Deep Drilling, Straight, Long Reach, Aluminum

I need to drill some holes in 6061 aluminum. No problem. I have drilled a lot of holes in 6061 aluminum.

The need to be deep holes. I've technically drilled deep holes in aluminum. Just maybe not this deep. Deep relative to drill diameter.

They need to be pretty straight.

This is for a 1/4" pivot/hinge pin. The hole can be large and sloppy (moderately). 5/16 might be to much, but an H or I drill might be tolerable. I might even be able to get away with a J drill. The goal is that there is enough room for the pin to be on center within a few thousandths somewhere in the open space of the hole.

On tiny (1/8 and under) deep holes (relative to the drill diameter) I've just bought carbide drills from Precise Bits. Stubby little carbide drills do drill pretty straight. This isn't like that.

I have to reach past almost two inches of obstruction on one side that prevents the chuck from being lowered beyond that point and then drill through 2 inches of metal for the pivot hole.

I did it with the prototype by spot drilling with an over extended spot drill, drilling a little over half way with a jobber drill, flipping the part (same issue on the other side), and repeating that process. The holes were pretty close, and I sort of wallowed out the little bit of ridge (not to bad) by forcing a drill through the hole off the mill by hand. (Cordless drill).

It was really sketchy, but it just barely fell within spec. Now I need to make 51 pieces like this. I can see it going badly after I get a little tired from making these parts for a few days. The drilling is done as a 3rd and 4th setup after machining on two other faces of the work piece. I have to do the drilling (I think) as two setups because the other side is two such pivot bosses that need to be drilled, and they are 2.005 inches apart. Drilling them from one side would be over

4.25 inches of reach not counting break through. That's just to much for me to have any confidence in meeting my admittedly rather sloppy spec.

I have been looking at parabolic drills, but other than not needing to peck as often due to their ability to clear chips I don't see any benefit for drilling "pretty straight" holes. Only thing I can see that would help with staying "pretty straight" is spot drilling for a good start and a carbide drill to follow.

Of course mounting has its issues as well. The part has an "ear" that is 1.5 (apx) x 2 x .05 that can be clamped in the vise. It does have one saving grace. There is a square perpendicular boss on the back of the part than can register for height and squareness (perpendicularity) on the top of the vise jaw. Once I have a process that works "good enough" I should be able to repeat from part to part fairly quickly.

formatting link

Reply to
Bob La Londe
Loading thread data ...

Some companies make deep hole drills see

formatting link
Note, a gun drill is the traditional method of drilling deep, straight holes but they are probably not what you want to use for your operation.

A solid carbide to start the hole and drill say 3/4 or 1 inch as a guide and than a long fluted drill to finish.

Reply to
John B.

...

...

...

...

...

I'd look at making a jig or fixture with drill jig bushings (like at

formatting link
and
formatting link
) arranged in pairs, one guide near the edge of the part to constrain the shank of the bit, and another to constrain the tip of the bit. Some bushings taper slightly.

Reply to
James Waldby

Besides mumbling something about drill bushings and a fixture to hold them and the workpiece, my real suggestion is to ask if there is any possibility you can talk the customer into milling out most of the material in the 2" portion? Make the one long ear into two short ears like on the other side. If this is just a slightly sloppy hinge pin hole, does it really need to be solid for that length? Being solid won't improve the alignment since that is set by the 2" width, not material in the middle.

Reply to
Carl

That is a perfectly valid option, and one I had considered. The problem really is that I sent the customer a prototype (2 actually linked together) that worked. Now its kind of hard for me to go back whining that its to hard. LOL.

Reply to
Bob La Londe

On Oct 13, 2019, Bob La Londe wrote (in article <qnvhue$og$ snipped-for-privacy@gioia.aioe.org>):

Is there any way to fixture this to a lathe faceplate, such that the desired drill centerline is on the lathe rotation axis? Spinning work, stationary drill, drill is compelled to follow the rotation axis. Start with a spotting drill (with long solid shaft), follow with parabolic drill. Use lots of coolant.

Failing that, make a fixture on the lathe to ensure that the drill bushings are colinear.

