Switching to carbide?

[warpedmephisto]

Hi All,

For the past year that I've had my Taig mini-mill I have been running HSS end mills, both uncoated and TiN coated. I was recommended to do so because they're cheap and it doesn't hurt the wallet too badly when the learning curve suddenly curves down. Now that I've been making chips for a year, I'm confident in my skills and knowledgible enough in my machine that I feel comfortable spending more on tooling to achieve a better cut.

I started with the import cutters and have recently (in the past 3 months or so) been using some US made cutters. Although these cutters are supperior to import cutters, they're still HSS and wear out over use. I mill aluminum most all the time with a slight exception of some stainless and even less frequently, mild steel. 95% of the time its aluminum though.

I've been acheiving finishes that I am completely satisfied with using HSS cutters. Also the speeds and feeds I've been running at I am completely satisfied as well. I recognize that it is still a mini-mill and that I'm not going to get super high removal rates so I can live with what it is capable of.

Recently I had a project where I had to mill 2 pockets roughly 4" x 1" x 0.75" deep in a piece of 7075 aluminum. I used a 3/8" high helix 2 flute HSS end mill to do the job. I practiced a bit on a piece of 6061 to get my feeds and speeds correct (first time really using a 3/8" cutter) and then did the parts. The surface finish on the first 2 parts was great and was exactly what I was looking for. However, I went to machine a 3rd part and I could tell the machine was struggling more with the cut. Removed the cutter and examined it and found no chipped flutes but just a slightly dulled edge. The cutter will still cut fine, but not at the speeds at which it had done the first two parts. So it seems that the cutter just simply wore out - which is expected. Switched to a brand new cutter of the same type - problem went away.

I know with carbide it is recommended to run it twice as fast as HSS cutters to achieve a better finish, but my machine could not possibly handle that fast of a cut. So my question is - Strictly from a tool life standpoint, would it be adventageous for me to switch solid carbide cutters, either coated or uncoated? And to a lesser extent, would I notice any difference in cutting or surface finish from switching to carbide? If I can spend twice as much on a cutter but get 3 times the life out of it, thats great. But I haven't worked with carbide cutters much before and don't know how much longer the life is vs. HSS cutters with the same type of cut. Any and all comments are appreciated!

-Andy

[widgitmaster]

Why not use cobolt, its a step above HSS and cheaper than carbide!
Eric

[lakeside]

what type of coolant are you using sray mist, flood or air This can have more to do with cutter wear and maybe a slower rpm to increase chip load

[warpedmephisto]

Flood coolant. I could try to drop RPM's and increase cut per tooth. I'll run some formulas and get numbers tomorrow.

[lakeside]

if you go high performance tooling for alum. try niagata 3 flute se carbide for steel spi z-carb. 4 flute

[warpedmephisto]

I have used Niagara cutters in the past and have had great success with them so I will definitely look into those cutters.

Just crunched some numbers and looks like my chip load was way low. 4300 RPM 0.375" 2 flute at 10 IPM = 0.0012" per tooth. So the dulling was caused by excessive rubbing I'm guessing.

By the book if I drop the RPM to 2900 while at 284 SFM with 0.005" chip load I have to run at 29 IPM which is probably unreasonable for my machine. For end milling and side milling my chip load should be around 0.004" and up, correct?

In the part I have to do a slot to clear the center for the small width of the pocket. So its a full width cut followed by an easy pocket routine. For the pocket where cut width is 50% of the cutter diameter or less I may be able to get my feed rates up which will help cutter life, but for the slot there's not much I can do. I could use a smaller end mill where faster feeds are possible and just keep "stepping" out the slot I suppose.

I will play around with different RPM's and feeds tomorrow and see what I find.

[dkochan]

Hey, Warped:

I know you said you're flood cooling but how big a flood are you running? Are you flushing the chips out of the pocket? Recutting chips will dull your cutters in a hurry, too, and your surface finish will be less than spectacular.

As far as chip load, the "and up" applies to massive machines. I wouldn't try that on my Taig. I don't think you're way low for a Taig. You're just never going to cut big chips (and get maximum metal removal life from a cutter) on a mill that weighs less than a couple of tons.

Dave

[warpedmephisto]

Flood coolant was heavy on to make sure it was extracting chips properly. I can usualy hear it when its recutting chips and I made sure not to let that happen. Surface finish was immaculate and was exactly what I was looking for. Maybe I'll aim around the 0.002-0.003" chip load area and see what that gets me.

[dkochan]

0.003! I can't see feeding 25.8 ipm into *anything* on my Taig. :^) That's at your original 4300 rpm - you'd be at 17.4ipm at 2900.

Also look at horsepower for metal removal - that's going to help you dial in on the Taig. For aluminum, you need about 0.33 hp per cubic inch per minute.

How deep and how wide are you cutting per pass? If you were cutting 0.125 deep and 0.375 wide, (have to start the pocket somehow) at 17.4 ipm, that's 0.272 in3/min or about 0.27 horsepower... Not likely to be happy with that. Just another data point that might help you figure out what's suitable for the Taig.

Dave

[warpedmephisto]

For doing the pocket routine where the cut load is only 50% or less of the cutter diameter I am still only taking 0.05" deep cuts - so I might be able to push it faster there. For the slot I'm running at 0.05" deep as well, but with a full width cut. I can't feasibly see running any faster for the slot, but perhaps for the pocket routine where cutting forces are lesser.

I'm still running the stock motor so my horsepower is lagging a bit. Boy, a varispeed DC motor would come in handy right about now. But I also have to consider the mechanical limits of the machine itself and how much it will flex under a heavy cut like that. Even if I did have a motor to power through a cut like that, I think there would be a lot of deflection not from the cutter, but from the flex in the machine itself.

Also, how are you calculating horsepower requirements for removal rates? Aren't there many more factors to take into account like cutter geometry/design and coolant?

-Andy

[lakeside]

you may want to try 1500 rpms 6 imp .1 depth of cut

[dkochan]

There are tables out there that give you a good estimate of the power constant (the 0.33 value above) needed to shift a given amount of metal. Machinery's Handbook is an excellent source. (For that and about a million other things.)

Tools like the one Lakeside used let you fine-tune even further. Very cool.

Dave