Deep drilling

[Speedy Builder5Participant @speedybuilder5]

I need to drill some deep holes in Al Alloy (I don’t know the specs, but it machines really nice).  The holes are 3.5mm diameter by 75mm deep.  I can drill from each side. Once drilled, I need to transfer the position of the holes and  tap into a second component.

What is the best way to prevent wander.

Does the the drill speed faster or slower help ?

Bob

[renardiere7Participant @renardiere7]

Mill or Lathe?

[Speedy Builder5Participant @speedybuilder5]

mill/drill, lathe.

[JasonBModerator @jasonb]

I’m not a fan of marking out so would locate the three holes on the face that will mate to the tapped part by finding edges and then use the millshandwheels or DRO to position. Start with a spot drill (ctr drill if you want). Then a stub drill which is nice and stiff to get teh hole started true. Then jobber length and probably have to finish with a long series drill. just drill from that one end.

Somewhere around 2000rpm, paraffin or WD40, peck drill and clear the swarf often. Should not need to say sharp well ground drills.

I also don’t much care for spotting through hole positions so again would us eedge finders and then set the position of the tapped holes with the mill.

[DiogenesParticipant @diogenes]

Use the correct speed for a 3.5 drill in Ali, failing that the highest available.

start with a stub drill, then a jobber, and or a long series if required.

clear the chips often – very often, as you get deeper (peck 1D and then clear) and let the drill do the cutting.

Use bright drills if you have them and use paraffin / diesel / wd40 for lubricant

[HuubParticipant @huub]

In short, prevent the drill from bending, start at the exact center of the hole drill from both sides if possible.

That results in:

To much tool pressure will bend the drill so very modest tool pressure.
Good chip evacuation is an absolute must. So peck drilling is needed.
Start using a center drill.
After that use a smaller size drill (3 mm) the shortest you can get.
Drill the hole to just over half the depth, each time using a longer drill.
Bring the hole to diameter using the same procedure
Finish the hole using a reamer preferably from one side only.

An end mill is often more rigid than a drill. Start drilling using a drill and bring the hole to diameter using an end mill is also possible. 4 Flute end mills have a larger core diameter than 2 flute end mills and are more rigid. So the 4 flute end mill is better.

Whatever you do, it is quit a challenge.

 

[Speedy Builder5]

On 23 July 2026 at 14:22 Speedy Builder5 Said:

I need to drill some deep holes in Al Alloy (I don’t know the specs, but it machines really nice).  The holes are 3.5mm diameter by 75mm deep.  I can drill from each side. Once drilled, I need to transfer the position of the holes and  tap into a second component.

What is the best way to prevent wander.

Does the the drill speed faster or slower help ?

Bob

Use a new long series drill of known decent make.

Centre drill the location or use a spotting drill.

About 2000 rpm with minimal feed, peck it every 2-3 mm with WD40 as lube, clear the flutes with a small brush, blow out the hole with comp air, more WD40 down the hole, then back down the hole again with the drill, rinse and repeat, be patient, don’t try to rush it.

Try the speed out on an offcut if possible first, if the metal welds to the drill, cut the speed down.

 

[JasonBModerator @jasonb]

You should not get metal sticking to the tip at 2000rpm, it is very conservative but I said that rather than 7000rpm as most people don’t have machines that go much above 2000. I’d be up at my max of 5000rpm on the CNC but the manual mills top out at 2000.

[Speedy Builder5Participant @speedybuilder5]

I don’t think I have ever owned a stub drill, perhaps time to buy one now.

Thanks for the advice – there will now be a short interlude before I publish the results.

Bob

[JasonBModerator @jasonb]

If you do inverst in one or a few try and get a make that has a split of 4-facet point. Dormer A022 for me.

The majority of the time these can be used without a punch mark or spot/ctr drill dimple. I have them in all my common tapping, reaming sizes as well as 0.5mm increments  and they get used far mor ethan the standard Jobber length drills.

[JasonB]

On JasonB Said:

….split of 4-facet point. Dormer A022 for me. The majority of the time these can be used without a punch mark or spot/ctr drill dimple.

I concur with one caveat; the suface needs to be flat. Even 4-facet drills can wander on a curved surface. I use Dormer A002 jobbers drills as standard, two sets 0-6mm and 6-10mm both by 0.1mm.

