How to handle drill wandering

[dbb-the-bruce]

I've got some ideas on how to handle what happened tonight, but looking for other advice on how to handle and control drill wandering.

What I did

Drilling a #14 hole (just under 3/16) thru a 1" thick piece of hot rolled steel (this is practice, actual part will be 1018 or stainless). Following with a a 3/16" reamer. First hole actually came out great, straight / parallel to two reference sides, checked with a dowel pin and a surface plate. The hole was slightly off position (the point of the practice is dial in precise location as compared to mating part / hole).

Adjusted the position slightly by .004 and checked again and the fit with the mating part was off by almost double? lots of head scratching and finally realized I could measure the entry and exit hole from the reference surface on a surface plate.

The exit hole was off by about .004 - .005 so my adjustment was practically double! Made sense once I figured out the hole was not parallel to the face.

Drill process was to spot with a centering drill (that's what I got) and then just drill through. everything locked except the quill. The #14 drill I have is full length and of questionable origin. However it seemed sharp and drilled fine. The entry was right where I wanted it.

I did have to take the part out of the setup check, adjust and try again. It's possible that I got sloppy with the second setup. I'm using the fixed vice jaw against the reference face as my way to ensure the hole will be square to that face. The part is tall 1" and narrow .3 thick.

I've ordered drill screw / short bits and will try again tomorrow paying more attention to the setup. I think the short bits will help, but it seems odd to me that I could have gotten the face not flat against the vice jaw the second time. could be a bit of swarf but I cleaned everything pretty good.

Like I said the entry was in the right place.

How do you drill straight true holes 3/16 x 1" deep? Again, not looking for advice on accurately locating, that part worked fine.

Thanks in advance.

 

[ErichKeane]

Unfortunately, all but a perfectly ground drill bit will wander, it is the nature of the beast. You can minimize it by drilling a center and drilling in the same step (this minimizes any 'side load'), as well as getting the S&F accurate, but a 2 flute drill bit will flex as it goes through. Stubby bits wander 'less', but something like 3/16, 1" long is going to move.

Typically you drill undersized by enough to make up for it when reaming, usually ~1/64". In this case, you are only under by ~5.5 thou, and that is not enough, even a truly drilling bit will drill that much oversized some of the time.

 

[Ulma Doctor]

boring is the only real way to expect a straight bore,
but that gets exponentially difficult as the intended bore reduces in size.


peck drilling with undersize stiff bits and a low runout drill chuck , seems to be the next best thing, then ream to size

 

[dbb-the-bruce]

Typically you drill undersized by enough to make up for it when reaming, usually ~1/64". In this case, you are only under by ~5.5 thou, and that is not enough, even a truly drilling bit will drill that much oversized some of the time.

Interesting.

I used a standard drill/ream chart and it called for 2% to 3% undersized for reaming, 3/16= .1875, #14= .1820 with a difference of .0055 about 3%. A 1/64th is 3 times that, 0.0 at .0156, also saying "usually a 1/64" doesn't take into account the size of the drill, based on the 3% suggestion, 1/64 is probably a good rule of thumb for holes 1/2" or bigger as bigger drills a way less likely to wander unless you are drilling a really deep hole.

What is the maximum amount one would use a reamer to remove? 1/64th for a 3/16 reamer is 10% undersized. That seems like a lot to ask the reamer to do, but I don't have a lot of experience with reamers.

 

[dbb-the-bruce]

peck drilling with undersize stiff bits and a low runout drill chuck , seems to be the next best thing, then ream to size

I drilled with maybe 4 or 5 pecks. As mentioned, the drill was drilling fine removing material, seemed sharp enough and only needed to peck to remove material when the hole got deep. I also used cutting oil.

I have been a little more aggressive with feed rate when drilling. I'm still learning to let the tool cut rather than rub, as long as the drill is producing long twisty swarf out the top of the hole, keep drilling and keep the feed up. Don't let it get crunchy as the hole gets deep - crunchy is just recutting chips and that's just not going to turn out well.

I'm also using a precision drill chuck. I'll try a little slower feed and more pecking.

Ordered stubby bits last night, I'm sure they will help. I'm guessing a this point that I may have had debri in vise, it wouldn't take much.

