Need accurate location of a hole at a 30 degree angle

I need to drill a 1 mm diameter hole into a piece of steel at 30 degrees off vertical. The location has to be within a few tenths. I've got a Bridgeport and a prayer. I'm thinking deflection is going to be a killer even if I spot it well. Any thoughts?

(I'm simplifying. I actually need to drill several of them and need the relationship between them to be within a few tenths.)

Is there a fixed relationship to another feature that establishes the first of the holes, or is it just each hole must be within a few tenths of one another? And are the tolerances cumulative or from an origin?

If it *really* matters, I'd look for someone to EDM this for me. If it's not quite so dire, then set up a tenths drop indicator along the axis you're cutting, and make sure to do the exact same process each time (for instance, spot with 1/32 EM to remove most of the center stock, spot with 1mm EM to get size and location, drill 1mm).

Can you mill little flats first and then do the drilling? If the flats are a problem maybe the surface can be milled after drilling.

Both those ideas sound pretty good. I'm going to put a locating hole or pin in the side of the part so I have something to indicate off of when the part is sitting at an angle in the vise. There are two holes close together, and it's the land between them that's critical. If I plan right, I may be able to grind the surface until the land width is acceptable, rather than having to have each hole dead perfect. Thanks!

I would start with a 1mm end mill

Conrad Hoffman said:

Both those ideas sound pretty good. I'm going to put a locating hole or pin in the side of the part so I have something to indicate off of when the part is sitting at an angle in the vise. There are two holes close together, and it's the land between them that's critical. If I plan right, I may be able to grind the surface until the land width is acceptable, rather than having to have each hole dead perfect. Thanks!

Click to expand...

Locating pin? This is a job for a tooling ball. The hole for the tooling ball can be drilled normal to the surface, and the call center picked up from any angle.

Dennis Storzek

Any way to fixture the part in a dividing head? For example, mill it on the end of a bar and then drill the hole? If you have a CAD system that you're good with, you can lay out the part relative to some arbitrary centerline and still get things in the correct place by working from there.

If the land (spacing?) between two holes is the critical dimension, I'd make up a custom drill bushing. Use a center cut mill to give it a flat place to rest, get the tandem drill bushing located -- and count on the bushing itself to hold those few tenths in spacing.

Even easier if by "tenths" you mean tenths of that 1mm drill diameter

1. Tenths and Bridgeport....eh

2. How the heck are you gaging or checking this??? EDM drilling is the only way I know?

I'm thinking hardened drill guide in a fixture.

metalmagpie said:

I'm thinking hardened drill guide in a fixture.

Click to expand...

+1 First choice usually. ONLY choice sometimes.

Doesn't even need to strain an ignorant drillpress.

Hi Conrad:
A couple of thoughts for you to consider:
First are they through holes and if not can they be made into through holes?
The reason I ask is that they can be wire EDM cut if they are, and that is the fastest easiest way I know to achieve both excellent hole geometry and excellent hole position in the size you have to make, and your critical feature sounds like it will require both.

Failing that, is there a way to make each hole in a separate piece and then put the pieces together?
If so you can drill the holes ream the holes lap the holes and then surface grind the blocks to bring the holes into position relative to one another before assembly.

Third question: does the design REQUIRE that the holes be round?
If not you could grind grooves into each side of a set of blocks, sandwich a spacer plate between them and assemble the works; provided of course, that your design allows this.

Failing that, can you make the holes first in a big lump and then cut the part shape from that lump after the holes are in?
That will make it a bit easier to produce the holes and will allow you to chuck away failures before too much is invested.

Failing that, I'd sinker EDM them as Milland suggests if they're not too deep.

Failing that I'd make the drill bushing jig but I'd make it out of two pieces so I can position the holes with the surface grinder as above.
Making the jig and the drill bushing (unless you can buy one) is going to be a right royal pain in the ass, and if you need to ream these holes you really need two bushings, and they must be dead nuts accurate.

This is a much more involved project than most appreciate...you have my sympathy!!

