The Art and Science of drilling the perfect hole...Need help from the folder makers

Robert Hankins

Robert Hankins

Joined
May 19, 2003
Messages
1,848
The Art and Science of drilling the perfect hole.
After messing around for the past few weeks I am getting closer, however there are subtle differences I am finding.
Drilling a hole leaves a jagged edge and the hole is not round!
Using a reamer helps but if you have drilled the starter hole to close to the finish size, your reamer only does a so so job!
Where you start out on one side of a piece of steel is not exacly where the hole wind up on the other side!
Different materials and steels using the same drill bit will leave a different sized hole:confused:

Granted we are talking in hundreds of thouthands of an inch here HOWEVER Whe you are making folders it is a big deal!!!

Any advice or tricks you old pro's can pass on could help us all!!!
 
1. use a center drill
2. use a stubby twist drill
3. might want to pilot drill the hole...
4. if you are going to ream the hole, you might want to 'plunge cut' the hole with an undersized carbide endmill to true it up...(i.e.- centerdrill, drill undersize, plunge undersize, ream to size)

i like dormer drills the best, cobalt if you can find it...they seem to produce good holes in carbon or stainless...cutting fluid or oil and speeds and feeds are also pretty important...
 
I found the biggest help in drilling good holes is in having a soild machine and set up, to drill them. I have only made a few folders but the ones I drilled on a brideport milling machine, turned out smoother than the ones I did on my little drill press.

As far a s what drill goes with what reamer I have always use a drill that is at least 20% smaller than the reamed size. I also buy good drills. Spend the money on good quailty cobalt drills and reamers made specificlly for steel.

I have bought cheap cobalt drills and the point is not ground as well as the good ones, I also champer all my holes before I ream, This helps the reamer stay in the center .

One tip I got from Bud Weston was to use undersize reamers. they are about .001-.002 smaller, thus making for a press fit on any of your pivots.



hope this helps
jimi
 
All of the above. I bought a new drill press because the holes started being oval. The bearings finally wore out in the head.

Be sure to adjust the table perpendicular to the drill. Chuck up a bent wire so the tip can just about touch the table and rotate the chuck slowly. The wire tip should have the same gap all the way around. I also use a flat piece of micarta on the table.

Be sure the piece is held securely and not allowed to wobble.

Consider buying a milling machine
 
nadz said:
i like dormer drills the best, cobalt if you can find it...they seem to produce good holes in carbon or stainless...cutting fluid or oil and speeds and feeds are also pretty important...
Click to expand...

Where do I get Dormer Drills?
 
Solid carbide drills, designed for the material you are drilling, or very high quality Cobalt drills. Stub length only. New drills help greatly, if you want precision. You need a milling machine to make a good hole, as well as the proper feed and speed. Carbide center drills are very helpful

Multiple drilling to achieve a certain hole size is not something I recommend. It is the point of the drill that keeps it centered.

reamers are your friend. Again, solid carbide is what you want.

You'll need to get familiar with number drills, too.
 
No such think as perfect :) but with the info above, you can get close.

I use high quailty cobalt screw machine drills and solid carbid reamers.
 
I like high tolerances on folders. I think the pivot should be around .0002 clearnace. For this sort of work you'll need a set of 'tenths pins,' or you're just guessing.

I don't like reamers. I REALLY don't like reamers. They're NEVER right on in size (certainly not within .0001, which is what you'll need if you want to get it right) and they bellmouth holes (You probably won't see it until you get the tenths pins, then you'll see how screwed up the hole really is.

If you're really serious about doing this repeatably, there are only two options I know of:
You can interpolate the hole with an end mill,
or you can drill the hole undersize and hone it to final.
Honing is the cheapest and most reliable way I know to hit these tolerances, with superior roundness and perpendicularity. You can buy a nice used Sunnen hone for a couple grand (sometimes less), a set of tenths pins for a couple hundred, and you're ready to go... Or you can find a shop to do it ... Should be .50 to 1.00 per hole if you're doing a batch, otherwise you'll be hitting some kind of minimum charge, most likely.
 
Good quality reamers are used every day in industrial applications needing higher toleances than you'll ever need to make a folder. If you're having problems with your reamers try another brand.

What kind of folders are you making that use 0.0001" tolerances? 0.00039" is more than enough.

I have a $35K CNC milling machine and using a tiny end mill to interpolate a 1/8" hole would be insane. The machine doesn't have a position accuracy of 0.0001"

Get good center drills, quality bits, sinkers and reamers and use a good drill press or milling machine properly and you won't have problems getting accurate holes where you want them.
 
I am SO anal about this... I can't STAND holes that are not perfect. I don't make world-class folders yet, but I've got holes down pat. So here goes. (It's not that hard and makes the 'Monk' in you happy)

General Rules:
1. If your holes are not round your drill is too fast.
2. Don't start your holes with a center-punch followed with a jobber bit.
3. Don't force a dull bit
4. Always use cutting fluid no matter what anyone else says about it. A fluid cut hole will have tighter tolerances and your bits will last several times longer.