I'm actually using a small brass rod on the moving jaw side of the vise to better hold reference face against the fixed jaw. The stock sides are close to parallel but I didn't fuss with it because this is just practice/test piece. The actual stock is better and I intend to use the same soft rod trick to force the reference face flat to the fixed jaw.

Part of this whole exercise is to up my game on precision and accuracy and understand where the weaknesses are in my hobby tools.

 

[GeneT45]

Definitely peck drilling and proper feed. A properly sharpened drill bit, and anything you can do to make the bit more rigid (shorter drill, switch to carbide, choke up on the drill in your chuck, etc.) If the flutes pack they will cause wandering as well as oversized holes. Same with excessive feed rate / force. Some wandering can be anticipated, but 0.004" in 1" seems excessive. A reamer might improve things a tiny amount, but they pretty much follow the bore, so if it's not right it'll just be smooth, on-size, and still not right after reaming. I kind of wing it with reamers, but I'm usually looking to remove no more than 0.020" and often about half that.

GsT

 

[ErichKeane]

Interesting.

I used a standard drill/ream chart and it called for 2% to 3% undersized for reaming, 3/16= .1875, #14= .1820 with a difference of .0055 about 3%. A 1/64th is 3 times that, 0.0 at .0156, also saying "usually a 1/64" doesn't take into account the size of the drill, based on the 3% suggestion, 1/64 is probably a good rule of thumb for holes 1/2" or bigger as bigger drills a way less likely to wander unless you are drilling a really deep hole.

What is the maximum amount one would use a reamer to remove? 1/64th for a 3/16 reamer is 10% undersized. That seems like a lot to ask the reamer to do, but I don't have a lot of experience with reamers.

The amount a reamer can remove is determined by the lead-in angle and the room in the flutes for chips. I do quit a bit of 3/16" reaming, and always use the 64th under without problems.

Another thing you can do is use a "D-Bit" drill bit. The wandering in a drill bit is caused by the two flutes not being "perfectly" equal, so one provides more cutting force than the other, pushing the bit around/twisting it/etc. So a "D-Bit" has a single-flute, so I'm told (though never used one, and I'm not sure how it works with the above) that it will stay true.

 

[rwdenney]

I'm highly experience at cutting holes that wander off-center.

A trick I have used, particularly for deep, small holes that will be reamed or enlarged to size. I drill half-way from both sides. The drill won't have as much stick-out and you can use a shorter drill more closely chucked--that will help. But it will also cut the wander in half, in theory at least.

You'll end up with a hole that has a cusp in the middle, and that's what you will clean up with the reamer.

You'll still want to peck the drilling, and everything else still has to be right, of course.

In my limited experience, reamers follow holes--this method gives it a course correction.

Of course, I'm assuming you have checked your tram to ensure that the drill is at precise right angles to the part. But you should also check that at various extensions of the quill to make sure that the quill moves true in addition to the chuck being straight. On my craptastic drill press, both are wrong in different ways, but one hopes that any well-trammed mill will do better than even a decent drill press.

Rick "something to try" Denney

 

[MikeWi]

It would take some work to set up, but drill bushing should do the job too. Not sure if a commercial one would be a close enough fit for this use, but one could be made and reamed to fit.

 

[RJSakowski]

At a company that I worked for twenty years ago, we had to drill a series of varying sized holes in an epoxy composite that was 50 mm thick, the smallest being 1.25mm in diameter. The holes were precisely positioned and had to be straight. We used parabolic drills and pecking on a CNC mill. We didn't use a spotting drill to start and the drills had to be extra long to drill the 2" depth.

In my experience, if a drill is not exactly centered over center punch of spotted start, it will wander. Holes in excess of 10X the drill diameter a prone to wander. When I start a hole, I will let the drill dwell when it touches to create its own center and then drill or peck drill to depth. This gives me the best shot at an accurate hole.

Another strategy is th start an undersized pilot hole followed by an end mill of near correct size. The end mill will cut a hole true to the spindle axis even if the pilot is slightly off. Then I finish drilling the hole with a drill if depth requires it, followed by a reamer to bring the hole to the final diameter. It's a bunch of faffing around but it produces accerate hole when the part demands it. disclaimer: I haven't measured runout on the e4xit hiles but the application was for 8 dowel pins for locating a sub platr. I normally woulde use 6 pins which is a highly over constrained scenario but don't have a problem with interference; the omplication being that the holes are precisely on position to better than a thousandth.