What's new
What's new

Can you machine steel in a Mini Mill?

rjibosh

Hot Rolled
Joined
Jul 22, 2003
Location
Los Angeles
The machinists that I know look down at Haas as the "Aluminum Machines". Does anyone use a Mini Mill for steel or stainless work? I'm not talking high production runs. Just under ten part batches removing 1 to 3 cu inches of metal per part. Facing, grooving and pocketing. No time limits. Need good to very good finish. Is a Mini rigid enough for this and does the spindle generate enough HP at under 1,000 rpm to to make .250 cuts with a .5 end mill? Also would you recommend coolant or oil?

Thanks,

Rick
 
Of course you can machine steel. I worked for a medical supply company and made hundreds and hundreds of 304 stainless steel parts with it. Some with heavy roughing too. Just make sure you get plenty of coolant to the endmill. Ours had no programmable coolant nozzle and a small pump so that was a challenge sometimes.

The machine was fine and held + -.0002 all day on 1/2 inch thick parts.

Oh, coolant not oil. Oil is a good lubricant but does not dissipate heat well at all.

Mike
 
Mini Mill and steel

I cut M4, D2, and O1 with a Haas Super Mini Mill 2. I use Blasocut 4000 for coolant.

If you want, I'll cut a part for you so you can check surface finish and report back loads.
 
2 for "of course you can"
don't know speeds and feeds but i've got one that makes all sorts of steel parts
there not hoggers, but they don't cost like one either
 
Are you doing those parts for yourself or for a customer? Specify a stainless steel that´s easy to cut, there are very nasty steels that are hard on machine and tool.
 
Use one of the Hanita style carbide vari-flute endmills and you'll do ok on both steel and SS. They work particularly well on "not so rigid", "not so powerful" machines.

These ones work well for me and are priced nicely:

Single End Variable Flute End Mills - MariTool

Check out the speeds and feeds chart on that page, for steel you'll want 500 SFM so your 1/2 endmill should be at 4000 RPM. Even with the toughest SS you'll want to be at around 2000 RPM.

Full slot width at .250" will be fine. At that WOC and DOC in steel you need about 1HP at the spindle for every 8 ipm of cutting. Take the HP rating of your machine and cut it in half (remember we're talking HassPower here) and that will set the high end of your potential cutting speed, so a 10HP machine means maybe 5HP usable at spindle, 5 x 8 = 40 ipm.

But that's your max, start out at half that and see how it goes.

These TIALN coated endmills like the heat, so they work best with just an air blast, but makes sure the chips are getting cleared well with the blast to avoid chip re-cutting.

Good luck-

Paul T.
Power Technology
 
A HAAS minimill is an extremely effecient mill for steel and stainless steel if you us the right endmills. I myself have ran inconel on one at 250 ipm and 17-4 stainless at 500 ipm. Just use the high speed machining method with a stepover of .025 to .05 . most materials do not need coolant with this method.
 
Machine cutting limits Excel chart

i use an Excel chart that automatically calculates speed, feed, and depth of cut AND also takes into account an end mill cutter length factor and number of flutes. Long end mills obviously cannot take as much load as shorter ones. Also long tool holders obviously cannot take as much force.
.
more importantly the chart auto calculates cubic inch per minute removed. The Excel chart auto calculates feed, speed, and depth of cut in the end mills normal power usage range. So using the chart to find a bigger end mill with higher inch per minute removed you find ALL machines have a cubic inch per minute removed when motor will stall from lack of horsepower or machine will vibrate and chatter as to make any higher cutting rates destroy the end mill cutter.
......point is ALL machines once you find the maximum cutting rate in cubic inches per minute that they can handle all you need to do is not exceed that rate.
......also another factor is material being cut. machinabilty rating for free machining Steel is 1.0, Hot Rolled steel 0.8, SS around 0.4, Aluminum is around 3. This means you can cut 3 times more cubic inches per minute of Aluminum than free machining steel. So once you know how many cubic inches per minute of free machining steel your machine can handle you can use the machinabilty rating to calculate what your machine probably can handle in cubic inches per minute of other metal alloys.
....... by doing the math and studying the engineering forces you can scientifically increase machining speeds often 10 or more times than what a machinist originally thought was the fastest.
....... attached is a zip file with the free Excel file. check all formulas and calculations it suggests and make sure you take precautions against breaking end mills, parts moving in vise, stalling motor out, bearing damage, etc. Excel file needs to be copied out of zip file and put in a folder to change it. When opened from a zip file it is usually in read only mode. Feel free to edit Excel files formulas that it uses to calculate. The length factor can be easily changed so if you want to use an extra extra long end mill a different length factor will better predict what feed and depth of cut to use.
...... i find the Excel file has increased my machining times as many as 14 times faster. As long as vise can hold the part. often if you really must use a certain size end mill the excel chart can give with slower sfpm and slower feed AND the cubic inches per minute removed and as long as that amount is below your machine limit for that metal alloy it should work ok, usually.
 

Attachments

  • SpeedAndFeedCalculator.zip
    4.7 KB · Views: 1,287
TomB
1st, thanks for sharing your excel table.

I was hoping you could help me with a question on it?
How have you adjusted the values if your mill can't reach the calculated RPM? If you adjust the spindle speeds to meet your machine's capacity, how do you balance the feedrate? Ex: I have a mill that tops out at 8000rpm and 200ipm. Using your table, I calculated a speed and feed for cutting AL with a 0.125", 2 fl carbide endmill is 18,336rpm & 24.1 ipm. How would you adjust the values?
 
If somebody tells you that a Haas cant machine steel, hes NOT a machinist.

I machine more steel on my Haas machines than Aluminum. Its all in the tooling and programming.

You dont need to take huge cuts to machine steel.
 
TomB
1st, thanks for sharing your excel table.

I was hoping you could help me with a question on it?
How have you adjusted the values if your mill can't reach the calculated RPM? If you adjust the spindle speeds to meet your machine's capacity, how do you balance the feedrate? Ex: I have a mill that tops out at 8000rpm and 200ipm. Using your table, I calculated a speed and feed for cutting AL with a 0.125", 2 fl carbide endmill is 18,336rpm & 24.1 ipm. How would you adjust the values?


This thread is close to 5 yrs old...........................start a new thread.................................
 








 
Back
Top