Issues milling 440c stainless

A. Richey Knives · Jun 4, 2017

So after two attempts at dry milling 440c stainless with a .25 AlTin endmill, I've decided to reach out for some guidance regarding speeds and feeds. I'm trying to profile the part with .04" doc / .25" woc using the speeds and feeds suggested by Lakeshore, and broke two brand new end mills. Any assistance would be greatly appreciated.

DMF_TomB · Jun 4, 2017

A. Richey Knives said:
So after two attempts at dry milling 440c stainless with a .25 AlTin endmill, I've decided to reach out for some guidance regarding speeds and feeds. I'm trying to profile the part with .04" doc / .25" woc using the speeds and feeds suggested by Lakeshore, and broke two brand new end mills. Any assistance would be greatly appreciated.

.
recommendations are MAX recommendations. try 50% rpm and 40% feed and see what happens
.
if corners breaking off reduce depth of cut

A. Richey Knives · Jun 4, 2017

Thank you for the speedy reply! I'll give it a shot and see how it goes.

Milland · Jun 4, 2017

A. Richey Knives said:
So after two attempts at dry milling 440c stainless with a .25 AlTin endmill, I've decided to reach out for some guidance regarding speeds and feeds. I'm trying to profile the part with .04" doc / .25" woc using the speeds and feeds suggested by Lakeshore, and broke two brand new end mills. Any assistance would be greatly appreciated.

Are you sure you didn't get the numbers backwards? .040" would be a reasonable width of cut (X-Y) for a .250" tool, and you should cut as deep as possible with the tool (Z) to get the best use of its cutting edges. If you really were doing .250" in X-Y and only .040" in Z you used the tool wrong.

Also, use the shortest flute length possible for the material thickness you're cutting, and makes sure that the chips are flushed away from the area by your air blast. If you don't get the chips out of the cut zone they'll damage the tool edges quickly.

Milland · Jun 4, 2017

More questions - are you profiling a blade from solid sheet stock? That would explain the full width of cut, but that's hard on an endmill in tough materials. And are you plunging in with the tool, ramping in, starting from the plate edge, or starting in a drilled hole? Endmills don't like plunging in hard materials, not a problem in softer stuff.

A. Richey Knives · Jun 4, 2017

Milland said:
Are you sure you didn't get the numbers backwards? .040" would be a reasonable width of cut (X-Y) for a .250" tool, and you should cut as deep as possible with the tool (Z) to get the best use of its cutting edges. If you really were doing .250" in X-Y and only .040" in Z you used the tool wrong.

Also, use the shortest flute length possible for the material thickness you're cutting, and makes sure that the chips are flushed away from the area by your air blast. If you don't get the chips out of the cut zone they'll damage the tool edges quickly.

I'm cutting a knife blank out of .187" stainless so I'm trying to profile the shape using tabs to suspend the blade in the steel.

A. Richey Knives · Jun 4, 2017

Milland said:
More questions - are you profiling a blade from solid sheet stock? That would explain the full width of cut, but that's hard on an endmill in tough materials. And are you plunging in with the tool, ramping in, starting from the plate edge, or starting in a drilled hole? Endmills don't like plunging in hard materials, not a problem in softer stuff.

Yes sir. It's a solid sheet. I probably should've mentioned that. I did plunge into the material which was my first mistake in the CAM programming. I just adjusted it to a ramp in, but my concern is the speeds and feeds because it obviously got way too hot. This sucker was glowing so I backed it off to 50% of the recommended speed and all was good for until it snapped. I just didn't know if there is something specific I'm not understanding with 440c or I just totally flubbed the speed/feed using the manufacturers and G wizards figures. .

Milland · Jun 4, 2017

A. Richey Knives said:
Yes sir. It's a solid sheet. I probably should've mentioned that.

Yeah, that makes more sense. There's a process that'll likely take a little longer, but will allow you to reliably cut your parts from sheet in one depth pass. Search the topic "trochoidal milling" and see if you can output code with whatever CAM you're using to suit. Try using a stub 3/16" tool at full depth and a 1/4" slot width, be sure to drill any entry holes you need at the start of each pass.

It may take a couple iterations of the geometry to come up with something reliable, but once you have it right you'll get good life from the tool and decent material removal. Remember what I said about being sure you can clear chips away, if you don't have enough airflow you're going to kill the tool.

DavidScott · Jun 4, 2017

My experience with annealed 440c is it is not difficult to machine. What exact end mill are you using? This may be a good application for a corn cob rougher, if you are doing enough parts. If using a normal end mill 3 flute stub with a corner radius. I would be using as much coolant as I could get to the tool, with an appropriate coating for this. For slotting you do want to run the speeds on the low side but keep the chip load higher, as long as you can keep the cut stable.

Milland · Jun 4, 2017

DavidScott said:
My experience with annealed 440c is it is not difficult to machine. What exact end mill are you using? This may be a good application for a corn cob rougher, if you are doing enough parts. If using a normal end mill 3 flute stub with a corner radius. I would be using as much coolant as I could get to the tool, with an appropriate coating for this. For slotting you do want to run the speeds on the low side but keep the chip load higher, as long as you can keep the cut stable.

A three flute tool's not a bad choice if you've got the coating on it for high spindle speeds. As he's going through the stock he shouldn't need a corner radius, or if there's one present he'll have to go past it into a spoil plate or air.

And he's trying to cut dry, not sure what if any air blast he's got.

A. Richey Knives · Jun 4, 2017

DavidScott said:
My experience with annealed 440c is it is not difficult to machine. What exact end mill are you using? This may be a good application for a corn cob rougher, if you are doing enough parts. If using a normal end mill 3 flute stub with a corner radius. I would be using as much coolant as I could get to the tool, with an appropriate coating for this. For slotting you do want to run the speeds on the low side but keep the chip load higher, as long as you can keep the cut stable.

It's the 4 fl Lakeshore Carbide AlTin end mill. I adjusted the speed/feed like DMF_TomB suggested, adjusted to a ramp-in and I'm all good! Getting a consistent golden colored chip and no breaky breaky! Thanks a million fellas!

Search

Largest Manufacturing Technology Community on the Web

Search

Issues milling 440c stainless

A. Richey Knives

Plastic

DMF_TomB

Diamond

A. Richey Knives

Plastic

Milland

Diamond

Milland

Diamond

A. Richey Knives

Plastic

A. Richey Knives

Plastic

Milland

Diamond

DavidScott

Diamond

Milland

Diamond

A. Richey Knives

Plastic

Similar threads