why long holes are bent ?

I have been experiencing this for quite some time and usually it's not a problem because most of these holes are for accomodating bolts so the precision required is not very high.

However I am interested in knowing why. Is it because of the quality of the drill bits ? Just last week I drilled a 3.3 mm diameter, 33 mm long hole through a 7075 aluminium rod with my Emco Compact 8 lathe. A 3 mm spot drill was used to start the hole. I can put the drill through the resulting hole without any resistence but a 3.3 mm gauge pin would stop at about 3/4 of the length of the hole. If I insert the gauge pin from the other end, it stopped at 1/4 of the length indicating that there is a bend there. Wondering what the cause is and how it can be avoided.

3.3 mm drills are reasonably flexible and will take the path of least resistance in a deep hole, i.e. relative to the diameter of the drill. The fact that the bend appears to occur at a specific location suggests that there may be a hard spot in the aluminium ( not an unusual occurrence ) at that point and the drill has deviated either enough to go around it or to the point where it will not bend further and forces its way through.

I suspect that someone will be along shortly to provide a formula for drill diameter, hole depth and flex in a uniform material but I don't think that is what is happening here.

Pero

It's called Wander; for longer holes there are techniques that can minimise it. Gundrills for example have a coolant channel up the centre to help combat work-hardening and remove swarf which can both contribute to wander, as well as being more rigid than normal drills. These are for specialist workshops of course.

At the level I'm working at (a very small amateur workshop with a tiny budget) I have to use techniques like "pecking" the drill to reduce the wander rather than using long sustained cuts, stopping to clear swarf on a regular basis, and where possible finding ways to avoid doing it (such as making a component out of two smaller pieces or going from both ends and meeting in the middle, with the issues that entails). Obviously none of these are ideal solutions, but they minimise the issues. By using a spot/centre drill first you are giving yourself a fighting chance of getting it right at the start at least.

Other things that can make it worse are excess pressure and a poor grind on the drill bit (sharpening the drill bit and not getting it quite even on each flute).

At the size you are drilling boring the hole isn't really an option, however in larger sizes thats the idea way of avoiding wander. But the best bet at my level is to drill undersized and then ream it with a parallel reamer.

I know thats a lot of info but hopefully some of it will be of some use.

When I had to work for a living I was making some workshop instructions. One of the points that can remember was the depth of the holes which can be reliably performed without too much care.....this was three times the diameter. In the case of a 3.3mm diameter hole, a reliable hole depth could be 9.9mm. Obviously this is a worst case, as mentioned, pecking is a cure as is cleaning the drill, using a sharp good quality drill etc etc

cheers

Bill

Drilling a straight hole 10 times the diameter (10D) is no mean undertaking, 3D is 'normal' and anything over 5 takes increasingly more care and attention. The simplest solution is to avoid small deep holes at the design stage.

As noted above, for an essential 10D hole I'd use a drill about which I had no doubts, use a short drill to make the pilot as straight as possible, use the correct speed, feed the bit in positively yet without forcing - let the drill cut and use some 'feel'.

I find the most important thing once over about 5D is to withdraw the bit and clear the chips frequently - if you pull the bit out after feeding in 3mm and can see chips are already packed in the flutes, then you will have to do it earlier next time; it's tiresome, but is key.

Different materials and drill bits 'pack' at different rates - if you can see chips 'sticking' there, make more frequent withdrawals.

I would pilot drill and complete the hole, to size, with a suitable end mill - they are much stiffer than a common twist drill.

Certainly need much more difficult, once more than 5 times the diameter, but attainable with care.

Not done it with holes as small and deep as the OP wants, but it works OK with intermediate holes that are a bit tight to bore easily.

Drills are a roughing tool, not a precision finishing tool. They wander. They drill over and undersized. They leave burrs. Your hole may not be bent, it may just have a slight burr or tight spot where it hit a hard or soft spot in the metal. Or not. Joe Piezinski has a good video on YouTube about drilling deep small holes. He drilled and then bored the first 5 or 10 mm of the hole to provide a dead true guide for the drill bit on entry and says that helps hold it straight all the way through. You will need a real small boring bar to do that on 3.3mm but it can be ground up from a blank of HSS.

Worth a watch: The theory is interesting at the beginning. He gets to the long drilling later on.

Edited By Hopper on 14/07/2022 08:33:11

Far too long ago to think about I worked in a jobbing machine shop where we did a fair amount of work for two local blow moulding factories. One of the items we did an awful lot of were 'blow pins'. Turned from stainless in sets of three they had a uniform shaped threaded top end and a long varying much smaller diameter lower end to suit the particular moulding (bottles) and varying lengths about 150-170mm long

They had a hole drilled right through which was done from both ends. Agreed, it only had to pass air which meant accuracy and perfect alignment wasn't an issue and yes the drill did wander at times but more often or not the holes would allow the drill to be pushed right through after drilling. If I recall correctly the largest drill was 5mm diameter and with some 4 and occasionally 3mm the latter a particularly fraught time. I well remember doing one when the drill wandered enough it broke through the side of the pin which was about 7-8mm diameter.

