Lead in chamfer on a tapped hole

[mike561h]

Just curious is there a specific calculation for the chamfer lead in for tapping and the angle.

 

Thanks

 

example

 

10-24 tap

[Josh T™]

Spot it deep enough to chamfer... is that what you mean?

[mike561h]

yes. That what I do this is the call out for the print...what would the call out be for the chamfer

depth and diameter on the drawing.

[chris m]

Personally I'd run .015 over the major diameter on a hole that size, .205 X 90deg would be what you get from us

[PeterM]

I don't know if there is a specification for this, but what I do is program the chamfer several thousandths larger than the major dia of the thread. It leaves a nice, burr free face.

[jeff]

I usually chamfer .015" - .030" over the major.

Depending on what kind of a mood I'm in that day

[Josh T™]

It's usually a 8-10% larger than the Major diameter of the tap.

 

For example:

1/2-13 Tapped Hole

Major Diameter = .500

.500 + (.500 X .010) = Chamfer Diameter of .550

 

That's how we teach it in school

 

HTH

Josh

[chris m]

Josh, you said 10% but your formula shows 1%; not busting your ball$, just a heads-up

 

...and 8% over is [drum roll] .205! Did someone say .205?!?!?! Oh yeah, I did!

[Mgrenier]

I do not agree with that 8-10% thing, a .05" chamfer for a .500-13 hole is really big. What if you have a 2.000-8 hole? I would mean a .20" chamfer. We go with mjor dia. + .030" for all the holes here. And yes we tap those 2.000-8 holes day in and day out.

 

Just my opinion.

[left coast lefty]

.550 dia over a 1/2-13 is a .025 chamfer, last time I checked!

[Mgrenier]

The numbers are irrelevant here, the point I am making is taht a bigger hole does not need a bigger chamfer.

 

Is this more clear lefty?

[Guest CNC Apps Guy 1]

Just enough for a burr free face is all I ever do.

[SydwazShawn]

If you form tap it will need to be bigger. Or tap, then deck face, then chamfer!

[Dave.L]

Best cycle form or cut:

 

1) Drill

2) Chamfer

3) Tap

 

We do like others, .015 per side up to about 1/2" then .03 per side up. We don't normally go over 1" but if we did, we would probably increase the size a bit.

 

Some times we chamfer via a spot drill and other times we contour with a chamfer tool which can take a bit longer but we find the cut has less burr.

[landscnc]

There are times we use a drill same size as major dia. and drill .010 full dia. below surface.

[kunfuzed]

If there's no call out, and there's a "Break all sharp edges .???" to ???" then I'll do that over the major. If no call out then I just do .015 for the heck of it.

[Josh T™]

quote:

---

not busting your balls

---

 

Man! You guys act like my students when I do something wrong! I've been verbally tarred and feathered!

 

 

In our Torrington Machinist Manual there is a spec for tapped hole chamfers that states a 8-10% chamfer diameter over the major. It has always seemed a little heavy to me also but we didn't argue.

 

IMO, deep enough to deburr the hole is good enough. Just be sure you c'sink before you tap. We try to do this when we spotdrill holes with a 90 degree spotdrill.

 

HTH and sorry for the error,

Josh

[Steve Z]

I always go 1/2 the major diameter for my depth (using 90 deg. spot). Example: 1/2-13 tap, I go 0.25" deep with 90 Deg. spot I have never gotten any burrs, and the transition looks perfect to me. Haven't ever gotten any complaint from inspection. Opps...hope I didn't open a can of worms.....

[Tim Johnson]

quote:

---

.550 dia over a 1/2-13 is a .025 chamfer, last time I checked!

---

Hmmm, my calculator says .064 chamfer.

[G10X0Y0Z0]

our standard is major tap dia +.015 regardless of spot drill angle i.e 120° or 90°

 

[ 05-07-2010, 11:09 AM: Message edited by: G10X0Y0Z0 ]

[specv]

.030 over major dia unless its a Helicoil

[K2csq7]

Steve Z. has a plan that works well for him because spot drills don't come to a perfect sharp point. If they did, he would never get a chamfer.

Make sure it's a 90 deg spot drill and the flat at the bottom is < .030 or so.. and his method should work great.