How should I remove more metal faster???

jumps4

jumps4

Global Moderator
Registered
i have a question about milling steel (hot roll)
today on my new mill i ran at 1.9 ipm a depth of .030 per pass and 620rpm 1/2"hss 2 flute cutter and it cut perfect no strain perfectly smooth no heat i just added a few drops of oil each pass. it took 46 minute to go 1/2" deep
now my question is if i wish to push it harder to get finished sooner less caring about finish more about removing more metal faster.
would i cut deeper, move faster or both?
are more rpms needed if moving faster?
at what point will i need flood cooling?
or is this good leave it alone?
steve

DSCF0290.JPG DSCF0289.JPG
 
Your feed rate seems right for the end mill, and the material (70 SFM for steel with a HSS end mill shows about 560RPM, 620 is pretty close). At 1.9 in/min that should give you about 0.0017" chip load, which is good, but you could probably go a bit higher (maybe try 2thou?). The easiest way to increase feed rate is to go to a 4flute cutter. With that you can double your feed rate without changing RPM or tooth load (to say 3.8). You could probably go much deeper than 30though too, assuming your machine is rigid enough (is this the Z45 you have been converting?).

http://www.niagaracutter.com/techinfo/common_mat/a36.html

I tend to refer to the Niagra website for feed/speed info, even if I am not using a niagra cutter (use the low end if you got the Enco special end mills). You are cutting a full width slot, which tends to be one of the toughest on mills for engagement. Niagra recommends only 50 SFM in steel with an uncoated cutter at 1/8 depth. But even 1/8th depth is 0.0625, which is twice what you have been doing.

So, I figure if you move to a coated 4flute cutter, and increase your depth to about 60 thou, you should be doing ok. Maybe start your feed out at 2.8 and ramp up slowly if you don't run into any issue.

Of course, going to carbide cutters will get you even more, but they tend to be a little more sensative to thermal shock and it's easy to chip the cutters if you are too agressive, or if you get a lot of chatter/vibration.
 
Last edited:
Your feedrate and your cutter surface speed work together to form your chipload. The chipload is limited by the cutter and the HP available. Ultimate surface speed of the cutter is determined by the nature of the cutter. Naturally, plain HSS won't run as fast (and hot) as some with cobalt mixed in, and yet not as fast as carbide.....and faster yet with various coatings. Lots of variables just in the type of cutter. Then comes all the material variables that help pick the best cutter, that chooses the best chipload, speed, feed, etc. It can be complicated. Have you ever done any roughout work with corncob end mills? They can take substantially heavier feeds, although not so much more speed. So end result is faster metal removal. Inserted end mills are worth looking at if you have lots of rpm, but maybe not so much hp. But they like a rigid, stable setup.
 
no tony i have done little to no work in steel my harbor freight and sherline mills just could not do much
steve
 
ok tomorrow i'm going to try a four flute at .050 and 2.0 chip load and see how the mill does
is that correct?
steve
 
One thing I would add is that if you are shooting for a 0.5" slot and dimensions are important at all, go with a slightly smaller end mill, cut the slot to depth (in passes if you need), and then clean up the sides at full depth but just taking off the last 10 or 15 thou on each side. Slotting tends to be pretty nasty at the best of time. There is not a lot of room for chip clearance, so you get a lot of chip re-cutting. That can lead to a really bad finish (you can read that as "every time I have tried it have have ended up with a finish that looks like wall texture). You can also get a lot of deflection when slotting, so doing things with a smaller end mill and a cleanup pass will let stay on target.

Most CAM packages have settings for roughing/finishing passes. It's a little tedious, but not hard to do if you are coding by hand (which is what I have done on all my CNC projects so far).

If your machine is anything like my X2, you may be better off with a smaller end mill, crank up the feed rate and spindle speed, and just take more, smaller, cuts. You have lots of spindle speed available, and you can use it more effectively with smaller cutters.
 
jumps4 said:
ok tomorrow i'm going to try a four flute at .050 and 2.0 chip load and see how the mill does
is that correct?
steve
Click to expand...

That seems like the right course to me. If you have air available, you may consider setting up an air blast to clear chips, it helps a lot (cooling, and improved finish). Early on I also followed the mill around with a chip brush flicking chips out of the way.
 
Steve

Not wanting to repeat what has allready been said, but Tony did mention those corncobb roughing endmills. I love those , they remove metal in a hurry.
If you havnt tryed one, try it, you might like it! I use them when ever possible.

 
I can code a finish pass i wasnt trying to make a real part just testing the mill for load and accuracy
i did this in a nfs wizzard and it stunk it was going to leave out the side at full depth and i caught it. I can do better than that i was trying something quick and I didnt proof it out before running duhhhh
I'm trying to learn how to mill steel without destroying cutters or anything for that matter.
so far this new mill has impressed me
steve
 
You must log in or register to reply here.
Back
Top