Done by hand on a Colchester 2000 lathe only basic HSS jobbers drills were used - standard and long series so nothing special and the drilling began with a short series drill to get a good concentric start.

As has been said pecking and frequent withdrawal with plenty of coolant was essential to aid swarf removal - a tiring exercise when the tailstock was constantly being moved and several batches were sitting there to be done.

My, that was along time ago

Tug

Edited By Ramon Wilson on 14/07/2022 09:02:01

I think that most have been covered by those mentioned above.

1 smaller drills tend to wonder more

2 blunt drill

3 incorrectly ground drills

4 material hardness through out (Hard spots

I find that pecking helps a little. As I work with metal and wood, wood tend to be the worse as it has grain which has soft and hard wood especially in the growth rings(OK not applicable in your case)

Another vote for Joe Pie. When you listen to what he says, it makes sense.

Thanks for all the answers. Just surprised by how much it takes to make a long straight hole.

Back in the 70s, standard instructions for drilling in automatic lathes was first peck after 3 diameters depth, then 1 peck for each diameter thereafter.

But I suspect that was more for surface finish in the hole than straightness - although of course they're not entirely separate issues.

I've come to the view that - given the grind is symmetrical on angle and lip length - pressure is the most significant variable under user control. If you feel vibration through the tailstock handwheel, there's likely catch-and-slip going on at the cutting edge. If you can eliminate it by backing off a little and then applying light forward pressure you might well keep the hole straight enough.

Endmills or slot drills are much more rigid than jobber drills, but they also cut on the helical flute land, which a twist drill doesn't, so you can be exchanging the risk of a bent hole for an oversize one unless tailstock alignment is very good.

Like a lot in engineering, it's a matter of particular circumstances, priorities of different features of the hole, time, cost and patience pressures on the operator, etc.

Edited By Mick B1 on 14/07/2022 10:42:05

would it be any use using a 1.5mm pilot and finishing with a 3mm d bit?

Tug, I just finished a set of 3 pins this week with 5mm holes through. The secret to drilling the long straight holes is the very start. I used to start with a Centre drill, and they always had some wonder. These ones I started the holes with a 6mm ball end mill to about 5.5mm diameter. Then went in with a stub 5mm drill, 15 mm deep. Then went in with a jobber drill, then with a long series drill. Sharpening the drills , so that they are even cutting from both sides and carefully either web thinned or 4 facet sharpened. I find the chisel point is good as it has very low pressure required to make it cut, compared to the conventional drill end grind. These pins are from 420 stainless, so not easy to drill. We also drill about 250mm deep with 8mm holes for injection cores, and the end of the hole is required to be quite concentric to the outer diameter by 0.1mm TIR. Quite often the drilled holes are well within the runout and roundness. The last batch the holes were round to about 0.02mm-.03mm tir at the front of the hole, and about the same at the end. We have a way of setting them up and trueing the hole to the stock, then finish turn the outers to suite. When I drill those holes, I put a very small radius on the outside corners of the drill. Gives a very nicely finished hole, and often very round too. Pushing the drill or forcing the drill , seems to lead with moved holes, same with the material getting hot. It seems to me that you just can not have too much coolant and regular pecks. On the long holes hand drill with .5mm pecks, and retract every 1.5mm-2mm. I used to gun drill the 5mm and 8mm holes, until the drills got damaged and were never replaced. I prefer for long hole drilling the shallower or longer point grind of the drill, so is about 120 deg included angle, compare to the standard of 135 deg. I have never had much luck with the flatter grind angle I see on alot of the long series parabolic fluted drills for making very straight holes.

Neil

If I had to design a part with a long through hole, where possible I would drill a larger diameter then finish with the small hole through the last bit. In most cases there is no need for a long small diameter hole.

You would need a new drill from a top manufacturer to minimise the wander. My old firm used to make aluminium hydraulic manifolds for Airbus. They were about 600mm long with a 6mm hole drilled from both ends done on CNC mills. The mismatch in the centre was about 0.75mm, good enough as long as any burr was removed.

A deep hole boring machine is like a lathe, but rotates the drill as well as the workpiece, they produce straight holes.

Edited By old mart on 14/07/2022 17:02:43

The gun maker guys have been dealing with it for years and can offer various solutions

Edited By Ady1 on 14/07/2022 17:42:19