A few hole Qs....

OK,

Boucou Angst over here, time to drill/tap the GR510 table, 1" alum plate, 5 rows of 11 holes, everything spaced 12".

Form tapping 5/16-18 blind holes, about .950 deep, with an L drill (.290), for a 5 flute emuge form tap, flat bottom. I'm going to bottom out the hole with a 9/32 em (.281) before tapping, and thicken up my coolant.

Might I go a little smaller on the drill, for bigger % thread engagement?

I'm assuming also that if I pre-drill the hole (say 1/4"), the hole will be tighter as well.

So the whole deal will be deep spot, 1/4" drill, L drill, 9/32 end mill, roll tap, rich coolant.

Advice? Normally, I'm not so anal about my holes, but I'll be stuck with these holes forever... no puns intended.... LOL Man, I got the DTs over here....

OR, mebbe the following:

deep spot, G drill (.261), THEN 9/32 end mill, then L drill, roll tap...??

Rigid tapping.

Is there a reason you can't make them thru holes?

The form tap has to displace metal from where the root of the threads are and that metal has to have a place to go i.e. to where the crest of the threads are. If there isn't enough room for that metal to go things will go bad fast so I wouldn't deviate from the drill size specified by the form tap manufacturer. It's not like a cutting tap where you just get a bit larger chips.

Yeah, fairly "busy" under the table, wires, serpentines, also beams. Thru wouldn't be a disaster, but just playing it a little safe.

Well, all taps have that 50-75-85% or whatever thing. But your point is well taken, and I'm sure the emuge site has a chart for their taps.

Also, a li'l birdie reminded me about reaming. I don't do windows, and I don't do reaming, but mebbe I should for the sake of the table.

OK, you got me to call Emuge. .285-.287 is what they recommend for their form. I'll do this the "right way" and just get a .285 reamer. I'll proly drill with a .266 (H) drill, bottom with the .281 end mill, ream .285, tap.

Emuge has some quality service, perty tight with Haas.

The main purpose of the counterbore is then it can also serve as a location hole

That's correct, jon, and it's one of the two main reasons that I fabbed the plugs myself, secondary reason being that even the hex recess in a plastic setscrew will collect chips and debris, and so since the holes were already counterbored, I chose not to use a threaded plug, opting for a simple press-fit instead.

Oh I see the plate your drilling IS the table. I thought it was a fixture plate on top of the table.

I would think an endmill to the manufacturer's recommended size would do it. If in doubt, run all the operations on a piece of scrap.

-jim

The main purpose of the counterbore is then it can also serve as a location hole ================================================================

Seems dats a perty shallow hole for location, tho.

That's correct, jon, and it's one of the two main reasons that I fabbed the plugs myself, secondary reason being that even the hex recess in a plastic setscrew will collect chips and debris, and so since the holes were already counterbored, I chose not to use a threaded plug, opting for a simple press-fit instead. =========================================================

The 5/16-18 holes in the table will all be utilized. It's the 600+ 1/4-20 holes in the rails that will be collecting crud. For me, the plastic set screw is proly the best compromise.

Next page has longer 1/4-20 set screws. Yeah, the hex recess can collect crud, but fugit....

Microplastics is a nice company, large inventory.

1/8" is plenty for locating. The screws take care of the load.

We have tombstones with grids of tapped and c/b'ed holes. Wouldn't use this on a vertical for the reasons mentioned by PrecisionmachinisT. Some newer tombstones don't have the whole grid and we put only the holes we need, part of the grid of course.

If you go ahead with it plug the holes not in use with wax.

Drilling undersize for rolltaps spells disaster. Go top limit. Or even better, use a threadmill.

I have never seen a rolltap bigger than 1/4".

DanP

Any reason you don't thread mill? Spiral in with a 0.250 end mill, that will give you a flat bottom, then thread mill.Turn the coolant flow up to flush the hole. I have taken to thread milling most of my multiple hole setups now, from 2-56 on up and have found it the least problematic way.

Doesn't need to be very deep....

--in practice, the other fasteners are first tightened down, then the locating pins are then pulled, and finally, fasteners are put in their place.

Anyways, I'm relieved to hear that you're not drilling a grid pattern across the whole dam table.

To install fasteners...

Less damage should an accident occur, IMO--especially if the pins were in only 1/8 in deep or so.

Don't do it yet. Quote, unquote I'll be stuck with these holes forever...

Helicoil or keensert. Otherwise, how long do you think the Aluminum threads will last?

You can thread-mill 2-56??? I didn't know that was possible!! There are LOTS of reasons I don't thread mill, one of them being I haven't learned how, the other being the knee-buckling price of thread mills, which is mostly why I haven't learned how!!

BUT, it is a thought to keep in mind....

How long( # holes) can a thread mill be expected to last, for the "typical" hole, #10, 1/4, 5/16, 3/8, 1/2?? all coarse thread...

How undersized is undersized? I called Emuge, they list .2874 for the 5/16, but they guy told me .285 would be fine for more thread %. Funny their table doesn't list the various thread % -- thought they'd be real anal about that.... lol

I have them 5/16, 3/8. Should/hopefully be OK in alum. But I get your point.

Oh:

I have a customer that needed 2-56 blind holes in 0.090 alum sheet to mount some electronic parts on. Thread mill was the only way. Thread milling is easy,I use the free Vardex program, make good code. The thread mills I get from maritool,good cutters at a good price. As for the number of holes I got well over a thousand 1/4-20 x 0.385dp in Alum on one cutter.That's the size I cut the most. The way I do it is to use and end mill to cut the pilot,being flat bottom it give me max thread, the call the thread sub, I always put the thread code as a sub,plus the thread code uses G41 so it's easy to adjust the fit.