms, and run the feed as fast as you’re comfortable, shrink the DOC to suit, and add a roughing contour pass, finish at final depth only, and pick an appropriate finish feed rate to clean it all up.
Rigidity is the limiter on things like REALLY hard wood and aluminum. When we take deep cuts, we end up going so slow that we turn chips into dust and burn endmills, making them dull and adding to the problem. If you can get up to 0.002"per tooth, virtually all the other problems go away, but the lower limit depends on the wood. 0.001"per tooth is generally safe.
Cranking the rpms up really helps throw the chips up and out on an upcut mill, and keeping the chip load high makes sure the chip is large enough to have momentum out, even with a smaller DOC. The second roughing pass helps make sure the cut is wide enough to let the chips out.
When I’ve done this on V1 CNCs (4 Burly, 3 primo, 1 LR2) I get at MOST the same cycle time, usually an improvement of some sort, WAY better reliability (fewer scrapped jobs), and the machines don’t sound like they’re struggling at all…which decreases my stress!
On my primo I cut hickory at 0.1" DOC at 100ipm with a 2fl endmill at 26000rpm (0.0019"/tooth) and 85ipm with a single flute (0.003"/tooth), like Ryan sells (short 1/8 kyocera) not the O-flute (also single cutting edge but different geometry). My 2x4 primo ran 0.08"DOC, and 80ipm/60ipm respectively. I’d have gone faster if I could have kept the chips from jamming up the bearings.
Cranking up the RPMs leads to burnt up bits if you cant move fast enough. Moving faster than the build is capable of leads to skipped steps and messed up cuts. Finding a good happy medium between RPM and Feedrate is a good start. Most LR3/Primos will need to be at the lower end of the RPM range to be able to keep the chip load high enough to keep the bit cool. If your turning 24k RPMs and just making dust you aren’t removing any heat from the bit.
When I finally learned that and slowed my RPM down, my cuts got a LOT cleaner and my bits last a lot longer
That’s true, but not being ABLE to move fast enough is usually not the problem. That’s why I cautioned about going slow, running the feed as fast as he was comfortable and managing the DOC from that speed. Packing and recutting chips has ruined WAY more bits for me than not being able to cross the chipload threshold.
The question was specifically about very hard woods, and these are my own tips and tricks. With harder materials, the rigidity we lack manifests in a larger load on the next pass down or over, which means more deflection, which means more load, etc. The strategy I’m suggesting is to reduce that deflection with shorter DOC to improve the consistency from pass to pass, which increases the reliability and, in my experience, cycle time because I usually get more than double the feed rate at half the DOC (not much more, but more). Of the two goals, consistency was asked for, and I would trade 20% of my cycle time for a 50% reduction in scrap every single time. That may not be true for everyone, but it seldom even matters to me because the cycle time is typically very close or better.
I do like the math of it, though. 30k RPMS on a single flute endmill hits the 0.001"cpt threshold for burning at 30ipm, assuming you are evacuating the chips (its a little higher for softer woods, higher still for soft plastics). I routinely cut at 70ipm+ on my LR2, and I didn’t even do a good job building it (which was the main reason I eventually took it apart). My 2x4 primo took on acrylic at 50ipm, 1/8 DOC limited by static clinging it all to the tubes, and ran 1/4 in endmills at 30ipm through soft maple down to 0.15 before having trouble. Those all ran with my 611 that tops out at 26k rpms (measured). A LR3 should outperform anything I’ve built except maybe that 8x11 teeny tiny burly.
If a V1 LR2 or 3, primo, or burly can’t cut at any depth at 30ipm without skipping steps, we should ask what’s wrong with the build and sort that out first.
