Setup and tooling advice for newby

I have a Tormach 440 (3/4 HP, 10,000 rpm spindle, 4" vise) and need a recommendation for an endmill to mill a hole in .125" 6061 plates.
2,3,4 flute? Carbide? flat or ball nose, Brands? I need a 1/16", 1/8" and 1/4" diameters.

Additionally, some advice on a fixture for the plates would be helpful. The plates arrive to me 3.0" x 3.0" with a milled hole (fixed size) in each corner and then my operation would be milling a single hole in the center. My initial idea is to simply mill a blank into a pair of soft jaws, or should i use top pressure so that the plate does not deflect?

Thank you!

If you are only doing the center hole and the corner holes are already done I would strongly recommend making a fixture that can sit in a vise with 4 tapped holes in it and bolt the plate to it. If location is more critical then use shoulder bolts instead of regular bolts and create counterbores in the fixture. Or do 2 bolts and 2 dowel pins. That looks like it would be alright to hold in a vise but plates are easier if they are bolted down so they don't bend under pressure.

NYC CNC on YouTube is a great starting place for fixture ideas for a beginner, he has lots of great videos as well as feeds and speeds on his website for your exact machine.

LakeShore Carbide makes good easy to purchase tooling for this type of stuff. There are tons of other brands out there selling quality endmills but I recommend them to beginners because you can buy direct and their website is very easy to understand. For aluminum you want a 2 or 3 flute endmills (uncoated or ZRN coating).
Either helix into the hole or predrill, do not plunge the endmill. If all your holes are always the same size, consider drilling and reaming to final size.

I think if I had to do a lot I would make a fixture to accommodate a few stacked with dowel pins to locate the corner holes. Then use something like destaco clamps or toe clamps to hold them down.

Too make the hole something like an anular cutter may be a good bet but then you have to remove the slugs.

Going at it with a decent 3 flute endmill should make quick work aswell. Just drop down the predrilled holes and spiral out.

Yg1 Alu power is what you want for aluminum cutting on a budget. The 3/8 and 1/2 are a very good value. These are exceptional end mills and they are dirt cheap.

You might state the incoming hole size and location specs, and the size and location needs of the hole you are making.
Perhaps a bushing plate may be due if a high number job.
Perhaps a center punch plate.
*How the part print defines the hole location is important.

What was said above, but if you have a lot of them to do consider holding them down with toggle clamps:

Vertical Toggle Clamps | Toggle Clamps | Clamptek Enterprise Co., Ltd

mhajicek said:

What was said above, but if you have a lot of them to do consider holding them down with toggle clamps:

Vertical Toggle Clamps | Toggle Clamps | Clamptek Enterprise Co., Ltd

Click to expand...

Don't make a mistakeo get destaco

Do you need to deburr/break the edge on the hole you're doing? Stacking them and bolting thru the existing holes would be fast. If you need to drill the hole and break both sides of it, I'd probably bolt thru the four holes as singles, on a pallet, or vacuum hold a bunch of them on a vacuum chuck.

I don't know if a tormach will make it through that many at once.

Is it a 1/8 inch hole needed or 3/8”? If 1/8 I would use the edge of fixed jaw as reference- set mill to center of first plate, drill, done. Rinse and repeat but your zero doesn’t need setting again.

Looking at the picture better it looked like a .380 hole if you gang them you could probably just drill with a stub drill and be fine.

For some reason I thought you needed a 1.25” hole

You can certainly get away with milling steps in soft jaws and holding it in a vise. However, you will need to be pretty consistent with vise pressure, and knowing when you're over tightening or under tightening. When holding onto a plate, depending on thickness and width (in this case 1/8" thick, 3 inches wide which is not too bad), it tends to bow up and away from the vise and it acts like a spring or drum skin. The cutter will put additional upward force on the material, plus vibrations, and will probably harmonize. One way of eliminating this is cutting a dovetail relief at the bottom of the jaws so that it is only contacting and squeezing the part at the top.
That being said, the best, most reliable, most fool-proof way to hold sheet stock is in a fixture with toe clamps or toggle clamps giving top pressure, and there is a lot of good advice already given for that way. For locating, you can machine "bump stops" in a plate to push the material against in the y and x directions (be sure to relieve the corner), or drill and ream 3 pins for locating, 2 pins on the back side and one pin on the left side is usually my setup.
As for endmills, it's hard to make a recommendation without knowing your machine better. I believe the Tormachs have a fog buster, and not flood coolant, which makes me want to steer you away from carbide, which tends to chip when it overheats. But I've seen plenty of people using carbide in that system without problem. Supermill makes a great endmill, as does destiny tool. Harvey tool also is really high quality and tend to last longer in my experience. I would suggest using 2 flutes, as it is more forgiving, and there is more room for the chip to evacuate. You're not going to be able to keep up with an extra flute in my opinion and the amount of time you will save is negligible. And if you are interpolating, consider the following formula: ipm x (hole diameter - tool diameter)/hole diameter = programmed ipm. So for a 2 flute 1/16" endmill you'd be going 10000rpm x .0015 cpt x 2 flutes = 30ipm when cutting. But to interpolate a 1/8" hole, you'd program it to go 15 ipm to maintain that .0015 cpt. Good luck

