I have yet to upgrade the V Wheels to linear rails. I actually been looking into that. What would you say is the max DOC if I were to stay with V wheels while keeping my machine “happy”?
Thanks
I would try running at a 0.025 axial, 0.230 radial at 24krpm and 100ipm. That will net you a 0.0014 chipoad and higher mrr with less force than your high depth cut. Also you’ll probably be able to feed override it almost to 200% depending.
Bonus thing about cuts like this is the floor finish will tell you exactly what the machine likes. Each cut is different, it even depends on which direction you are cutting.
Ide think about some 0.375 endmills to effectively increase your sfm a bit. Bigger shank really helps when sticking it out there as well.
4 Likes
I see. Based on your IPM, I assume this on a quarter inch cutter with 3 flutes. What about the advantages of single flute?
Yep, this.
The Shapeoko has a whole series of mechanisms of deflection and they are absolutely not symmetrical between X, Y and Z.
Floor finish is key not just from the horizontal movement but due to the coupled Y-Z nodding movement of the Z carriage on the V wheels tracking the X rail.
You’ll learn the sound pretty quickly, I’ve found that fiddling the spindle speed and feed rate can frequently get the machine out of a resonance mode, it’s not always going slower that’s the answer and I’ve found that, for example, 22kRPM works a lot better in X traverses than 20kRPM for single flute cutters, that’s just the harmonics of my Z carriage and spindle.
4 Likes
And that’s also not even getting into different tool balances/geometry. Its an interesting game for sure.
A 3/8s, chamfer tip Destiny Diamondback would probably run very well at 20krpm.
If chip clearance/evacuation is an issue then try less flutes.
5 Likes
I used Kennametal’s 1.76 K-factor for that endmill with the cutting parameters shown in the workbook. The cutting parameters were chosen to minimize cutting forces while keeping within Kennametal’s calculated acceptable operating range for the endmill. Similar parameters for the 1/2" version of that endmill are shown here. If you compare predicted performance with the 1/4" endmill, you’ll see that the 1/2" endmill should further decrease cutting forces. (They should be cut in half at the same MRR). Chip clearance should be improved with the larger endmill too.
I’ve learned from @spargeltarzan and others that K-Factor is dependent on much more than the just workpiece material. Cutter geometry (rake angle, edge radius, helix angle, etc.,), chipload, and the use of lubricants can have a significant impact on it. So, calculators that consider those factors should provide much better estimates of milling performance. Kennametal’s probably does that, as does the “new kid on the block” Millalyzer.
4 Likes
Be interesting to see more about at what size the multi-flute cutters become more effective than the single flute in non-clogging, dry chip evacuation. As the cutter gets bigger the flutes between the faces get bigger and if you’re doing n cuts per rev instead of 1 cut per rev then presumably your chips can be smaller at the same MRR (i.e. not having to push to max per tooth cuts).
I ordered a 10mm 3 flute to play with.
To walk before I run? 
Do you run that dry or with air blast / lubricant?
1 Like
Haha, I understand that. However I personally couldn’t pass up this tool deal before its price goes back up to $100.
I’m actually 100% dry nowadays, ya know, smaller sweetspot, really put cam to the test. Probably should learn how to use the Millaylzer one of these days.
1 Like
That looks like a nice cutter, once I’ve done the linear rails maybe…
I nearly bought this;
but figured I’d stay uncoated so I could see the result of just changing the no. of flutes from the single and two flute 4 & 6mm I’m running at the moment;
It’s cheap enough to experiment with.
So far I’ve managed to make the 2 flutes work really well on exterior adaptive clear and contour where they can throw the chips away from the workpiece but still learning how to keep them happy in a pocket. I’m also being stingy and working my way up the DoC instead of the WoC because I’d like to use more than the bottom 1mm of the cutter.
Whilst you’re here and we’re talking big cutters…
What do you use for facing with?
Have you found anything with inserts that will run in ER20 size collets that’s actually balanced?
I saw these sorts of things;
https://www.amazon.com/12Pcs-C12-12-130-Holder-APMT1135PDERDP-Wrench/dp/B07QGBKQTJ
But in the 10 and 12mm sizes they appear to have a single insert and don’t exactly look like a balanced tool for high speed spindles.
These fly cutters would fit in a ER20 collet; haven’t tried them. Question is whether your spindle can run slow enough - what’s your minimum RPM ?
I tired something similar but I think their max RPM at 5k, the minimum spindle RPM is 8k.
2 Likes
I’ve been able to run mine reliably at 800-1,200RPM for the edge finder, the VFD has a silly value for min RPM. Running at 2,000-2,500RPM for spot drilling it has lots of torque and seems quite happy.
My concern is the lack of balancing on a fly cutter, the Shapeoko just isn’t rigid or heavy enough to take those out of balance cutters or the heavy loads in an out of balance large radius cut. The single flute cutters are OK but they’re < 8mm diameter and balanced to run at 20,000RPM taking tiny cuts.
Ahh - So you should be able to see some significant motor currents when drilling at those low RPMs? Maybe another argument for those monster water cooled spindles?
Not much current, only running a teeny feed rate to avoid the rumble and more importantly the down-force from the HDZ can bend everything else really easily. I’ve got the 3, 4 and 5mm spot drills working really well at
2500RPM
30mm/min plunge
0.012mm / revolution
which with some isopropanol lubricant and a retract every 1mm gives a nice curly continuous chip and a clean hole.
800 RPM sounds more reasonable.
Let’s say the small fly cutter has its centre of mass 4 mm out of centerline, then at 1200 rpm that would mean 6g centrifugal acceleration. How much does that thing weigh? 150g maybe? Would be 9 N centrifugal force, rough estimate. That half-inch cutter discussed above will certainly generate way larger radial cutting force contributions than that…
Have wanted to try Sensorless Vector mode, but still haven’t got my spindle installed, I did try to enable it on the bench once but didn’t work out of the gate (I have a different VFD (than in the video) that offers the mode but with limited parameters).
I missed that - what was it?