6K vs 10K Spindle Speed For A2 O1 3V Tool Steel

First post and a question about spindle speeds(rpm).

A little background first:
I'm new to cnc (rank beginner) and in the process of purchasing a Haas(Minimill or TM1) for my knife making business. I work with O1, A2 and CPM 3V tool steels .125" thick +- and at present use a local waterjet cutter to cut out two parts from 12"x36" plate.

The main piece (fixed blade blank) is fairly simple with 1/4" and 5/16" holes cut in the tang and flat grind bevel of 12deg. The second piece has a 1/2" long slot .125" wide and cut through the material(.125").

I have looked at several speed and feed calculators and gotten a rough idea as to what spindle rpms might work but because of my ignorance on the subject am not sure as to the type of tooling best used for each process, and don't know how many teeth or chip rates to put into the calculation as well as having no experience in milling these materials other than band saw and grinder am at a bit of a quandry.

If possible I would like to use .125" end mill(?) for cutting out the profile of both parts to decrease waste and maximize the number of parts per unit of steel plate, and also for the slot in the smaller piece. I understand smaller tools need faster speeds to make up for surface area, however I am not in need of running hundreds of parts every month so slower feed rates might be an option.

So my question/s : Will the 6k max spindle speed rating work for this application or would the increase to 10k(and possibly $3800 increase in price) be a better option?

Thanks for your time and looking forward to your insight.
mtnscout

For a 1/8" endmill, the circumference is 0.0327 feet. So a 6K RPM spindle will give you 196 SFM, while the 10K spindle will give you 327 SFM. The latter would be more effective with carbide endmills. If you are using HSS endmills, the 6K spindle would be ample.

For an 1/8" endmill, most often 2 teeth, sometimes 3 or 4 teeth, no more than 6 teeth. This affects feed (and finish), not spindle speed, as you'd want to hold the feed-per-tooth at a fixed target value. Since 1/8" endmills are not very strong, let's say 0.001"/tooth. With 2 teeth and 10K RPM, that's 20K teeth/minute or 20 inches/minute feed. If you can find a 6 tooth 1/8" endmill, you'd get somewhere between 20 IPM and 60 IPM feed, depending on how much you want to risk snapping it off. With such small tool flutes, you will want copious coolant to flush out chips.

I'd be inclined to use a bigger diameter endmill for profiling, as it would allow higher feeds with less risk of breakage or flute clogging. It would also get the SFM up higher to better exploit carbides with modern coatings.

[Added in edit] In fact, people will tell you that you can't properly rough with a 6-flute 1/8" endmill at all because the flutes are just too small for the volume of material being removed. Probably fine for actual profiling of your parts, but not for cutting them from the sheet. For that, use a bigger endmill with fewer, larger flutes, and take the hit on feed.

mtnscout said:

I work with O1, A2 and CPM 3V tool steels .125" thick +- ...

If possible I would like to use .125" end mill(?) for cutting out the profile of both parts to decrease waste and maximize the number of parts per unit of steel plate,

Click to expand...

Assholic comment from someone who is only 80% into his workweek on a Friday night ....

Seriously? O1, A2 or even CPM10V is worth more than a 1/4" or 3/8" carbide endmill's kerf as waste?

If You want to decrease waste and maximize number of parts, you better be talking about tens of thousands of parts to start with!
Less than that number, have it saw cut to near-net, fixture it correctly, use the biggest tool to rough and the biggest tool to finish it.

sfriedberg said:

For a 1/8" endmill, the circumference is 0.0327 feet. So a 6K RPM spindle will give you 196 SFM, while the 10K spindle will give you 327 SFM. The latter would be more effective with carbide endmills. If you are using HSS endmills, the 6K spindle would be ample.

For an 1/8" endmill, most often 2 teeth, sometimes 3 or 4 teeth, no more than 6 teeth. This affects feed (and finish), not spindle speed, as you'd want to hold the feed-per-tooth at a fixed target value. Since 1/8" endmills are not very strong, let's say 0.001"/tooth. With 2 teeth and 10K RPM, that's 20K teeth/minute or 20 inches/minute feed. If you can find a 6 tooth 1/8" endmill, you'd get somewhere between 20 IPM and 60 IPM feed, depending on how much you want to risk snapping it off. With such small tool flutes, you will want copious coolant to flush out chips.

I'd be inclined to use a bigger diameter endmill for profiling, as it would allow higher feeds with less risk of breakage or flute clogging. It would also get the SFM up higher to better exploit carbides with modern coatings.

[Added in edit] In fact, people will tell you that you can't properly rough with a 6-flute 1/8" endmill at all because the flutes are just too small for the volume of material being removed. Probably fine for actual profiling of your parts, but not for cutting them from the sheet. For that, use a bigger endmill with fewer, larger flutes, and take the hit on feed.

Click to expand...

Thanks for the info. helps me understand the process better. I did a quick layout with the parts and 1/4" over 1/8" works fine, might even be able go a little bigger. I'm not too worried about the feed rates, being a one man shop putting together a half dozen knives a week, doubling that would be sprinting for me.

