Lathe Drill Depth Calculations for 135°-tipped Drills

[MaverickNH]

I’m to drill and ream a 1/2” hole to 3/4” depth (to shoulder) and will use a 31/64” 135°-tipped drill before reaming to 1/2”. Are there handy charts that have data on drill tip lengths for each sized drill? I suppose that depends on trip geometry and don’t know if that’s standardized for 2-flute 135° drills.

My understanding of technique is I can drill my final 31/64” hole by standing the tip off the face with a 0.005” feeler gage and adding 0.005” + the drill tip length + 0.75” to get my total drilling depth on the tailstock quill DRO. There’s little clearance w/o breakthrough on my workpiece.

BRET

 

[markba633csi]

Really it depends on the drill tip geometry and how much material you want left over
at the bottom of the hole (tip of drill) to the outside world
There will be a cone shaped hole bottom after drilling and the reamer will stop there

You could use an endmill smaller than the hole diameter to remove much of the "cone" before reaming
That way you would get a fairly square-bottomed hole

Mount the endmill in the toolpost, then bring it over to nearly touch the side of the hole

 

[rabler]

Unless you really need depth accurate to single digit thousandths, I just start drilling, and zero my DRO when the shoulder of the drill first engages. Having a chip brush on hand is helpful.

 

[RJSakowski]

For a 135º drill, the angle to the horizontal is 180 -135 =45 and 45/2 =22.5º The tangent is 22.5 is .414 an the depth correction is d/2 x .414. or .212 X the drill diameter. Actually it is slightly less due to the width of the web of the drill. .2 x drill diameter should get you close though.

 

[RJSakowski]

If I need to drill to a precise depth when I am drilling holes, I will advance my drill until I I just begin to cut the shoulder, zero my readout and go from there. I only go to a precise depth if I am impacting some feature on the back side. Otherwise, I drill to the prescribed depth and add some .05" or more for good measure.

 

[Jake M]

There's nothing wrong with your theory, except you have to know that distance. It can change depending on how the drill is ground. But it's a good approximation. You also have some small radius on the reamer that will need to be accounted for. If you were doing production work, that might arguably be the best way to set up a punch card.

Personally, if I were doing a one time thing, (and I had a DRO....), I would use the feeler gauge/drill tip/DRO zero you mentioned NOT to calculate the depth of the half inch reamed area, but to set the " safe enough to not blow through" point. How long is the workpiece? how much do you have to work with?

You didn't say, but if for example, this was a one inch long piece that's a quarter of an inch to work with. Less 0.100 for the drill tip (pencil and paper math, verify that), you'd have 0.150 inches to blowout. Which will deform the back before it blows through, you've got to leave "some" material there. Put 0.050 inches in there at minimum to ensure no marks on the back of the part. But I think you can leave 0.100 there.

My suggestion is to use the feeler gauge to find the drill tip, "find" that tip with the feeler gauge as you said, drill in 0.900 from the TIP, not the diameter, which will leave 0.800 of drilled cylindrical area. That leaves 0.050 "window" which is plenty to burn up any radius that will be on your reamer, and still leave a somewhat comfortable safety margin at the cylindrical reamed hole depth, (you can always drill deeper), and a VERY comfortable margin at the blowout point (which pretty much scraps a part).

Basically what I'm suggesting uses the same math as what you're suggesting, except I've changed the reference points so that the "subject to real world error" parts are moved to where you can recover from a little discrepancy.

For a THEORETICAL 135 degree drill point (tan22.5)X(1/2 drill diameter) will tell you how tall the theoretical point on your drill should be. If we assume the angle to be correct, then any small error from the grind (if it looks "good" at the point, that won't be much) will make the tip's actual point "shorter" than theoretical. The only way to make that point longer is to mess up on the angle of the grind.

 

[benmychree]

You can also grind a drill to produce a flat bottom in the hole, I just grind the drill to resemble an end mill, all by hand, you just use a standard pointed drill to start the hole nearly to depth, then use toe flat bottom drill to finish the bottom of the hole flat; this is common practice with old fashioned machinists such as myself.