By continuing to use this site, you agree to our use of cookies. Find out more
Forum sponsored by:
Forum sponsored by Forum House Ad Zone

Drilling deep holes - 10x drill diameter - Runout?

All Topics | Latest Posts

Search for:  in Thread Title in  
Steve Withnell30/10/2011 18:07:13
843 forum posts
222 photos
I need to drill an accurate hole in HE30 finished out with a 7/32 reamer. As a test run I set a piece of HE30 bar to truth in the four jaw, drilled a 3mm pilot hole with a new long series drill, keeping each "peck" less than the diameter of the drill. I brushed paraffin with a toothbrush to keep the flutes clean at each peck. Once I had a through hole, I repeated the drilling process with a 5.5mm drill and finished off with a new 7/32 reamer. I was running the lathe a little over 2000rpm for the drilling and very slow for reaming.
The hole in the practice piece is 75mm deep.
Then I removed the test piece from the chuck and re-set it so the exit wound was facing the tail stock. Having set the workpiece to truth on the OD, I then used the DTI to measure the runout, by running the DTI in the ID. - slightly less than 0.2mm TIR.
I checked the tailstock aligment and as best as I can measure, it's better than 0.05mm over the distance (ie not perpendicular off-axis distance at the tailstock).
It struck me that I don't know if 0.2mm is good, bad or indifferent for a properly set up chinese lathe! Any thoughts welcome.
If the DTI is reporting 0.2mm TIR, does that mean the drill only wandered 0.1mm?
What can I do to halve the error?
Regards Steve
Ramon Wilson30/10/2011 18:27:41
1319 forum posts
382 photos
Hi Steve,
To me you are approaching the job correctly but the hole will only run as true as that first pilot hole - any subsequent drill and the reamer having a tendency to 'follow' the previous hole. As your first hole is quite small despite your care in pecking it's this that is probably deviating rather than any error in your set up.
Are you drilling that first hole with a normal drill before changing to the long series?
If you are able to accurately turn the job round you may be better off drilling the initial hole from both ends, it's surprising how accurate that can be providing the holding is true.
Failing that I would try using a larger drill for the initial hole and if possible before opening to the reaming size run a long series end mill if you have one (or a D bit) down as deep as you can to true the hole to give you the best chance of guiding the reaming drill.
Hope that gives you something to work upon to improve the 0.1 deviation
Regards for now - Ramon
Clive Hartland30/10/2011 19:09:47
2820 forum posts
40 photos
My first thought is that your rpm at 2000 is very high! I would have done mine at about 400 rpm.
The 3mm drill even if slightly uneven lip length will wander even though you are pecking.
Alu being easy to cut will allow the drill to wander much easier than steel.
As Ramon mentioned, if you can drill from both ends and see what happens.
75mm is long for a 3mm drill and a more rigid type of tool may be better, perhaps again as suggested a 'D' bit drill.
I would think the weakest part of a helix drill is where the flutes end and the parallel shank starts, it wobbles from there.
I would also start with a stub drill up close to make sure of a good start.
Ramon Wilson30/10/2011 19:39:47
1319 forum posts
382 photos
Err - 400rpm Clive? Hate to disagree but that seems rather slow to me, particularly in aluminium.
Taking it at a cutting speed of 500 fpm gives roughly 17000rpm - for the 3mm drill, so Steve is actually well too slow but taking it too slow will probably lead to crowding of the drill and even more deviation. A conservative 250 fpm gives appx 8500rpm so 2000 is still well short of the accepted surface cutting speed. Obviously very few of us have kit that will do these kind of speedsso a compromise has to be made but I do think there's a greater likelyhood of deviation by going too slow.
The 5.5 drill seems very close to the reaming size too leaving only a couple of thou for reaming - I would have though 5.3 more the likely candidate running around a 1000 rpm.
My money's still on an initial 4 - 4.5 drilling then the reaming drill.
Regards - Ramon


Edited By Ramon Wilson on 30/10/2011 19:43:15

Clive Hartland30/10/2011 20:15:18
2820 forum posts
40 photos
I was going by what speeds I have on the lathe Ramon, I think my highest is only 820rpm.
I just find that at anything faster than 400rpm the WD40 smokes and it starts to run dry!
Stub Mandrel30/10/2011 20:38:23
4315 forum posts
291 photos
1 articles
Do you have a means of rotating the drill in the tailstock? If both work and drill rotate in opposite directions at about the same speed. any errors cancel out completely.
Andrew Johnston30/10/2011 20:39:02
6601 forum posts
701 photos
Right, flameproof overalls on; here are my thoughts!
If runout of the hole is critical I wouldn't use the lathe. I'd drill the hole in the vertical mill and then machine the rest of the part using said hole as the reference for set up. The problem with using the lathe is that it relies on the drill being perfectly aligned axially and dead parallel to the rotation axis of the headstock. The one thing you can gaurantee is that it won't be.
I agree with Ramon that the 5.5mm drill is too large, the reamer will be rubbing or not even cutting. I wouldn't bother with a pilot size drill, just go straight through with 5.3mm. Larger drills will tend to follow any 'wander' of smaller drills so why not start with the largest, and stiffest, drill. Less 'pecking' needed too. Also, keep the feedrate up, that minimises any errors due to slight asymmetries in the chip size.
I also think that 400rpm is a bit slow; I'd be up at about 2000rpm for drilling, and half the speed, twice the feed for reaming.
My sequence would be; start the hole with a carbide spot drill, drill through with 5.3mm, ream 7/32".
Here's a thought, you could consider a carbide drill; like for like carbide is much stiffer than HSS.
Chris Trice30/10/2011 20:39:30
1375 forum posts
10 photos
Starting with a stub drill is a good bet and then proceeding with a split point four facet drill. I've found the latter tend to self centre better than a regular jobber drill. I don't know why but they do, possibly because they require less pressure to cut. The other thing is to use a good quality drill that you trust to have been ground accurately. The problem with soft aluminium is it tends to clog the flutes which in turn scores inside the hole. Not the best formula for true running.
colin hawes31/10/2011 09:07:17
558 forum posts
18 photos
Using a slot drill to correct concentricity of the pilot hole will improve the chances of a larger drill to correct any initial inaccuracy as it will then be guided by it's diameter rather than it's point or pilot hole.
Richard Parsons31/10/2011 09:40:27
645 forum posts
33 photos