SeymourDumore said:

Assholic comment from someone who is only 80% into his workweek on a Friday night ....

Seriously? O1, A2 or even CPM10V is worth more than a 1/4" or 3/8" carbide endmill's kerf as waste?

If You want to decrease waste and maximize number of parts, you better be talking about tens of thousands of parts to start with!
Less than that number, have it saw cut to near-net, fixture it correctly, use the biggest tool to rough and the biggest tool to finish it.

Click to expand...

No problem on the "Assholic comment", crappy work schedules suck.

Thing is, in my world, for every extra knife blank I can cut out of a piece of plate, I'm potentially putting another $200 in my pocket. My production numbers are small, friggin' tiny compared to what most on here produce. If I can put out 40-50 knives a month compared to what I do now I'll be in the gravy. Even with the cnc work there will still be a fare amount of hand work finishing to complete each knife not to mention the sheaths. So speed is relative for my needs.

Get the higher RPM or you'll kick yourself later. You'll decide to engrave a nice decorative pattern or something and be stuck at glacial feed rates. Or you'll want to do some aluminum or brass handle bits that want as many RPMs as you can throw at them.

SeymourDumore said:

Assholic comment from someone who is only 80% into his workweek on a Friday night ....

Seriously? O1, A2 or even CPM10V is worth more than a 1/4" or 3/8" carbide endmill's kerf as waste?

If You want to decrease waste and maximize number of parts, you better be talking about tens of thousands of parts to start with!
Less than that number, have it saw cut to near-net, fixture it correctly, use the biggest tool to rough and the biggest tool to finish it.

Click to expand...

No problem on the "Assholic comment" crappy schedules suck. Probably shouldn't have put in "waste" in my comment but for every extra blank I can get out of a sheet of steel I potentially put an extra $200 in my pocket.

mhajicek said:

Get the higher RPM or you'll kick yourself later. You'll decide to engrave a nice decorative pattern or something and be stuck at glacial feed rates. Or you'll want to do some aluminum or brass handle bits that want as many RPMs as you can throw at them.

Click to expand...

That's what I'm thinking, just figured I'd check to be sure before I through more money at the it.

For knife work you want the 10K. Even if you're not using it for the profiling, if you ever want to do some fancy 3d machining on the blades or handles, or you need to put a lockbar slot in with a 1/32" endmill, you're going to be glad to have the RPM to spare. I just did a run of knife blanks for a friend of mine in S30V steel and 6Al4V Ti. Most of it was spent around 5k with a 5fl 1/8" endmill, and the blade bevel was contoured at around 8500 for the roughing pass and 12k for the finish pass with smaller ball endmills. Also ran some carbon fiber and micarta, both topped out on RPM in my HAAS VM3. On either of my other machines with lower RPM it would have taken twice as long.

npolanosky said:

For knife work you want the 10K. Even if you're not using it for the profiling, if you ever want to do some fancy 3d machining on the blades or handles, or you need to put a lockbar slot in with a 1/32" endmill, you're going to be glad to have the RPM to spare. I just did a run of knife blanks for a friend of mine in S30V steel and 6Al4V Ti. Most of it was spent around 5k with a 5fl 1/8" endmill, and the blade bevel was contoured at around 8500 for the roughing pass and 12k for the finish pass with smaller ball endmills. Also ran some carbon fiber and micarta, both topped out on RPM in my HAAS VM3. On either of my other machines with lower RPM it would have taken twice as long.

Click to expand...

Thanks for that. I forgot to to mention I do use micarta for scales so looks like the higher rpm will be mandatory.

Hello,
If most of your material is .125 thick, your end mill budget will benefit from buying double end stub length cutters. Four flutes, with the best coating that you can find.
If you are cutting phenolic for scales, be advised that the shit is considered to be carcinogenic. Please read the MSDS sheet that should have come with the material. I finished one run of parts from that stuff, and vowed to take no more into the shop. The best plan would be to situate the machine next to an exterior wall. that would help with ducting the nasty yellow flour out into the "big sky", or into a large tub of water in another area. The particles will clog any type of filter media quickly.
Best wishes on your project. Brand name?

Chip Burns said:

Hello,
If most of your material is .125 thick, your end mill budget will benefit from buying double end stub length cutters. Four flutes, with the best coating that you can find.
If you are cutting phenolic for scales, be advised that the shit is considered to be carcinogenic. Please read the MSDS sheet that should have come with the material. I finished one run of parts from that stuff, and vowed to take no more into the shop. The best plan would be to situate the machine next to an exterior wall. that would help with ducting the nasty yellow flour out into the "big sky", or into a large tub of water in another area. The particles will clog any type of filter media quickly.
Best wishes on your project. Brand name?

Click to expand...

Ive never hear of phenolics being classified as carcinogens...quick research showed the same.

We no longer use msds, is now sds...thanks to the ghs lol