Tapping a clean thread cross-wise through a cylindrical bar?

[rons]

A 3/8" stainless bar
1/4-20 GH3 coated tap
#7 cobalt drill bit.

When the tap is exiting the underside of the bar there are metal shards sticking out which is understandable.
I tried to wrap a collar around the bar but the finish on the bar gets damaged.
I know I could use a larger diameter bar and turn it down.

How do you get a clean threads on a curved surface.

 

[L Vanice]

The most work would be to mill flats on both sides of the bar, then drill through and countersink both sides. Then tap. Slightly less work is to drill through and then use a piloted counterbore from both sides, just deep enough to achieve a full cylindrical hole. Then tap.

Easy way is to use a fine round or half round file across the tapped hole and countersink if needed.

Larry

 

[TeachMePlease]

Burraway | Deburring Tools by Cogsdill

Cogsdill Burraway Operation - How it works - YouTube

 

[CarbideBob]

Burraway | Deburring Tools by Cogsdill

Cogsdill Burraway Operation - How it works - YouTube

Round bar? Say hole 25-50% of stock diameter?
.375 bar .250 hole. One heck of a back chamfer or counterbore.
Bob

 

[rons]

Round bar? Say hole 25-50% of stock diameter?
.375 bar .250 hole. One heck of a back chamfer or counterbore.
Bob

Yep, it sounds like a bad deal. But I scaled down another mechanism that I have and the dimensions do work
on this particular clamp.

It started with a linear bearing.


Then I built everything from the inside out. A perfect grind for a carbide bit to shape a high-flow fitting.
The square block is for truing the wheel. A diamond point at the far end and a 8mm-0.5mm screw at the near end.
The cardboard and tape are just temporary to layout angle lines.


The bottom profile where the inside thread meets the bar side wall is not shape and clean.

 

[atex57]

Can you thread mill it?

Ed.

 

[EPAIII]

Drill

CS both sides

Tap

Quick cleanup with hand held CS (in a small drill chuck or mounted on a handle if needed/desired)

That should do it.

 

[wesg]

A scallop cut on both sides, using a cutter that's bar diameter, will meet the intersection of the thru hole pretty nicely. A little fiddling with dia and depth should give you something useful. Of course it's 3 cuts total, but easily indexable. As is c'sinking.

 

[rons]

A scallop cut on both sides, using a cutter that's bar diameter, will meet the intersection of the thru hole pretty nicely. A little fiddling with dia and depth should give you something useful. Of course it's 3 cuts total, but easily indexable. As is c'sinking.

What forms on the underside of the bar are two sharp projections. Developed from a partial thread and they look like shark teeth.
The only way to remove them is to break them off. A scallop on both sides is something worth trying.

The pilot hole for a 1/4-20 is a #7 drill.

Would the scallop cutter be better at .250 diameter rather than .375?
Or would .3125 be better?

1/4 or 5/16 or 3/8 cutter. Which one?

 

[yardbird]

Is clean threads on a round surface a requirement? Unless you sink an oversized chamfer in exiting side your going to have to remove a bur afterwards. I'd hit it kinda hard on the one side with a counter sink then run a tap down in it and call it good. If it had to be clean threads on a round bar then drill and tap it then roll it on the belt sander or grinding wheel. Maybe hit it with a file at the lathe. Probably have to run a tap back through it to clean up the threads before you called it done.

Brent

 

[rons]

Can you thread mill it?

Ed.

I don't know how to get the correct feed for a 1/4" - 20 thread.

 

[atex57]

I don't know how to get the correct feed for a 1/4" - 20 thread.

I guess I didn't ask if you have a CNC mill. If you don't then it is tap and cleanup time. If you do, a thread mill goes to the bottom of the hole and helixes back out at the thread pitch.

Ed.

 

[Mike1974]

The short answer is you won't, without some handwork or such as others have mentioned. If it is production work, definitely worth investing in some tooling to do it in machine, otherwise belt sand, grind, file, etc.

Something to consider, if using a c'sink, it will be extra big one way, while barely covering the other way. If you have the resources, I would model a chamfer around the hole and use a small* ball endmill and surface it. More work upfront, but will give you one of the best "chamfers" without being overly ugly/oversize.

* relative to your thread size...

 

[camscan]

Have you tried A roll tap?

 

[Scottl]

A suitably sized double cut carbide ball burr does a pretty good job of creating entrance and exit chamfers for tapping.

 

[wesg]

Some fiddling in CAD shows a bar diameter scallop just works for whatever hole size. It intersects the 'edges', and is tangent at the center. I don't know what principle of geometry is responsible for this, but I'll take it ;-)

So a .375 cutter is the one. I'd probably be looking for something a hair bigger, like 13/32, to give me a bit of a 'flat' around the hole. But a 3/8 should be fine. Just play with the depth until it cleans up decent.

And you should also enlarge the tap drill. The proper calculation for a 1/4-20 would be a #4, .209 dia. Regardless of whether you want to stick with a tap drill chart or not, practically any tapped hole in SS, or tool steels, should be oversized a bit before tapping.

I like the idea of a ball endmill, or burr, also.

 

[TeachMePlease]

And you should also enlarge the tap drill. The proper calculation for a 1/4-20 would be a #4, .209 dia. Regardless of whether you want to stick with a tap drill chart or not, practically any tapped hole in SS, or tool steels, should be oversized a bit before tapping.

Say what, now?

 

[CarbideBob]

Also taps come in many flavors.
Some push the chip forward, others suck it upwards.
Both likely to leave some burr but different sized shards.
The concern of scaring the OD finish rules out an abrasive brush on a bench grinder but they do make brushes that you can run through the hole.
Bob

 

[wesg]

Say what, now?View attachment 298201

Yeah. I know. This came up a couple years back, that thread charts are based on an obsolete, Sellers, thread with a full sharp profile. The formula for a UN thread takes the root into account and results in a larger tap drill for an equivalent percentage of thread.

Machinery's Handbook has the formula, which I stuck in my Excel file with the rest of my engineering calc's. .209 is what comes out for a 75% thread.

But double check, and let me know if I've got something fumbled up.

 

[rons]

Drill

CS both sides

Tap

Quick cleanup with hand held CS (in a small drill chuck or mounted on a handle if needed/desired)

That should do it.

A countersink would probably be good if the ratio of hole diameter to bar diameter is small.
But in this case the ratio is .250/.375 and the counter sink would cut more on the top two edges of the hole and leave a uneven appearance.