Joe Gwinn

Reply to
Joseph Gwinn

My old, worn lathe disproves that theory. Drill bits held in the tailstock most certainly can wobble, and the hole can drift off axis, as clearly shown by reversing a drilled bushing blank in the collet, inserting the drill bit in the hole and turning the spindle. I have to straighten the pilot hole with a boring bar and then drill to final size.

Reply to
Jim Wilkins

On Oct 13, 2019, Jim Wilkins wrote (in article <qnvtor$c1q$ snipped-for-privacy@dont-email.me):

One can almost clamp the tailstock to calm the wiggle. The lateral offset may be off center as well. But these rears cause tapered holes. If the chuck jaws are off, and the workpiece is held at an angle to the rotation axis, you will get crooked holes. The classic way to test this is to center drill a piece of stock held in the chuck, and also turn the outside of the bar without disturbing the chuck, Inside and outside should be concentric, although there may be some taper, not necessarily parallel.

More generally, think of it this way. If one is drilling on a mill, the hole will be made wherever the drill is located when the quill is moved downward. If one is drilling a rotating workpiece in a lathe, if the drill bit isn´t on or very close to the rotation axis, the drill bit will promptly snap right off.

Joe Gwinn

Reply to
Joseph Gwinn

I bought enough stock so I can experiment a little, but I'm just going just going to try carbide drills first. I ordered a long reach solid carbide spotting drill, and a couple jobber length carbide twist drills.

After I ordered the drills it occurred to me I could spiral mill it with a 1/4" end mill if I had periodic retracts to blast the chips out of the hole. I've got some long reach 1/4 end mills. If its a little sloppy the hole might be slightly over sized or if it flexes it might be slightly undersized, but it will spiral interpolate straight. I could just adjust for whatever I get after the first one, or chase the hole with a drill bit afterwards.

Drilling will be faster, so I'll try that first. If I can get "close enough" with carbide drills I'll keep the long reach end mill in mind for some future even tougher drilling problem. I actually spiral interpolate holes all the time on the mini high speed mills for screw and pin holes. Don't know why I didn't think of it sooner. Its something I already do.

Reply to
Bob La Londe

Not to be insulting or trying to start an argument but you seem to be going at the problem arse backward. The best method of determining how to do something is in the pencil and paper stages. As you are "designing" this "thing" the major thought in your mind should be, "how am I going to do this".

Granted you have already started on this project and now you have to solve your problem.... but next time :-)

Reply to
John B.

I'd like to thank you for all the insight and assistance you offered in your post. Here it comes. The thanks will be proportionate of course. I'm going to do it in the next sentence. _____ ___ ____ ____. Oh, well maybe next time.

I already made the part twice. I just was looking for better options. Several people suggested things. Some I'd already thought of. Sorry you didn't have anything to add.

Reply to
Bob La Londe

On Oct 13, 2019, Jim Wilkins wrote (in article <qo072l$3jj$ snipped-for-privacy@dont-email.me):

Yep, if one is slightly off center, but not so much that the drill bit snaps off immediately. This will yield a tapered hole on center. But the drill will nonetheless follow the rotation axis. If the starting dimple is on the rotation axis, the hole will not be tapered. This is the basic principle of the gun drill.

One way to get the dimple on axis even on a loose lathe is to hold a spotting drill in a boring-bar toolholder on the compound, with cutting edge of the tip on the side towards the operator, and move carriage such that the drill slightly off center to the operator side. The drill will now cut an accurately centered albeit slightly oversize dimple. Adjust tailstock so that a pointed rod held in its chuck is centered on the dimple, and then replace the rod with a pilot drill bit, and proceed.

If you want to use an end mill to produce the final hole (I´ve done this), use a pilot drill that provides ample clearance for the solid core of the endmill bit. Note that reground endmill bits will be undersize. Or, one can use a reamer. A piloted reamer is a standard way to ensure that the holes are co-linear despite the gap between separately-drilled sections.

