Hi All,
I’m running the VFD spindle on Shapeoko 5 pro. I’m using a 1/4" 2 Flute down bit. Recommended settings are rpm 18000, plunge 40ipm, feed 80ipm. My attempts so far, I am burning the wood on a contour cut on 0.750" Oak & shredding the edges. I have tried different combos of RPM & feeds with same results.
Looking at a chip load chart for hardwood & 1/4" bit, the chip load should be .009" to .011". The odd thing is, if I use a chip load calculator and input the bit’s recommended settings I get .002" chip load which is way below.
Going by the chip load calculator it says I should use 330ipm to achieve minimum .0091" chip load. This seems excessive. Also, how much should I be taking off in one pass? I have it set for .118" (3mm)
Last question. Should the chip load calculator be depended on. Are the Shapeoko machines capable of reaching the recommended chip loads? Thanks!~
You can also increase the chipload by slowing down the RPM
0.009 = 330 / (18000 x 2)
0.009 = 144 / (8000 x 2)
0.009 actually sounds like a lot for hardwood to me. I would start with 10000 RPM, 60IPM and override the feedrate until you get a nice smooth cut with no burning.
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
I can’t tell you what the actually minimum would be as that is dependent on the tool geometry and carbide grade. However, if you are burning you need more chipload. Either more feed or less RPM.
One other thing this could be that isn’t in your data is chip thinning. Are you taking less than half the tool diameter as a stepover?
Charts and tables aren’t really interchangeable. They are again dependent on the tool geometry and carbide used. So you can’t really take anything from one company to another without at least knowing that they are similar (rake, helix, grade, etc.)
The tool has a recommend RPM and feed that works out to a 0.002" chipload?
It’s not excessive depending on the tool and machine. We regularly have customers running higher chiploads on 1/4" tools without issue.
The how much you should be taking in one pass is a different matter. Although it is tied to chipload. This is due them both being tied to how much cutting force is generated in the cut. The more depth, or chipload, the more force the tool and machine will have to resist.
What this all comes down to is that you need a minimum amount of chipload to cut a chip, sink enough heat to not burn up, but keep the cutting forces down so you are not deflecting the tool or machine. There’s also an issue of surface speed but I’ll get into that below.
If I was going to attempt a guess at this without knowing the tooling here’s what I would be looking at.
First I would lower the RPM unless you have specific recommendations from that manufacturer to run at 18K or ~1200SFM. This is due to surface speed, the material you’re cutting (oak), and not knowing the tool geometry. If I’m going to use a generic number for SFM in oak It’s going to be around 600-800 to account for “generic” or metal cutting geometries in wood. That works out to 9000-12000 RPM on a 1/4" cutter. Again, this depends on the tool geometry but if you go too fast for the tool it will damage the flute and material (plus usually scream).
For chipload I'd probably start around 0.004". That will give you enough room to compensate for direction change slowdowns and still cut a chip with most tooling. I would increase this as I went depending on the deflection and cut quality. Typically you are going to get better quality cut with more chipload until you reach a limit of the cutter, material strength, or deflection.
The pass depth is where you can get away with a lot. I'd use something completely absurd like 0.0313" or 0.0625" and run up the chipload to test for the best cut. Then start increasing the pass depth until you hit a force limit (chatter or deflection). This will let you take a lot of the force out of the test to look for a decent chipload.
Hope that’s useful. Let me know if there’s something I can help with or expand on.
I’ve had good success with that bit (Whiteside) at 60 ipm & 15000 rpm in cherry, maple and walnut. I also use depth of 1/8" and stepover 1/8". That’s a chipload of 0.002" which is about as aggressive as I get in hardwood. I also leave about 0.020" for a full depth finishing pass.
Well sadly, I have discovered why it is chewing up bits and burning no matter what I try. The spindle is running in reverse, counter clockwise. Never in a million years would I have thought that to be a problem on a new machine/spindle. I will need to contact support again
