Form grinding a straight flute carbide drill.

So I'm currently running into a new problem at work where I am drilling an ID of a part with a fairly large tolerance of .330-.350 and a full diameter depth of 2.110"-2.170" and the blueprint calls out for a 114° to 122° drill point at the bottom of the hole. The material is 15-5ph heat treated to 38-42 HRC. The kicker is the radius that makes the shoulder that goes from the diameter into the drill point needs to be .050" - . 070". Our solution is to go in with a 5/16 jobber drill with 118° point to rough out the hole, and form the finished drill point. Then we go in with an 11/32 drill with a .060" radius ground into the cutting ears and the drill tip ground to a flat bottom. Then match up the endpoint on Z so there is no mismatch between the two. They do not want to spend the money on carbide so both drills are Guhring Cobalt. I don't understand why we can't grind a .060" radius into a drill without taking off the drill point. Or even why cant we grind the .060" radius into the cutting ears of a straight flute 118° carbide drill? Why would that not work like a straight flute form drill and get the job done with one tool? When I ask people at work no one can give me a straight answer. Thank you for your time and God bless.

Bulletsnatch said:

So I'm currently running into a new problem at work where I am drilling an ID of a part with a fairly large tolerance of .330-.350 and a full diameter depth of 2.110"-2.170" and the blueprint calls out for a 114° to 122° drill point at the bottom of the hole. The material is 15-5ph heat treated to 38-42 HRC. The kicker is the radius that makes the shoulder that goes from the diameter into the drill point needs to be .050" - . 070". Our solution is to go in with a 5/16 jobber drill with 118° point to rough out the hole, and form the finished drill point. Then we go in with an 11/32 drill with a .060" radius ground into the cutting ears and the drill tip ground to a flat bottom. Then match up the endpoint on Z so there is no mismatch between the two. They do not want to spend the money on carbide so both drills are Guhring Cobalt. I don't understand why we can't grind a .060" radius into a drill without taking off the drill point. Or even why cant we grind the .060" radius into the cutting ears of a straight flute 118° carbide drill? Why would that not work like a straight flute form drill and get the job done with one tool? When I ask people at work no one can give me a straight answer. Thank you for your time and God bless.

Click to expand...

Interesting problem.
Question - why on earth does a 2" deep hole need to have a 60deg radius on the bottom of it? That is interesting.

I guess I don't see a reason that this wouldn't work, as goofy as it is. You would want to make sure that the geometry of the ground drill still allows for shearing and chip evac. I have a feeling that slapping this on a diamond wheel pedestal grinder is not going to yield a good result. You'll need to make sure both edges are ground exact or else you're going to have issue. I could be wrong but this sounds like a job for a CNC grinder. Perhaps you could get a custom drill modified through your vendor?

The answer to "why" is that it is probably easier for whoever did it first.

What's the quantity of parts to run? Does this job repeat? Has the company been doing it this way for years? Are the drills with radii on the corners shop made, or were they ground by an outside vendor?

I haven't looked up straight flute carbide drills, but *most* carbide drills have a bigger angle than 118, while it's easier to get cobalt or HSS with 118.

Cobalt drills are cheaper than carbide. Quite a bit cheaper.

Do you have through spindle coolant to justify trying to run a carbide drill 2 inches deep?

If the form drills were made in house, it was probably easier for the guy to put a radius on the end of a square bottom. Although I think most people here could do it by hand on a regular drill with a 118 tip.


Without knowing some of these answers, I'd probably rough drill the thing just as you are, but my form drill would also have the 118 angle on it, so i wouldn't have to worry much about mismatch.


If you have thousands of these holes to do and a machine with through spindle coolant, sure, maybe getting a form drill out of carbide would be worth the extra cost, because of time saved. But if you've got a hundred of these to do and you've already got a half dozen tools whipped up with a proven program, why rock the boat?

I'm making the part on a lathe I don't know why it needs a .060" radius going into the 118°.
The part is some sort of linkage rod end for the launch bar of an f-35. I have to make about 150 of them and I have the capability of using through coolant if I had a through coolant drill but my boss doesn't want to buy them. We send the flat bottom drill out to get the radius ground on it so we could send a straight flute drill and get the radius ground on it. The problem I'm having is convincing my boss that it's even possible. he says if I turn the cutting ears on the drill to a radius I will lose my cutting capability and the drill won't cut it will just break. I said if we could do it to a flat bottom drill we should be able to do it to a drill with a drill point. But he still said no.

So you just need a .060 rad on the corners of a 118 degree drill?

I'd freehand that radius on a bench grinder and do it in one shot. Only need 150 holes, and if the drill wears out do up another. How will it be inspected?

Bulletsnatch said:

The problem I'm having is convincing my boss that it's even possible. he says if I turn the cutting ears on the drill to a radius I will lose my cutting capability and the drill won't cut it will just break.

Click to expand...

