[wwendorf]

Ok, I have a few questions.

I have typically only machined aluminum and I have no problems running that, but I need to be doing some steel too. I decided that tonight was a good night to start, and, I subsequently snapped off a .25" endmill.

I was trying to machine a "step" into the jaws that came with my vise. I just wanted to do a slot that .15' deep. Normally, I do that in aluminum soft jaws, but it's a new vice and I don't have any soft jaws for it yet so I figured that adding a step into the jaws that came with the vise wouldn't be a big deal.

That being said, here is what I looked up/calculated for feeds/speeds.

Cutter Diameter: .25 HSS
Surface Feet per Minute: 120
Calculated RPM: 1833

Number of Teeth: 2
Chip Load: .003
Calculated Feed Rate: 11ipm

I tried doing a Depth of Cut of .05" deep.

• What the heck did I do wrong?
• How do I choose the SFM and ChipLoad accurately?
• I've been using Whitney Tool I Speed and Feed Calculator for my feed/speed calculation and their only recommendation is .002 to .005 for chip load as a starting point.
• How do I choose how deep of a cut I can make at one time? I was always told that you should take the diameter of your endmill and divide it by 3 and that is usually a safe number. Is this just for aluminum? I didn't think so, but it appears that my thinking is flawed.

If someone can help give me a better understanding of feeds and speeds, I would be forever in your debt. Some of the values have been a guessing game with me and I'm tired of being frustrated with feeds and speeds.

Also, does it mean that I should be able to double the RPM and double the feed rate?

Thanks in advance,
Wade

[txcncman]

I think you selected speeds and feeds for aluminum, not hardened steel, especially the feed per tooth with HSS tool. (I would never purposely butcher the stock vise hard jaws.)

[a1diesinker]

1.What made you think you could cut hardened vise jaws with a HSS cutter.
2.Just buy some soft stock drill and counterbore a couple holes soft jaws done

[wwendorf]

As I stated, I typically have only machined aluminum with very little knowledge of steels of any type.

If you look at the chart on the page I gave, all the settings are for steel. Apparently my problem was that they are not for hardened steel.

As far as why I thought I could cut them, obviously, because I have never used them before, or HAD use for them before, and didn't realize they were case hardened. That would have been the end of my attempt for sure. All my parts used steps in the jaws, so it made sense to have them in the stock jaws.

I'll update my question based on the info you guys gave me.

IF I was using LOW carbon steel, and I used the setting above, would that actually be the correct feeds and speeds?

Would I be able to double the RPM and the speed or would that just cause more problems? If it would cause more problems, how do you increase the speed of cutting, or don't you?

Thanks,
Wade

[a1diesinker]

you have to stay within the SFM your cutter can handle
for HSS in harden steel below 40RC dont go over 50 SFM
If you have to cut the jaws use carbide and stay around 300 SFM
.002 chipload

[wwendorf]

Thanks a1diesinker!

Can you give me an idea where to get at least some idea where to get SFM and chipload for various types of cutter out of various materials?

Those are 2 tidbits of info I have yet to find good sources of.

Thanks,
Wade

[RICHARD ZASTROW]

Cutter manufacturers such as Regal Beloit, Niagara etc.

Dick Z

[wwendorf]

First of all, I found this chart, which, if it's accurate, should help me out a lot:
http://its.foxvalleytech.com/machsho...edratecalc.htm

And, here's another question.

My old mill had a spindle speed of 3600 rpm and I was able to cut .100" deep at 18ipm with good clean results with a .25 endmill. I calculated that with a .0025 chip load in 6061-T6 but had to use a max SFM of 235 because of the max speed of my mill.

Now that I have a spindle capable of 10000 rpm, does that mean I should be able to cut with the same cutter and a spindle speed of 10k at 45ipm?

Here are the values I used in the Whitney feed/speed calculator listed in my first post.

Material: 6061-T6
Cutter Dia: 0.25"
Depth of Cut: 0.1"
SFM: 600
Calc'd RPM: 9167
Num of Teeth: 2
Chip Load per Tooth: .0025
IPM: 45.84

Thanks,
Wade

[a1diesinker]

when cutting aluminum the only thing that will limit you is heat
and adhesion.
I cut 6061 with a 1/2 EM at 10000 rpm 50ipm all the time
If I can get in the OKK I run 20000 and 100 ipm
keep it wet and cool

[wwendorf]

Ok, thanks a1diesinker. That helps a lot. All of my machining has been done at 3600 RPM, I almost feel like I'm starting over with my new machine and a 10K spindle.

I just bought a Tormach 770, so it's a very new experience for me. Needless to say my lack of knowledge about the original vise jaws being hardened was an annoying first attempt with my new machine.

Wade

[txcncman]

Get a copy of the Machinery's Handbook and study the section on speeds and feeds. Reference the tool makers recommendations. All other sources are suspect.

[diamond.3211]

Check out G-Wizard's calculator, it is really dependable in my opinion.

[zero_divide]

Check out this calculation for the situation you have described
FSWizard

For a 0.05 slot in 45 rc steel you have to use 0.001 chipload
Otherwise you will snap the endmill or chip the corners

Your RPM should be around 1000 and feedrate 2.0 ipm.

Generaly it is not a good idea to machine hardened steels with HSS tools. A carbide EM would do a quick job in your case.

Btw FSWiz will recommend DOC depending on your endmill geometry and material being machined.
It also considers length of the tool and other factors. I have yet to hear from anyone who broke anything using calculations from it.

[wwendorf]

Awesome site Zerodivide.

Thanks for the info too. I opted not to machine my hard jaws afterall, but now I at least know what I did wrong.

I also found that doing a .16 DOC in aluminum my speed is only about 8 IPM as it starts to bog down a bit. I figured I can do something more like a .1 DOC and probably step my speed up to 15 IPM. It could also be that switching the type of endmill I use would help out a lot too.

My Tormach 770 has a 1.5 HP motor. So far, i'm pleasantly suprised how nice it cuts and how quiet it is.

Wade

[zero_divide]

when cutting aluminum the only thing that will limit you is heat
and adhesion.
I cut 6061 with a 1/2 EM at 10000 rpm 50ipm all the time
If I can get in the OKK I run 20000 and 100 ipm
keep it wet and cool

With flood coolant we run 1/2" 2fl carbide em's at 10000 rpm and 90 ipm. DOC depends on type of EM and length. But 0.25" deep for slotting with regular length generic endmill is a safe start.

It will take almost 4 HP to make that cut however.
When power is the limiting factor i think its better to reduce DOC and use proper chipload. You will get more tool life this way.

[BOATDUDEGUY]

Get a copy of the Machinery's Handbook and study the section on speeds and feeds. Reference the tool makers recommendations. All other sources are suspect.

I try all the time but I find it not very descriptive
Also I have never had anyone properly explain it to me
Ive gone over and over but does not make sense to me

[wwendorf]

I'll be honest, the FSWizard shown above has been what I am looking for.

It actually includes a calculated chipload and everything, as well as different tool types out of different materials.

I really appreciate the link, and I'm sure you will too BoatDudeGuy.

Wade