Your motto: Drill straight, sharp, slow and cool.

Setup:
1. Get a dial indicator if you don't already have one.
2. Mount dial indicator on your drilling/milling table.
3. Place a piece of drill rod, a chucking reamer, or high quality bit in your chuck.
4. Adjust dial indicator to ride on smooth shank of rod/reamer/bit.
5. By hand-turning arbor, verify that rod/reamer/bit runs true. Re-chuck the rod a few times and test each time. If you have more than 0.002" runout don't proceed until this is fixed (bad bearings? bad chuck? cheap junk?) I have my rig adjusted down to ~0.0004" on the drill shank (HF mini-mill).
When you can chuck up a rod/reamer/bit and it turns true proceed to the next step.
6. Remove the magnetic base from your dial indicator stand.
7. Adjust indicator position on the two rods such that you can chuck one rod up in your press/mill and the other rod extends horizontally with indicator pointing down toward table. Adjust so that indicator can be swung around the periphery of the table like Bruce's 'Z' wire test. Changes in indicator reading as it moves in a circle around the table (Turn by HAND!) will indicate if table is true or not. I use aluminum foil (smooth out the wrinkles!) as shim material and adjust until there is no more than 0.002" (count those zeros) variation across the entire table surface. (See I said I was anal) A flat table is important because not only do you need straight holes, but if the table is off of true then if you move your workpiece between drilling operations your bit will never be lined up with the pilot hole. They will be at different angles.
8. Now that your quill runs true, and your table is true it's ready to start drilling.

Drilling:
1. Start with an appropriate sized starter bit. There are spot drills, step drills, and combo bits. I like to use these starter bits with combined countersink.
2. Put a drop of cutting fluid on the piece to be drilled and with apropriate speed and pressure start the hole.
3. Stop drilling before the shank of the bit past the countersink reaches the material. Your hole should NOT have any portion of straight side yet - it should be countersunk all the way to the top of the hole. If the countersink is recessed in the hole you went too far.
4. Switch to a machine drill (short shank drill bit) or a jobber. At this point you can pilot drill the hole with a bit the same diameter as the nipple of the combo bit, or you can go right to a bit the diameter of your starter bit shank. You'll have to experiment with technique and materials to find what works for you.
5. Drill through the material with the bit you have selected.
6. If you piloted the hole in the previous step now drill with your final bit which should be the size of the shank of your starter bit.
7. Carefully countersink the rim of your hole with an appropriate countersink tool. I typically do this operation by hand only just removing the bur around the lip of the hole.
8. Ream the hole to final size at moderate speed and quick feed with a lubricated chucking reamer. Reamer is not for hogging. It should remove very little material (sorry I don't have my Machinery's Handbook handy for exact specs. I'll look it up tonight and post back) For some this is the final step. For the ultimate hole do this step with a 0.001" undersize reamer and go to step 9.
9. Using a brass barrel lap (less than $10 from MSC) and fine diamond paste lap your hole to final size and internal surface finish. Brass barrel laps are adjustable and with patience you will end up with a hole with tolerances tighter than can be accurately measured in the home workshop.

If your bit chatters durring any of these operations you are spinning it too fast. This is the biggest problem with most drill presses.

The above steps were taught to me by Don Robinson (tool&die maker, teacher, and knifemaker extrordinaire). The optional step #9 I got from the amazing Johny Stout.

-Ben M.
 
Kevin Wilkins said:
Good quality reamers are used every day in industrial applications needing higher toleances than you'll ever need to make a folder. If you're having problems with your reamers try another brand.

What kind of folders are you making that use 0.0001" tolerances? 0.00039" is more than enough.

I have a $35K CNC milling machine and using a tiny end mill to interpolate a 1/8" hole would be insane. The machine doesn't have a position accuracy of 0.0001"

Get good center drills, quality bits, sinkers and reamers and use a good drill press or milling machine properly and you won't have problems getting accurate holes where you want them.
Click to expand...


I suppose it's all what you're used to using (and happy with) and what you're after.
I'm working on a folder project that has a few areas calling for .0002, including the pivot. ---Going into the third prototype now, but we've done interpolation for .1865 and have had it honed. Both seem perfect, but honing is a lot less headache. We're getting a pivot with no perceptible blade wiggle in assembly or just loose on the pin. Assembled, the thing opens smoothly with a light touch and you can't wiggle the blade even with the lock unloaded. (There's more to getting this than just a tight tolerance on the pin, but that part of it.)

I'll admit, I'm the designer on this project, not the machinist. (He's an aerospace guy that is used to getting high tolerances on a mill--something of an artist at it, really). We're doing some challenging things on this knife.

One crazy thing is a sliding, oblong lug/slot fit with less than .0005 total clearance. That's four surfaces cut with by end mill with tolerances that, combined, result in clearance between .0005 and .0002. ---Sounds nuts, but that's optimum for this particular thing (though you could double that tolerance and it would probably be acceptable to most folks.)

Kevin makes some nice knives, and if he's getting good results with reamers, I won't argue with him. My experience is different and my machinist won't touch them for really tight work that has to be repeatable.

