tooling recommendation

I'm using as small of a dia tool as I have to basically profile out a knife blade. I'm cutting an annealed piece of W2 Steel that is .200" thick and using a 2 flute carbide finish endmill. No plunge on the tool, all cuts are full face cut though, around the contour. I'm running depth cuts and going .05" deep per cut for a total of four passes. Of course, every cut gets deeper and increases the wall impingement on the tool. I broke the first endmill in the first .05" deep cut. The second broke in the next pass at .100".

I was running 3250 RPM (highest speed on the bottom pulleys) and originally tried running F2, but that broke the first tool within 2" into the cut. I reduced F down to .5 (25%) and made it through the whole .05" pass and half way through the .100" deep pass. So time consuming and slow it is almost unbearable..

I'm thinking I may need a three flute endmill or maybe a rougher (if they even make those that small).

Whatever I do, I'd like to move a little faster on feed and have an endmill that actually lasts, because there will be a lot of the kind of cutting I described. Some will also be in Ti. Not even sure what kind of tooling to go with there.

Thanks.

I haven't cut much steel so I can't help there, but I have a couple questions that might help someone else give you recommendations...

What is the diameter of the tool you've already tried?

What do you mean by "each cut is full face"? I'm guessing that's another way of saying "slotting" or "full width" cutting.

Do you need to use a very small diameter cutter? If you're using one to maximize the number of blades you can make from one piece of stock, perhaps getting one less blade out if a piece of stock would be worth being able to cut them faster and more reliably. If you're using one because it's required to get into one area with a lot of detail, perhaps milling the majority of the profile with a larger end mill and milling the small detail as a seperate op would be a good idea.

a .250 cutter may be OK at .050 depth of cut, flood coolant and 5 ipm 3200 rpm.

I cut 18 feet of 304 ss with a .25 carbide 4 flute at 5ipm 2500 rpm .035 doc FLOOD coolant. The tool steel will tend to harden if cut at too high an rpm and no coolant, just the heat generated cutting it will cause the edge to harden if no coolant is used.

Would be nice to know the cutter size, doc coolant feedrate rpm etc. the more info the better.

I'm sorry I didn't specify size. It is a 1/8". I'm trying to keep the size as small as possible because this particular piece of blade steel is very expensive. Sometimes I buy forged pieces of stock from makers because I do not forge myself. This particular stuff is called San mai, and it cost around $200 for this piece, which is 14" x 2" x .200" thick. I can get two blades out if as it sits, but I am trying my best to minimize waste. On a cheaper piece of bladensteel it would not be such an issue, but it is here. I may have to move up to a 3/16" or 1/4" to finish, but I hate to waste the stock from the wider kerf.

Yes, full face means full width or slotting.

Also meant to mention, this particular piece of steel is actually two different types in layers. It is 410 cladding I believe, with W2 in the middle. Think a peanut butter and jelly sandwich, with the 410SS being the bread and the W2 being the jelly.

How thick is the 410SS cladding?

410SS has a 125 sfm (carbide). That means 2000 rpm max with a 1/4" cutter.

W2 has 256-384 sfm (carbide). That means faster than 4100+ rpm with a 1/4" cutter.

If the cladding thickness is more than your first DOC, than you need to slow it down.

EDIT: whoops, I see you are using a 1/8" cutter. Disregard my last....

Forward: I have never tried machining the steel you are working with and have zero experience with what you are trying to do.

That being said, have you tried going to a smaller end mill and using HSM-style paths (lots of tiny circles) instead of slotting? For example: Use a 1/8" end mill for a 0.130" wide slot, but use a stepover you are comfortable with instead of slotting. I have done this on hard steel and it made all the difference for me.

Take a look at some of John Grimsmo's videos on youtube. He has quite a few ops with end mills that size.

I've never seen that type of path, but I bet that it would make a difference. I stepped up to 10k rpm and F2, and it finished the job. It did something I've never seen though. In the kerf of the cut, it left a wake of pretty much melted metal. Flood colla t on so no hot steel or glowing orange (to the eye anyway). I could take a sharp tool like a dental pick and break it away. I thought for sure it would grenade the tool when it came around and hit again on the next pass, but suprisingly it cut it. I ended up slowing down to a little less than 10k rpm and the same feed to finish with not so much of that melted metal in the wake.

Grimsmo did a video the other month on profile cutting his blade blanks.In the end, he decided it was not worth it to try and cut the blanks himself, and will continue to use a local waterjet company to make the blanks.

But if you do want to try profiling your own blanks, then look up this video and you can see what worked for him. He still ended up breaking quite a few tools, even once the cut recipe seemed to be dialed in.

im not super experienced, but it was my understanding you should used 4 flute with steel. 4 flute is stronger than a 2 flute cutter and you can feed faster... altho with a 1/8" you might be maxing out your RPM anyways, but you would have to do the calculations on that.

Two flute was all I had on hand. I will definitely go four next time. I know that it would probably be more efficient to water jet or laser out blades and parts, but I'm trying to keep as much as possible in house for the time being. I don't do that much volume yet. Hopefully this machine will change that, and when it starts picking up, I'll then start jobbing things like that out.

Mike C8, thanks for the recommendation on the vid. I watched it and that was almost the exact thing I was doing. I have no idea how he got as high as 11 IPM feed though, maybe that is possible with a four flute and steel that is the same all the way through. I was happy to see 2 IPM when I turned my spindle up to 10k.

I've been watching some of his vids. He has some great ideas and seems to have no trouble sharing how he does things. He is a great resource for the path I'm on.

4 flute, quality end mills, and as short of a flute with as little stickout as possible will help you reach higher feed rates.

Definitely use a 4 flute. It is much stronger. Use a good quality solid carbide mill with a good coating for steel. If you are only cutting .2" thick material buy an end mill with only a 1/4"flute length or at least no more than 3/8" if you can't find 1/4". I recommend using an ER collet to get low runout and keep the cutter stickout as short as possible. Download a copy of Gwizard to get the recommended speed and feed.

At that price, I'd consider getting it waterjet-cut to net shape. Or the poor man's waterjet, aka vertical bandsaw.

How much do you really gain by using a 1/8" EM versus a 1/4" or even 3/8" one? I get it if it gets you another blade out of a piece of material, but it's not clear what you're really gaining. A .250 4-flute roughing EM would probably eat that in two or three passes easily.

Either way, you need to use a feed and speed calculator and a 4-flute tool. Use the harder material to determine the settings. Oh, and you will want carbide for this, otherwise it's a fool's errand. And flood coolant or an air blast to clear chips. If you insist on punishing yourself with a 1/8" EM I'd consider two passes per depth offset by say .05" so that you have more chip clearance and less tool flex to contend with.