I would start with a carbide spot drill, then a stub drill, standard jobbers drill and a long jobbers drill if required. To get the holes in two parts to line up there are two options. One, do the drilling with the parts assembled. Second, drill the first part from the mating surface rather than the top. Then it doesn’t matter if the drill wanders slightly.

There is one golden rule to avoid drill wander, buy good quality drills that are properly ground. Also the mill needs to be accurately trammed and have a quality drill chuck.

I find WD40 to be good for drilling aluminium alloy; not so much for lubrication but it stops the swarf sticking to the flutes and jamming the drill.

Julie

[egaParticipant @ega]

I find it important to “listen” to the machine – lathe, drill or mill – and for this a lever-operated mechanism is helpful, both for improved feel over a screw feed and for instant withdrawal.

According to Duplex, the ideal is counter-rotation eg work in lathe chuck, drill bit in rotating device of some sort.

Who is the favoured supplier for stub drills? (I have used The Drill Service in the past).

[Julie AnnParticipant @julieann]

My first port of call for drills is Drill Service, but their pricing can be rather inconsistent at times and I have had the odd duff item. Albeit the last one was a 0.5mm diameter milling cutter that kept breaking on the CNC mill. Changed to one from Cutwel and it ran fine with the same CNC program.

Julie

[Paul LousickParticipant @paullousick59116]

A good video on Youtube by Joe Pie about machining straight deep holes.

 

[JasonBModerator @jasonb]

Have gone back to using MSC Direct for my Dormer drills, I used to use them in the past until Ketan started doing them but have now had to go back to MSC.

[DiogenesParticipant @diogenes]

Stub drills? As per JasonB – Dormer A022-series work for me – not really any telling who will be cheapest on the day but a set going up in 0.5’s is worth chasing-up – I use mine every workshop day..

i will get the box p/no. if I’m up there later..

[egaParticipant @ega]

Thanks to Julie et al for the pointers to drill suppliers.

I’ll look at a set by 0.5s but am mainly interested in tapping sizes and double-ended drills.

[Speedy Builder5Participant @speedybuilder5]

It sounds expensive buying a full set of stub drills at this stage. More than 60 years ago, I “earned” a full set of drills, Fractions by 1/64″, Number and letter drills and still have them as full sets however the drill points have wandered over the years of re-sharpening by eye.

Now they are complimented by metric drills  1- 13 by 0.5mm increments for day to day usage but are not much use when used for tapping as the sizes do not correlate to the taps.

I constantly use a Shetac drill size calculator which again after 60 odd years is showing its age.

Bob

[JasonBModerator @jasonb]

I only bought what I commonly use in stub length, anything else can be spotted and drilled with a jobber. My jobber 1/16th to 1/2, 1-5.9 and 6-10 sets in 0.1mm increments started out a cheaper sets but over time I have replaced when needed with Dormers.

[DurhambuilderParticipant @durhambuilder]

It’s horses for courses. From your previous posts it looks as if these holes are the cylinder fixings on a farmboy IC engine. Assuming that is correct then you would be better off drilling the cylinder from one end and use transfer punches (a sharpened length of silver steel rod) to transfer the hole positions to the mating part. A few thou out of the drawing position buried deep in the engine  will do no harm. Of course if it’s not a farm boy and instead part of a moon rocket for NASA then more accurate options are available as described by others.

[JasonBModerator @jasonb]

The heads for the cap head screws are hidden under the cylinder head so does not really matter if the hole has wandered at that end either. They don’t hold the head down.

Saves having to buy a length of 3.5mm silver steel and sharpen/harden/temper it if you start both sets of holes where they meet.

[Speedy Builder5Participant @speedybuilder5]

Yes, FarmBoy.  The drawings are in decimalised fractions of an inch which gives some some funny dimensions as to the rounding to nearest 0.001″

Bob

[not done it yetParticipant @notdoneityet]

Can you possibly drill larger from both ends and bush the ends to size?  The middle parts being perfectly in line is not such an important requirement like that and can be over-sized by a tad….

[Speedy Builder5Participant @speedybuilder5]

NDY, If it all goes a little astray, that may be an option.

[DalboyParticipant @dalboy]

When I did mine I drilled from both ends after drilling and boring the main cylinder bore but before shaping the outside. I just started with a block the correct size for the part.

It worked for me any slight deviation was easily sorted by running the drill bit from both ends, so no step was left in the middle. I used the pecking method to help prevent the bit from wandering too far off course.

Drilling and counter sinking for the heads

 

The outside shaped

[Author]

Posts