[Rich05]

Do I have to use a lower gear? What depth cuts and feeds and spindle speeds are safe? 1/2 endmill carbide 4 flute? using coolant also.

[Runner4404spd]

depending on what steel you want to cut, my chart says somewhere between 100 and 600 sfm. this translates into 765 rpm to 4580 rpm. depth of cut at .1 should be ok. you may be able to increase this if your cutting less than full width on the end mill. feed should be around 55 ipm at the peak RPM. you should be shooting between .001-.003 chip load per tooth.

IPM = chip load * RPM * # of flutes

[Rich05]

man thats flying.

[Runner4404spd]

thats based on optimal conditions. the IH mill may not be rigid enough to take advantage of the full capabilities of the carbide end mill. i would start at the low end and work my way up. if you start getting chatter or break an endmill back it down some and make note of it for future use.

[Cruiser]

And don't forget to adjust for the weekest link in the setup. Most often it is in the workholding methods involved. I have witnessed some rather large parts go flying in a very destructive mannor even tho the math was correct.

[Rich05]

thanks for the advise,

I am running 750 rpm with 5 ipm feed rate, depth cut of .05" with flood coolant on mild steel, with .5 flute endmill.

Still getting a bit of chatter. Tried Conventional milling, read somewhere that would be better, seemed to chatter more.

I tried also the software ME Consultant Professioinal not bad, it recomended 521 RPM, with 1.838 Ipm feed, (68 SFP).

Update - actually both of the above tend to chatter too much I turned RPM up to 3240 and now running at 3.68 IPM, seems better even though the chips are grey/blue on backside. The higher rpms seem only way to dampen the chattering.

part is tight in a kurt vise. the part is a 8" long 1"x1", the milling goal is to make a .625" slot running .625" deep down the center, basically to turn the steel bar into a custom piece of channel.




any other steel tips appreciated pls.

R

[cjdavis618]

I may be able to help a bit here. I needed to mill out several pieces from A36 plate that was 1" thick recently.

I was cutting at about 20ipm, with coolant at .025 with a 4 flute carbide in 1/4". I was also running 1800rpm. Obviously, this was a bit tedious since I was using a longer bit than usual. One difference was the mill as I was using an SX3 that I cnc'ed. Your's is undoubtedly more rigid than mine.

My cut path was a simple bracket with a 1.25 through hole and then an outside cut pattern. There were multiple brackets (arrayed) in the same cutting op so what I did for entry points was to drill a 1/2" hole though the starting points so it could ramp sideways into the plate. This eliminated the jumping that occurred with plunging into the steel.

On the first few "test" plates I did, I experimented with ramps, arcs, helix's etc. They would all cut fine, but not the mill out acceptable tram. So I that was my only conclusion.

I even ran a couple of plates at 30 ipm and started to dull the bits, so 20 was my sweet spot. (At least for that plate of steel, others may be different. )

[Rich05]

interesting sounds like my depth cut is a bit aggressive. I will try .025 depth cut from now on. My endmill probably is nice and dull now... was brand new.

also using the a whole tool diameter .5" cut the slot seems to really change the numbers in ME consultant, program says 1.1 ipm.. I will try the .025 depth cut and mess around with that maybe ramping too? Since the whole tool is getting used in the slot?

Bottom of this post is an AVI movie of cutting the slot, and attached is screen shot of ME consultant. I used 80% on spindle efficiency have no idea what that means.



MOVIE (right click save dir then play - not embedded in post - quicktime playere seems to run it best)
http://www.terrablades.com/001.AVI]

[cjdavis618]

Yeah, using HSS will be a bit different. I got 13 ipm with HSS vs 20 for Carbide.

Here is my toolbox calc,

[Rich05]

Did not know could use a high helix blade for this? That would be nice!



just noticed did not have 4blade endmill selected above still that would only get it to 2.8 ipm

[skullworks]

1st off, the most effective method to remove cubic inches of metal is a drill.

Drill yourself a line of holes near the full depth you need.

Next I would use a TiN coated HSCo "corn cob" roughing endmill and go plowing thru whats left. Roughing endmills can cut at a depth equal to there diameter with ease. Slow it down.. about 75 SFPM and let it take good bites .003" IPT it will purr right thru and leave a nice gravel like pile of chips. - This assumes flood coolant, without flood, reduce the depth, use plenty of cutting oil and pulsed air blasts. Chips piled around a cutter running without flood in a slot hold the heat in and burn up the cutters.

[Rich05]

I have more information on the steel I am trying to mill 1018 that has been hotrolled and pressed in a die to form the shape, the supplier claims it has been made harder by the process no other info.

[skullworks]

1018 formed hot or cold is still a low carbon steel and should not exhibit any workhardening. However if they are case hardening the parts after forming that will leave a hard outer skin which will cause havoc with tool life.

Also Cruiser is right! "And don't forget to adjust for the weekest link in the setup. Most often it is in the workholding methods involved."

[Rich05]

I switched from HSS to Cobalt, huge difference.

[Capteod]

Do I have to use a lower gear? What depth cuts and feeds and spindle speeds are safe? 1/2 endmill carbide 4 flute? using coolant also.

The first question I WOULD NEED TO KNOW IS WHAT TYPE OF STEEL! Machining stainless steel is one thing, while working on 11l17 or 12L12 is another animal.

There is a general formula as to determining RPM it is:

Cutting Speed x 4
------------------------------ = RPM
cutter diameter

For free machining steels like the 12L or 11Lthe cutting speed is up over
400SF/M. When you get into 4XXX steels you can get as low as 50 SF/M.

As to the depth of cut, it is a function of the HORSEPOWER of the Spindle. A good rule of thumb is 1/2 cubic inch of steel per horspower. The next question is how fast can you flush the chips out of the way.