Hi Everyone,
Using a Shapeoko Pro5 with VFD Spindle I am machining a paper-resin material (.50" & .25" Thick) with these tool bits. Has anyone used ones like these? If so, any recommendations to the …
Feed & Speeds, Ramping, etc. to use?
Thank for any help ~ KAP
There are links to download the tool data in the user guide
Hi Tod1d … Thanks for the link. I did look at that matrix. Can you tell me what the part numbers are for these tools so I can look at the F&S for these? Maybe I am just missing them in the chart.
Cheers~KAP
It doesn’t really say in the Amazon page. I’d guess by the sizes it must be the 70C15 series. (1.5mm - 3.175mm). Double check the product numbers when you get them.
I will. When I finish this project I will share my results here. Hopefully all goes well …
Thanks for the help ~KAP
A $4,500 machine using cheap Chinese $1.40 bits? My expectations would not be high for their cutting ability or longevity.
Actually I have some of those still in my bit holder. Bought them when I got my machine. YES they are not the best. Broke a bunch of them. I used them to teach me (didn’t know it at the time) how to use the machine.
I know their limitations treating them so. A cheap bit that works is as good as an expensive bit that will do the same thing.
I know time, messed up cuts and dollars spent.
I actually go through a lot of $5 1/16 inch SpeTool 0 Flutes and don’t see a reason to pay for a more expensive bit. But then again I just purchased an Amana 1/6" spiral bull nose for $65 and had tried several other lower-priced bits, go figure.
For wood and aluminum, the best performance is achieved when the router/spindle speed is maximized (24000 RPM for Carbide 3d and other Chinese spindles). The attachments show that, with the exception of Yonico, most suggest 18,000 RPM for wood.
Amana.pdf (514.8 KB)
Freud.pdf (211.7 KB)
SpeTool.pdf (194.3 KB)
Yonico.pdf (1021.0 KB)
Whiteside’s vary with product.
Everything has been telling me 18k, so you are saying I should crank the VFD up to 24k?
If you have cutters that are rated for that speed (safe and adequately balanced), your cutting forces for the same material removal rate should be reduced by 18/24 by running at 24k rather than 18k RPM. If you have a constant torque HF Spindle (kike Carbide 3d’s), you should be able to get 24/18 times the power out of it.
All of my cutters are Amana, most are Spektra bits. I have Carbide’s VFD.
These are diamond-cut router bits with most likely a nACo coating. They are typically high RPM low feed as they are a grinding not cutting tool. An example for a 0.0625" would be 50IPM (1270mm/m) at 37,000 RPM.
They may or may not work for that material. It will depend on the hardness of the resin. If it’s even a little soft or temperature sensitive it will load the tool.
Never really understood this as you should be targeting a surface speed and that changes by the diameter. My assumption has always been that they are just using a point inside the acceptable range of the listed tools. There’s also different best surface speed based on the wood type.
Hope that’s useful. Let me know if there’s something I can help with or expand on.
But their download speeds and feeds show a 9,000 RPM maximum.
Like Whiteside does.
That’s because their test machine only goes to 9KRPM.
In fact if you look at that list they use 9KRPM for everything other than the acrylic. Additionally, if you’re going to go by that they only recommend these for roughing wood.
In my opinion, that sheet isn’t going to be worth much for anything other than potentially that specific machine. It’s too deflection, feed, and power limited to tell much for other machines.
These cutters are from the PCB industry and designed for machining FR4. They can be used in other materials but they really want hard materials at very small chiploads. Anything not hard enough won’t cut well, especially at low RPM.
Yeah, there are a number of manufacturers that do. My comment was specifically at the everything at X RPM sheets. I guess it makes simple to follow instructions. In my opinion though it makes for more confusing data as you are locking one of the variables that should be moving (assuming similar geometry).
As you can see in the attachment, it seemed a lot more difficult than it should have been to get an Amana rep to finally say that the maximum speed for their 46102 endmill is 28k RPM. Everything else, including their Vectric tool data base recommends 18k RPM.
Tools Today Amana Endmill Speeds.pdf (115.2 KB)
Interesting for sure.
I’m wondering if i should stop using the coated bits (The K models). The noise is horrendous, i’m trying to play around with speeds and feeds to reduce the noise. I just ran another part and increased the RPM to 20k, but reduced my feed speed to 80 and it was louder than the previous 18k RPM and 100 SPM. Same depth of cut. I’m using the 46416-k which is a 1/4 downcut bit. It’s my main bit to keep my work piece edges smooth and be able to cut 1" deep.
I was going to say something about my previously listed bias… But apparently I forgot that in the first post and can’t edit it so…
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.
Said bias being listed there’s a couple things here in general I can address.
First is that coatings are not a total positive. When you are coating a tool you coat ALL of the tool including the leading edge. That has the effect of slightly dulling the edge in exchange for an increase abrasion resistance, surface hardness, and lubricity (depending on the coating). If it’s worth it, or “better” depends on the base tool, the material your cutting, and failure mode.
Noise is commonly caused by a few factors. Too little chipload, too much surface speed, deflection (bit, machine, or both), and poor hold down.
First, let’s assume that you don’t have deflection and you have good hold down. That leaves us with chipload and surface speed. Your 2 listed cuts are 20KRPM at 80IPM and 18KRPM at 100IPM. The 18KRPM at 100IPM works out to 0.0028" chipload, the 20KRPM at 80IPM works out to 0.0020" chipload. So if you want to see if the SFM is effecting the noise you need to run at either of those chiploads at the different RPMs to actually test it:
0.0028" chipload
0.0020" chipload
Additionally, I would probably give a bigger delta as with a 1/4" cutter 18KRPM is 1178 SFM and 20KRPM is 1309 SFM. So only 131 SFM difference between them. Don’t know your RPM range but I’d try to get at least 300 SFM delta to test with.
The easiest way to test if deflection is causing it is to just chop the pass depth on a cut at the same feed and speed. That will give you less cubic material removed per flute, per rotation, while maintaining the chipload and surface speed. If you want to drill down on this further there’s a simple deflection test you can do that I previously posted: Nomad 3 tolerance in aluminum? - #43 by TDA.
Can’t really help much with hold down. There’s not really a good test for it that I’m aware of.
Depending on the results you can play around with things to get the best cut/performance.
Hope that helps.
Very helpful thanks.
I was going to set up a cut piece with different tool settings and see what happens.
I’ll check out your company bits too, always willing to try a few and see what works best.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.