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

I'm in the usual situation I find myself in- the production part can be EDM or use a lot of fixturing but... this is a prototype piece to test the overall concept, and is needed in a couple days. Little time, no budget. Great ideas above, and I'll try simple first, then more complex if needed. Inspection is with a video microscope (OGP Smartscope) and should be OK, as it's only the face where the holes exit that I care about. BTW, they are through holes in a 1/4" plate. Also, no conversation concerning dimensions is worth anything without mixed units. 1 mm holes, but a tenth is 0.0001".

Hi again Conrad:
Can you flip the block so the exit side becomes the entry side?
If so, you can control the features you care about much better since they appear to be most critical on the exit side.

Do you have 1 mm endmills and ball cutters?
If you do, you can poke in your flats as Bill Zweig suggests, then poke in your ball cutter to get the hole spotted, then drill a twitch undersized then clock in your 1 mm endmill than gently gently pop it in and see what kind of hole you get.

If you have access to a cutter grinder you can also make a 3 flute boring tool and pop it in with that.(like a stubby reamer but with no corner chamfers)
Make it a bit undersized and you can try it out to see your location before you commit to final size.

The proper way forward if you care most about the relationship of the two holes is to finish one first, and that then becomes your datum hole.
Now you can screw around with tenths clocks on the axes to diddle the second hole into position.

Being able to interrogate without dismounting or moving things helps you.
A copper banger smacked gently onto the saddle or the X axis slide to tweak the last tenths out of an axis movement helps you too.
Nipping the quill clamp until you can just float the quill without slop is useful too.
So is never touching the knee elevation handle...in fact TAKE IT OFF!

Being able to bore a smooth round hole that's undersized helps you too.
Gauge pins in tenths increments are your friends.

So what kit do you actually have to do all these things with?
Can you grind a cutter?
Can you grind a 0.9mm mm 3 flute carbide cutter accurately?
What about a 0.9mm HSS cutter?

What resources you have will determine what you can do (of course)!
So show us your shop in all it's glorious detail...even if we can't actually help you, we're always curious (at least I am!)

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

You are planning on drilling a .040 hole with location within tenths?

Can you check it on the machine? Do you have more than one part and how expensive is it to scrap it? If not too expensive, make one, check it then move your spindle whatever and make another one.

If it's expensive, and inspection is not ton the machine, then you need a way to set it back up accurately enough(which I know is what you are asking, but a big difference in the fixture for option 1 and option 2)

Drill undersize and bore it would be optimal. Then you can pull, it check it, then move your hole. The drill bushing fixture gives you a decent shot. But, there may be development and refinment to get it produce the part correctly, which means setup pieces. Tenths are doable but they always take work. Or maybe a small series of endmills to pluge with?

Can you mill the feature it is relationship to after you put the hole in? That might be the easiest to machine and measure.

Resources are limited, and I can't measure without removing it from the machine. No cutter grinder either. No biggie if I have to make a couple to get it close. There are people who would bore it, but I'm not that good with a manual Bridgeport. The part is simplicity itself, a small block of mild steel with a couple holes. I'll take the first shot tomorrow and report back.

As usual, my dreams are larger than my capabilities. I did all the features on the part, save for the angled holes. I redesigned it a bit with some perpendicular holes as a comparison. I can usually put any features about where I want, but it's amazing how quickly errors add up on multiple features. Even with the tenth DRO, I question the BPs ability to get anything much better than a half thou. It's also amazing how much holes and such upset a flat surface. I had ground my blank near dead on size, figuring that was one less thing to think about. A quick polish after putting in a bunch of holes showed raised material around each one. Not unexpected but even some 1 mm holes showed an upset twice their diameter away. Not talking Mt. Everest, but I'll definitely be lapping or regrinding that surface when everything is done. Might get to the angled holes early in the week.

Meadville, Pa is within 2 hours driving.

Plenty of shops that could do this for you.

Nothing up in Rochester ?

So what is this thing, and why does it need these features?