[MFchief]

Hi All,

I'm hoping for some advice on getting a better finish on a part I'm working on. It's a 2.6" diameter hemispherical cavity in 6061 Al. As you can see from the photo the surface finish leaves something to be desired!

I used Meshcam to generate the code, the finish pass is with a 3/4" HHS ball endmill cutting waterline only, mostly 0.01 to 0.02 inches per pass. Meshcam uses "adaptive step down", depending on angle. The step over is 0.02". Spindle was at 5100 rpm, and feed was 15.00 ipm.

Am I completely off base here? Tooling or F & S or something else? I chose the largest ball mill I had for rigidity. By the way, I would trade complete accuracy of the hemisphere for a better surface.

I appreciate any inputs you might have.

Terry

[popspipes]

On a large cutter rigidity can be a problem , also the cutter needs to be super sharp, this would be my guess, I would try a smaller cutter just for grins to see if the finish improves.

[SCzEngrgGroup]

Your biggest problem is WAY too much RPM, and WAY too slow a feedrate. For such a light cut, you really should be running closer to 2000 RPM, and feeding at about 80 IPM. And that's for a HSS tool. The "ideal" RPM and feed (again, for HSS) would be more like 8K RPM, and close to 300 IPM. At the RPM and feed you're running, you're not so much cutting the metal, as pushing it out of the way, and burnishing it.

I would also reduce the step-over, if you're looking for a really fine finish.

Get yourself a copy of HSMAdvisor to see what your feeds and speeds really should be.

Regards,
Ray L.

[Steve Seebold]

Hi All,

I'm hoping for some advice on getting a better finish on a part I'm working on. It's a 2.6" diameter hemispherical cavity in 6061 Al. As you can see from the photo the surface finish leaves something to be desired!

I used Meshcam to generate the code, the finish pass is with a 3/4" HHS ball endmill cutting waterline only, mostly 0.01 to 0.02 inches per pass. Meshcam uses "adaptive step down", depending on angle. The step over is 0.02". Spindle was at 5100 rpm, and feed was 15.00 ipm.

Am I completely off base here? Tooling or F & S or something else? I chose the largest ball mill I had for rigidity. By the way, I would trade complete accuracy of the hemisphere for a better surface.

I appreciate any inputs you might have.

Terry

How much are you leaving for your finish cut? Your ,020 step over for your finish cut is fine, but as Ray said, your spindle speed is WAY too fast.

Slow gour spindle down to 3,500 RPM and increase your feed to 30 IPM and you'll see a world of difference. And only leave .015 to .020 stock for your finish cut.

It's OK ro ruff machine your part at 5,000 RPM, but I would only tale about a ,1 step over and no more than .150 deep. Yeah, it;s going to take a long time but it's only one part and you'll like the results.

I NEVER use HSS end mills. I ALWAYS use carbide. I know, it's a lot more expensive, but it works SO much better.

[MFchief]

Thanks Guys for your great suggestions
I had a feeling I was feeding too slow, but hadn't considered the rpm to be too high.

I tried the cut again at the F&S's that everyone suggested and it did greatly improve the finish, but I am looking for still better. I ordered a new carbide ball mill today, hopefully the will be the final piece of the puzzle. I'll update when I get that in hand and can try again.

Terry

[wildwhl]

MFchief - I've had some of the same challenges you're experiencing. I sometimes have better luck with a round modular insert tool - but for shapes/pockets such as you're attempting I concur that the F&S were way off. I'm currently running a part (no pictures, will try to snag some tomorrow) with .020 finish cut an .02 stepover, using the 16mm toroidal TTS tool from Tormach (came with my mill) at about 4100 RPM, max feed (110 ipm?). Part is coming out nicely. Plan to try it with one insert removed just for giggles tomorrow.

I've run the same part in the past using .3750" ball end mill, 5140 RPM and 300 ipm on a different machine and it came out beautifully. Takes some experimentation I suppose.

WW

[MFchief]

Thanks for the heads up WW,

Hope do you program that type of cutter in CAM software? Is it treated as a ball nose, or can you define the actual shape?
Terry

[wildwhl]

Terry -

I'm using CamBam and while I can define the profile of the cutter (name it) I don't think it really takes anything into account. I frequently tell the software I'm using a cutter diameter 1/2 the size of actual to get the results I want (have to then leave a roughing clearance to match or shape will be overcut).

The trick is to make sure the cutter isn't rubbing, as has already been suggested. I don't know a simple/actual way to calculate that - I've only had to do some trial and error. You want to make sure your cutting chips the whole time. Stepovers that are really small become more challenging with this. I've had success finishing the surface using a burr as well...

WW

[G59]

I NEVER use HSS end mills. I ALWAYS use carbide. I know, it's a lot more expensive, but it works SO much better.

Please explain how it "works so much better"?

We're talking Aluminum. What improvement does carbide offer in this situation when using a ball end mill over 1/2" in diameter? Such a small cutting edge is actually doing any cutting to the Aluminum on the finish cycle.
My opinion, waste of money.
And please don't even go into the rigidity BS, as aluminum is butter for any HSS tooling. Try it and save yourself lot's of cash. Anything in carbide is 2.5 times the money and the finish is the same as HSS or worse.
Not just my opinion, it's a fact.

[popspipes]

Im with Steve on the carbide cutters, in the smaller sizes for rigidity and a fine finish.

They do get expensive in the larger sizes though!!

[SCzEngrgGroup]

Im with Steve on the carbide cutters, in the smaller sizes for rigidity and a fine finish.

They do get expensive in the larger sizes though!!

Carbide is better for small cutters for no reason other than the added stiffness. But for larger cutters, on low-horsepower machines, there is no advantage to carbide, and it is, on average, much more expensive. HSS will give the same, or better, surface finish, last just as long, and cost 1/2-1/3 as much. These machines have neither the spindle RPM, nor the power, nor the rigidity to take advantage of the benefits of carbide tools in larger sizes (over about 1/4").

Regards,
Ray L.

[FuriousGeorge]

Has anyone found a good quality variable flute endmill made from HSS? I use Lakeshore Carbide endmills which give an excellent finish and allow me to do much more aggressive cuts. While the difference between carbide and HSS is probably very marginal for a tormach, the end mill geometry makes a HUGE difference.

[jid2]

Your welcomes.
SUPER HSS, STD LENGTH