I could be misunderstanding your description, but it sounds like a racon point, or maybe a bickford. If so, they cut fine, I used to do this all the time to normal drills for use in nasty stainless (the kind that screams and howls when you drill it). They work super.

http://neme-s.org/2005 May Meeting/drills.pdf

I see sort of a Racon or Bickford but full rad outside edge.
Easier done on a straight flute. Gets more complicated on a heilx drill as the top surface rake winds up more positive and the edge may get too weak.
On a helix drill dubbing the area of the flute in the rad area may help. Sort of a gash on the outboard edge.
If full hole flat front drills do not self center very nicely so 118 point better.
Unsure why the boss thinks this will not work. Perhaps experience with bad grinds as flank clear is a problem in this grind.
More expensive by far but should actually outlast a normal drill as the chip is thinned at the highest wear area of a drill.
Bob

Bulletsnatch said:

I'm making the part on a lathe I don't know why it needs a .060" radius going into the 118°.
The part is some sort of linkage rod end for the launch bar of an f-35. I have to make about 150 of them and I have the capability of using through coolant if I had a through coolant drill but my boss doesn't want to buy them. We send the flat bottom drill out to get the radius ground on it so we could send a straight flute drill and get the radius ground on it. The problem I'm having is convincing my boss that it's even possible. he says if I turn the cutting ears on the drill to a radius I will lose my cutting capability and the drill won't cut it will just break. I said if we could do it to a flat bottom drill we should be able to do it to a drill with a drill point. But he still said no.

Click to expand...

AH, that is the reason they want a radius. Eliminating a stress riser for military use.

Houndogforever said:

AH, that is the reason they want a radius. Eliminating a stress riser for military use.

Click to expand...

Yes but ours is not to reason why or even think about it.
The customer wants a radius and they get a radius as specified.
Our op in a how and that should have been thought about at quote time and not tossed to the floor as a problem to solve.
It all looks so easy in the computer and CAD.
I wonder if this job has the custom tooling in the price tag. Here is where the machine floor gets blamed for not meeting the quote.
Bob

It absolutely wouldn't surprise me if it did have it in the price tag

So at the very least we could send a Cobalt drill out and have the radius ground into the corners? And it would work?

I'm not sure either. He seems to think that the hole is non functional because the hole is in the threaded shank. Since we make a lot of assemblies that mentality of knowing what you can get away with is taken with non assembly parts as well. But we unfortunately I am limited on what I can work with. If I can tell him I can do it with a basic Cobalt jobber with the radius ground into the corner I think I can get him to do it.

Drills are more fun.
On can get a hold of turning, milling and single point boring,
Drills get so complicated.

mhajicek you got to shove a bunch of dental mold inside and stir it around for a minute or two to get all the air pockets out. Then Jam a pair of tweezers in there pull it out and hope for the best. Then you check it on the comparator.

QT: [The part is some sort of linkage rod end for the launch bar of an f-35. 150 count to do.]
I think it is odd to go into the hole with a .360 flat bottom straight flute drill with a .060 radius on its ears. The OP has not stated if the radius straight tool is a two flute.
Good that the Op is thinking, and better answers from the boss might be due.
The tools used seem odd because it is possible to error on the intersect of the .060 radius and the 118* drill point, perhaps that intersect doesn't matter, and that fact is known to the engineer? But consider, they seem to be sending that cutting tool to a specials shop.

If my job I think a .360 reamer would make a better bore and with .060 radius might better finish the operation. A 23/64 reamer is a standard and would cut a smooth straight bore, so I would likely go with that having the .060 radius. I might even try a reamer that has that radius, and two flutes going to the 118*point. * or just the straight drill with the 118* point left on, so just adding the .060 radius. Yes still going in with a pre-drill hole. A simple tool to make on the likes of a Royal Oak.

RE; A straight flute drill offers a very good finish hole, and no pull-in as might a spiral flute drill, so that may be a good/best choice.

It is very common for a tool guy to hand radius a drill or reamer. Just by eyeball to radius gauge is Ok. The more professional way is to circle grind an angle or couple angles at the intended radius, and then hand backoff/roll the radius. likely I would not recommend this shop to try that / do that for a high price part for an f-35 launch part.

REF: drills
parts of a drill nomenclature - Bing

Re: On the Royal Oak one can make a male of the desired form/shape and then crush that form into a crushable grinding wheel. Then that form is ground to that cutting tool in one smooth form grind all together, first as a circle grind and the n with a 1/2 * kick to then add the clearance to a land for cast iron, or to Up-sharp for steel.. There in no fancy/difficult trying to match the radius to another angle as is done on many other tool and cutter grinder machines.

The tolerance on the diameter of the hole is pretty big the tolerance on the full diameter depth of the hole is like a mile. There's no need for a reamer. Thank you everybody for all of your help and thank you for that awesome PDF file with all the information on drills. I only have a few years experience but I've learned a lot just from this thread. I showed my boss and he had no argument but he still said no maybe next time. I get what I get and I don't throw a fit I guess. I got a $2 raise yesterday so I don't have any argument either. You all take care and God bless.

Bulletsnatch - Try Dan at Primier Tool grinding out in Avondale - They can whip that out ricki-tik

B&T Tool Grinding on Broadway can do that too...

Grinding this on a straight flute easy.
I would never try to hand grind if unless you have a mile of hole variation to play with.
Now way you get these two in sync.
Now you have a imbalanced load and that drill is going to flex and follow. Maybe bad enough to bind and break or enough to make a bigger hole.
Part of the deal here the outside lip edges and height, other the rad itself.
Bob

Sorry for taking so long for an update my boss fought me tooth and nail about the drill and we kept trying it his way. I eventually got fed up and went behind his back put the radius on the drill myself with a diamond file and the comparator and it worked perfect. Ended up with me getting a pat on the back. Thank you all for your input I would not have been able to do it without you guys