[asssets]

Hi everyone,
After sometime of trials and errors would like to ask your opinion and help to get this right.
I'm using 61991 Niagara cutter (representative recommendation for my material) on there web site I found data sheet for 304 steel, but cannot understand how to use it.

I have 0.022 inch steel plate where i do cut out.
My settings are:
Spindle speed: 1800 rpm
Feed: 10 inch/m
Depth per pass 0.0055 inch
Tool: 5 flute 1/4 diameter
For me it looks like feed is slow for this RPM, but I do not now what to adjust first.

[hawkburger]

What is so bad about that? Slower RPM will stop the overheating in thin stock. Rigid as possible? It's bot horrible looking. Could have been worse.

[MetalZilla]

Why is the depth of cut so small? Should cut easily at full depth.

[isaac338]

FSWizard

Looks to me like your DOC is way too low as well as your feed.

I should point out that I just had an interesting time slotting 304 and the speed and feed numbers that FSwizard gave me were pretty workable once I adjusted the feed and SFM sliders down to about 70%. I was using HSS and cutting a slot thru a .250" plate, though.

[zero_divide]

How do you hold the part?
You have 2 problems.

1. The endmill is too big for the thickness of the material you are cutting. Unless you glue that sheet down to something vibrations and heat will kill such a big cutter. I would not try to mill something like that with anything larger than 3/16.dia
2. It is best to use 4 or 3 flute cutters on stainless steel.


So assuming you use a 1/4 4 flute carbide end mill you should get:
3000rpm , 18 to 25 ipm full depth.
You need to find a way to keep that sheet from flapping though.
I think you are addressing it by doing a very shallow depth of cut, but it hardens the material and ruins your cutter.

This is why i think you should use a much smaller endmill than what you have now. Even a 1/8 3 flute tialn coated endmill will do a better job job

Cheers.

[Sho409s]

304. You can't let it heat up and running too low of feed will heat. I cut the speed and use lots of cooling until it works, but usually try to keep the s/f ratio similar or less feed. We don't do a lot of it but compared to 409 I often start at roughly 75% speed and 60% feed if nobody knows what to use. I had to cut out plugs .015-.020" 304 and used a .500 hypercarb type 3 or 4 flute EM seemed to work best. Ran it 2500 and F25 but still were not lasting that long, but the .375 thick plug would sometimes hit the EM hard enough to bend the flap on it. It was better than prying plugs out by hand. Maybe I should have run it slower but was thinking more speed would help it better take impact as the plug was cut loose. I managed about 200+ inches per used EM doing that and finished the parts. Normally run a .500 EM double that speed, and never used one for cutting out plugs before. As usual the parts were due lol.

[asssets]

Thank you for replies a lot of good information. But I'm new to routing and do not understand some calculations.
I will order 3 flute and 1/8 from Niagara (61802) and will play with it.

Hold material is the biggest problem. I have wooden board and screw part to it. Small steps hold material flat. But idea with smaller bit looks is the way to go.

[Starrett2012]

What type of machine are you using? Pictures please.

Alot of getting your setup right is trial and error. The formulas are a starting point to get you going and adjust if necessary.

What problems are you having with the "Cut"?

You should be able to sink that end mill all the way through the material and cut at full depth especially on .022" thickness of work material.

If I was cutting stainless I would start at 50 sfpm. (The link that you gave for the material shows 50-160 SFPM.) This would give me 200/.25=800 RPM for a 1/4" HSS Cutter. (50 SFPM X 4) / Cutter Diameter. I can't tell what material your end mill is, looks like Carbide? X2 for Carbide. So I have 1600 RPM starting point for a carbide cutter.

Depth of cut per tooth is .001 to .0018. Start at .001 and go up from there if you think the cutter and machine(rigidity) can handle it. Next formula is # of teeth X Cut per tooth X RPM. so 1600 X .001 X 5= 8 inches per minute. You have your starting number, give it a try.

This will be 4 times faster than taking 4 .0055 passes.

If this works well the first thing to do if your machine can handle it is more feed. plug another value into the feed formula like .0018 for doc per tooth and try it.

Are you using a cutting lube/coolant?

Your number one resource is the salesman that sold you the tool. I would like to know what he recommends for feed and speeds,or the manufacturer should either give tech advise over the phone or on their website.

Let us know how you are making out.