Honing seems an easy and (relatively) cost effective way to get optimum results reliably.
---take it for what it's worth.
 
If you're only doing a few knives, Messinger's approach (ream undersize and lap to final fit) is a good way to get a great fit. A lot of guys do it this way.

Some people will warn about using diamond in this situation-- the idea being that the diamond particles stay in the surface of the metal and contribute to premature wear. I don't know if this is true.
 
Well, I do get good results using high quality reamers and working carefully. Ben has given a really good set of instructions for anyone to follow a few posts above this one.

Blade wiggle is not a problem on my knives.

I design knives to work reliably with tolerances around 0.0004" or about 0.01mm where fit is critical. Tighter tolerances wouldn't make my knives any better, it would just make them a lot more expensive.

I do have the barrels of my hardened pivots lapped by an outside vendor but generally I like to do all the principle work (except heat treating) personally in my own shop on my own machines. So to start holding 0.0001" tolerances I'd need to invest in an entire high accuracy measuring area with temp. control and really expensive measuring instruments for starters. As it is, I can't reliably measure 0.0001" increments. Truthfully, I can't see how such an investment would ever pay off, not for me (if I used it to make knives) and not my customers, if they're buying my knives.

Of course there are many workshops in industry where such tolerances are required. I haven't heard of anyone investing in setting up a shop like that to make pocket knives... or of any knifemakers having the dough to hire work done in such a shop to those kinds of tolerances.

So you've sure made me curious to see what kind of a knife you guys are making and hear what they're going to selling for. How about posting some pics!!
 
Kevin Wilkins said:
Well, I do get good results using high quality reamers and working carefully. Ben has given a really good set of instructions for anyone to follow a few posts above this one.

Blade wiggle is not a problem on my knives.

I design knives to work reliably with tolerances around 0.0004" or about 0.01mm where fit is critical. Tighter tolerances wouldn't make my knives any better, it would just make them a lot more expensive.

I do have the barrels of my hardened pivots lapped by an outside vendor but generally I like to do all the principle work (except heat treating) personally in my own shop on my own machines. So to start holding 0.0001" tolerances I'd need to invest in an entire high accuracy measuring area with temp. control and really expensive measuring instruments for starters. As it is, I can't reliably measure 0.0001" increments. Truthfully, I can't see how such an investment would ever pay off, not for me (if I used it to make knives) and not my customers, if they're buying my knives.

Of course there are many workshops in industry where such tolerances are required. I haven't heard of anyone investing in setting up a shop like that to make pocket knives... or of any knifemakers having the dough to hire work done in such a shop to those kinds of tolerances.

So you've sure made me curious to see what kind of a knife you guys are making and hear what they're going to selling for. How about posting some pics!!
Click to expand...

You're absolutely right about the cost of set up! That's why I've farmed out this part of the project to someone I trust that is in that world and set up to do it. He's somewhat tired of aerospace and eager to do something 'fun' for a change. This puts me in a unique situation to benefit from his capabilities at a reasonable rate. Up until this project, I too have done everything, specifically forging damascus, so this is a departure for me.

The knife, though high tolerance, features pretty classic lines, and a unique patent-pending feature that I think will get noticed (maybe not universally loved, but certainly noticed).
The primary reason for the higher tolerances is for consistency in performance. The materials are all pretty premium and I'm pretty picky. I can't afford to be rejecting a lot of parts, and I'm sure not going to be putting out 'good-enough'.
This is a $45K project all told. That's kind of a lot for me. It's really a no-compromise sort of project, but the knives won't be stupidly expensive either.
Trust me, I'm dying to put some out there and see what happens! I should have something in a few months.
 
JCaswell said:
If you're only doing a few knives, Messinger's approach (ream undersize and lap to final fit) is a good way to get a great fit. A lot of guys do it this way.

Some people will warn about using diamond in this situation-- the idea being that the diamond particles stay in the surface of the metal and contribute to premature wear. I don't know if this is true.
Click to expand...

You know, I've wondered about that. I don't know the answer. I think this is one reason that as a rule the lap must be of a softer material than the workpiece.
-Ben
 
Awww, shucks, Ben.

I'd like to add one more thing. A good HSS reamer will cut several diffent sizes depending on the following:

1. Run the reamer about 3/4 to 1/2 the speed of your drill.

2. Drill (for knife sizes) .005" to .010" smaller than the reamer.

3. For metal to metal fits, use tapping fluid.

4. For oversize holes, use water or nothing.

5. For a press fit, use a little lubricating oil. Warning, the reamer may seize in the hole and burn.

If your reamed holes are oversized or tapered, refer to above..;) Leaving too much stock for the reamer to cut will do this.
 
@JCaswell
Thanks for the info! Best of luck with the project, I hope you will post some pics when the knies are on the market.

A very good source for drill bits, reamers and countersinkers, etc is Gühring. The sell in the USA too. Here's their website:
http://www.guehring.de/home_static.htm
 
You must log in or register to reply here.
Back
Top