Joe Gwinn

Reply to
Joseph Gwinn

Greetings Bob, One of the problems with setups like your two bosses is that the flutes of the drill don't provide the best location in the short, close boss while drilling the farther boss. So a drill with flutes shorter than the space between the bosses works well in your type of situation because there will be a solid drill shank locating in the first drilled boss. You may be able to use a type of drill called an "aircraft extension" drill. You could also make up your own short flute length drill. This can be done by turning down the shank of a 1/4 stub length split point drill and then soldering it into a piece of straight 1/4 rod. I use drill rod in situations like this becasue it is very straight. Turning down the shank for about a 1 inch length would be more than enough for soft solder to have enough grip to prevent the drill bit from letting go. Another option, and this may be useful for the long hole, is to drill with the spot drill deep enough that the whole 1/4 diameter of the spot drill enters the material for about 3/8 inch. Then drill undersize all the way through with a .letter B or C drill. Then finish with a 1/4 diameter "D" bit. With a D bit you may need to peck but probably not because the hole is a through hole and not much material is being removed. And D bits can be used to make very straight holes. Eric

Reply to
etpm

The dominant characteristic of a gun drill is that it tries very hard to follow a straight line, regardless of where that line is pointed. It has no tendency to follow, or return to, the axis of rotation of a workpiece. The start of the hole is all-important, and is usually accomplished by careful alignment of the workpiece and a drill bushing, or by boring a starting hole equal to the gun drill's diameter.

Reply to
Ned Simmons

On Oct 14, 2019, Ned Simmons wrote (in article snipped-for-privacy@4ax.com):

I see the source of confusion. I should have mentioned that the term "gun drill" has come to mean two very different approaches to achieve very long and slender holes that are straight, as for a rifle barrel.

The traditional approach was to rotate the barrel in a lathe and use a long straight drill held stationary in the tailstock. Often, the lathe was purpose-built. This method is modernized and still widely used: .

formatting link

The other method is the rotating D-Bit on a perhaps hollow rod, where the workpiece is stationary and only the drill rotates - this is what you describe above, and others have explained.

The rotating workpiece approach was first, and people did use the D-bits as well, so they didn´t have to peck drill. Eventually, the D-bit approaches got good enough for use on stationary workpieces as well. This is widely used for such things as coolant passages in heatsinks.

Joe Gwinn

Reply to
Joseph Gwinn

That video is of a BTA drill, despite the text on the page. The voice-over describes it as such. The tooling is is similar to a gun drill only in that the tool is guided on pads that follow the cutting edge(s). In a gun drill high pressure oil is pumped to the cutting edge thru the hollow drill shank and the oil and chips exit the hole thru a groove in the shank. A BTA drill turns that inside out -- the chips and oil are evacuated thru the drill shank.

What I described as gun drilling applies whether the workpiece is stationary or counter-rotating (I was not talking about D-bits). While the D-bit is likely the precursor to the gun drill, the difference between them is considerable.

The most accurate gun drilling on cylindrical workpieces is typically done on machines with a high-speed drill spindle and a slowly counter-rotating work drive.

In any case, none of the tools we're talking about -- gun drills, BTA drills, D-bits, or twist drills -- will self-correct to follow the axis of a workpiece, whether the work is rotating or not.

Reply to
Ned Simmons

On Oct 15, 2019, Ned Simmons wrote (in article snipped-for-privacy@4ax.com):

Well, we are going in circles for sure. I´m talking about how we got here, and you are talking about where we are.

Going back to the original question, if one sets things up correctly, with rotating work as stationary drill (of reasonable stiffness), the drill prefers to follow the rotation axis. As with everything, if one does not get the details reasonably correct, it will fail one way or another. There were many discussions of this on metalworking sites ten years ago. Joe Gwinn

Reply to
Joseph Gwinn

Fair enough and I understand that I was just thinking about things I already had to hand or could  get easily. I wasn't intending to be doing production gun drilling just thought it might be an option to try sometime for some thing I make occasionally the require deep holes.

Reply to
David Billington

Sterling Gun Drills and Elodorado both supply rules of thumb for oil pressure and flow.

formatting link
As a point of reference, the oil pump motor on a deep hole machine is usually comparable to the spindle HP. I've designed and built oil systems as large as 30HP; I've seen large machines with 50-100HP pumps. As Eric says, you need enough flow to keep the chips moving thru a small passage. I'm sure you can fudge the recommended flow quite a bit depending on the nature of the chips and how much you're willing to fuss with clearing chip jams manually.

Reply to
Ned Simmons

True, but that's a more modest claim than your contention: "Yep, if one is slightly off center, but not so much that the drill bit snaps off immediately. This will yield a tapered hole on center. But the drill will nonetheless follow the rotation axis."

Reply to
Ned Simmons

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.