Make a fixture to stack a bunch together with pins for locating, bolt them together and blast a fucking drill thru a bunch at a time.
Some of you people are turning this part into something it's not.

Mtndew said:

Make a fixture to stack a bunch together with pins for locating, bolt them together and blast a fucking drill thru a bunch at a time.
Some of you people are turning this part into something it's not.

Click to expand...

Blast? 3/4 HP.

Because he is new and trying to learn, I like exposing him to many ideas for workholding.

One thing I never do with stuff like that is stick it in a vise But I'm a bit of a pansy. "Risk Adverse" I like to say.

I am going to assume the corner holes are a nonstandard size; I would take an aluminum drop I have on the shelf, stick it in the vise and face it, then mill two bosses in opposite corners about half the thickness of the plate that will fit into two opposing corner holes. Then drill and tap for toggle clamps and probably machine a clearance hole through the center for chips to fall through. Then I'd get at them.

This supposes the plates are held to close enough tolerances to slip onto the bosses.

if the person who did the 4 holes had numbered the 4 sides and put side #1 to his vise solid jaw..and then you put side #4 against your vise solid jaw likely the center hole would not be on location/center.

You have to know how the customer wants the hole you make to relate to the part, or to other features of the part.

If you place your hole wrong likely you will take the blame for the scrap.

I would not run the job if there was a doubt. Better to refuse the job, rather than get blamed for scrapping it.

You may have to measure the square, the 4 holes location to the square, the 4 holes center distance and the 4 hole relation to the sides and to each other.

You might inspect the parts with a caliper and so determine if you can locate them the same way as the guy who made the 4 holes...and inspect them so you know your work will not put the part in jepority.

Suppose you charge $2 per hole..and with scrapping the part the customer blames you $5 for each part. Plus you lose a customer, and all the potential customers he tells about your scrapping his job.

Depending on how many you need to do will dictate how your fixturing should be designed. Im thinking a plate with dowels for two opposing holes and two threaded holes for 3/8 threaded holes and a bolt to hold the plates down. Make the dowels at least 3/4 tall to stack 6 at a time.
Then helix a 1/4 3 flute end mill down leave enough for a finishing pass and you will have a nice hole. What cam are you using?

For tooling look at Mari Tool. He has VERY nice end mills and even better holders for a lot of things. A cheaper and often faster end mill is like others have said is a YG-1 from amazon or the like. They are carbide with a high polish and cut very well.

CITIZEN F16 said:

Blast? 3/4 HP.

Click to expand...

It's aluminum, he shouldn't have much of an issue drilling a small hole. Sure he can't blast thru it. Jesus quit being so literal.

An end mill is sharp at the OD so will cut oversize to the amount if run out in your spindle or holding device..so good to run a test part and measure it to the given spec.

Mtndew said:

Make a fixture to stack a bunch together with pins for locating, bolt them together and blast a fucking drill thru a bunch at a time.
Some of you people are turning this part into something it's not.

Click to expand...

I was thinking the same thing but use a drill press with a small jig fixture.

mulcahla said:

I have a Tormach 440 (3/4 HP, 10,000 rpm spindle, 4" vise) and need a recommendation for an endmill to mill a hole in .125" 6061 plates.
2,3,4 flute? Carbide? flat or ball nose, Brands? I need a 1/16", 1/8" and 1/4" diameters.

Additionally, some advice on a fixture for the plates would be helpful. The plates arrive to me 3.0" x 3.0" with a milled hole (fixed size) in each corner and then my operation would be milling a single hole in the center. My initial idea is to simply mill a blank into a pair of soft jaws, or should i use top pressure so that the plate does not deflect?

Thank you!

View attachment 338008

Click to expand...

For an admitted newbie all caution should be in place
What are the tolerances?
How are you going to hold it so it might repeat in tolerance?
What will you touch off from?

Even +- 1/64 is a close figure if you don't relate correctly to the already done features.
To scrap your first job is not good.