I feel pretty confident about most of those settings because they have worked well since I’ve been using it. The one I’m most interested in is my depth of cut. I’m wondering if I can be a bit more aggressive with it. However, if you think I need to back off some, I’d like to know that as well.
Personnally I’m surprised by the chipload
30in at 30.000RPM using a 4flute 0.25" endmill grants a chipload of 0.00025", which is a quarter of the minimum I would ever use in wood with that endmill size (or any other material for that matter)
Either this is evidence for @gmack’s argument that maxing out RPM makes the chipload value moot, or you must be very near rubbing ? Or are HSS endmills sharper than carbide ones ?
I have read that HSS endmills were once sharper than carbide, but my experience suggests that quality carbide endmills are plenty sharp enough for chiploads significantly smaller than 0.001". They can also provide less tare-out, smoother cuts, and easier chip/dust extraction. The OP should “try it, he might like it”, hopefully he’ll let us know how it works out. I’m glad we’re not talking about needing bigger chips to “carry away heat” anymore! Power woodworking tools “make sawdust, not shavings/chips”.
From memory I think I run nearly triple that with a 0.25” single flute straight bit at about 22000 rpm on maple plywood. Again from memory since I’ve not been doing much SO3 lately:
DOC: 0.125
Feed: 100ipm
Plunge: 50ipm
Router speed: 22,000
Single straight flute 1/4” router bit
Ramp in the cuts over I think 2”
It is ugly loud, which usually means ugly cut, but it comes out great. You can tweak those settings on the fly to lesson the noise until it’s bearable. I’ve cut a crap ton of 3/4” plywood this way.
Yeah I’ve got to agree with the above too, you’re definitely moving too slow for the rpm you’re using.
I cut ply using a 2 flute 1/4" downcut or straight flute at anywhere between
2500mm/min (close enough to 100ipm) at 24,000rpm or
2000mm/min (about 80ipm) at 16,000rpm.
Depends a bit on the type of ply. It is horrendously loud though, even with a spindle it just cuts loudly.
Mostly stock XXL, belt driven Z. Really the only thing not stock on my machine is a SuperPID on my Dewalt router, removed leveling feet and sitting on 1/2” of rubber matting. Been running like a champ for around 3 years now. I have a screw driven Z (not HDZ) sitting in a box, never installed because everything is working good.
[quote=“DanoInTx, post:9, topic:16301”]
Mostly stock XXL, belt driven Z. Really the only thing not stock on my machine is a SuperPID on my Dewalt router, removed leveling feet and sitting on 1/2” of rubber matting. Been running like a champ for around 3 years now. I have a screw driven Z (not HDZ) sitting in a box, never installed because everything is working good.
Thanks! Do you ever use the SuperPID’s added low RPM capability?
Yes, I use it for peck drilling. Regular drill bits don’t really like spinning fast, so I slow it way down. I haven’t done a ton of it, usually alignment pin holes with a 1/4” stubby drill bit, works great. I originally bought it for plastics, but by the time I got it I’d already figured out normal range speeds/feeds for the projects I was doing at the time. Now that I’ve gone laser crazy I cut my acrylic with the laser.
Just to be sure I’m reading this correctly, are you all saying I should increase my feed rate, DOC, or both? I really don’t feel like I’m putting a ton of stress on my CNC, and it’s not all that loud (I still use hearing protection), but at the same time I don’t want to shorten the life of my machine by cutting too aggressively.
@DanoInTx Can you post some pics of your laser addon? and appreciate it if you can include details about all what you ordered to add Laser to your S3, thanks.
@DanoInTx has apparently repeatedly subjected his stock XXL to over 5 times the force/stress as you (7.6 lbf vs. 1.33 lbf), without ill effects. Naturally, since he uses over 4 times as much power to cut 4 times as fast, his approach is going to be a lot noisier, but it does use more of the machine’s capabilities. Note however that, Carbide 3D’s @wmoy seems to recommend maximum forces less than 1.5 lbf, so it’s up to you.
Mine started as a “50 watt” Chinese laser, but the Chinese apparently round their numbers up to the nearest 10 (likely closer to 35-40 watts). I added a 1000mm tube and 60 watt power supply and I should be pulling (peak) 53 watts now as my tube was actually tested. I run it at 16ma max, which is just below peak 18ma. It will cut 1/8” plywood at 24mm/sec and 1/8” acrylic at about 1/2 that speed for nice clean cuts. It’s no powerhouse, but it does what I need.
I have a 7 watt JTech on my XXL, but it’s kinda lonely since I bought my CO2 laser a few months back (my XXL is actually covered in junk/tools right now). The JTech is a really nice piece of kit though, and if I didn’t need the cutting speed of the CO2 it would work great for me and engraving.
If you’re happy with your feeds and speeds and the results/finish you’re getting versus cutting time, then by all means keep them, experience is king. On my side I felt like with those settings you seem to be close to the lower limit where rubbing could happen, so I’m still curious whether you get any hint of burnishing on the edges ?
The discussion above seems to indicate that you could push feedrate quite a bit (probably x2 or x3) and still be fine, maybe just try that on a sample cut and see what happens. I would not increase DOC by much if I were you, slotting is hard and 40% of the endmill diameter is in the comfort zone. But @gmack would probably recommend using a DOC up to 100% of the diameter, and that may very well work out fine too at those high RPMs.
I try to keep stuff simple, while I really appreciate the science and work behind all of the speed and feed recommendations, I usually just stick with a really basic formula for wood.
DOC=1/2 of bit diameter
Speed = 60 IPM for 1/4", 50 IPM for 1/8", and 40 IPM for 1/16" These go up and down depending on the hardness of wood, but should work fine for Ply.
I try to keep my RPM around 18,000
Nothing scientific really, but this works for me.
I do plan on playing around with my adaptive settings though. I usually set Fusion at 0.1 engagement and 0.125 DOC at 60 IPM for a 1/4" Dia, but at some point I want to try going deeper and faster with less engagement. Just to see if I can increase my MRR.