A 5.5 mm hole drilled 75mm deep. That is a job for a Nug drill (the spelling mistake is quite deliberate). There was a discussion a few months ago on this site about them. Even then the hole will not be true. It will tend to be a curve and this has to be straightened. This was done ‘by eye’ looking down the hole at a window with good daylight and bopping the thing with a mallet or in a press. This process was written up in ME in the past 2 years.

The drill its self had a flat at its business end with a diamond shaped cutting edge. It had a groove or a flat along its length to take the swaff. If you are peck drilling you can get away with without pumping oil down a separate channel, but a hypodermic syringe and a thin length of plastic pipe is a good idea. Use it to flush out the swaff. Hold the work piece so that all of it is between the chuck and the tailstock.

The second method is to rough drill a hole and then use a Greener tool. This is a shaft with a ‘V’ shaped tool with two cutting edges on one end. The shaft is threaded up the hole and held in the chuck. The other end of the thing you are machining is held in a gimble so that the tube can ‘flap about’ but not turn. Greener used a trunnion and chains for this. The cutter is rotated and the work piece is pulled slowly down the tool. Greener used weights for this purpose. Greener claimed it drilled a perfect hole. He would then machine the outside to size.

Ramon Wilson31/10/2011 11:10:50
1319 forum posts
382 photos
Hi Clive, yes understand perfectly - that's when you really have to compromise

One of the biggest advantages of the Super 7 over the 7 I guess but then I hardly ever changed up to top speed range - different now with the VFD though.
Steves gone quiet - has he drilled his hole successfully I wonder
Regards - Ramon
Steve Withnell31/10/2011 12:50:28
843 forum posts
222 photos
Just ordering some drills...
I've been pondering if I can actually reverse the workpiece accurately and I think it may be possible as the hole has a flat reference surface related to it. So I think the next test run will be to drill the hole on the mill, using a carbide drill. If that is still off, then I'll try another test piece and drill halfway and reverse the part. The mill will run upto 2500 (my lathe can beat that...) but the real part will have to be bolted to angle plate on the face plate, so the speed will be way less than that - the fixture is static on the mill, so I think that is where the machining should be done.
I will report back after the new carbide has arrived...
chris stephens31/10/2011 13:15:28
1049 forum posts
1 photos
Hi Guys,
For all you speed freaks, who think the books are right about drilling speeds, you might be surprised how slow you can drill. There is some merit in the thought that you should drill at speeds that allows the lips to cut and not just rub.

The Merry Miller31/10/2011 13:44:08
484 forum posts
97 photos

That's very true Chris, especially when using large hand operated ratchet drills (shades of the 1950's)
Len P.

Versaboss31/10/2011 16:13:12
490 forum posts
69 photos
Posted by Richard Parsons on 31/10/2011 09:40:27:

The second method is to rough drill a hole and then use a Greener tool. This is a shaft with a ‘V’ shaped tool with two cutting edges on one end. The shaft is threaded up the hole and held in the chuck. The other end of the thing you are machining is held in a gimble so that the tube can ‘flap about’ but not turn. Greener used a trunnion and chains for this. The cutter is rotated and the work piece is pulled slowly down the tool. Greener used weights for this purpose. Greener claimed it drilled a perfect hole. He would then machine the outside to size.


Dick, would it be possible to show a sketch of that Greener tool? I admit having trouble to visualizing this from your description. Google just brings up a lot of 'greener ways to drill for oil', not what we do here?

Greetings, Hansrudolf

Donald Wittmann31/10/2011 16:53:01
40 forum posts
Your drilling is maybe not at fault, The problem could well be that your chuck jaws are not holding the part true to the lathe bed. Even if you set the outer end to a couple of microns the inner end that projects to the rear of the chuck could well be off with the result that the hole [even if it is true] would be eccentric to the outer Ø.
So you should also check your chuck / chuck jaws.
Buffer05/02/2022 16:31:07
338 forum posts
153 photos

Hi All

I need to drill a 14mm hole 300mm deep right through a bar 60mm diameter of EN1A steel.

It doesn't need to be precisely on centre as I will probably turn between centres at the end.

I was going to hold it in the four jaw with the fixed steady and then drill and bore a hole to get the drill off to a good start. Then just go at it for the day with a HSS jobber drill and extend it when I need to. Has anyone done this sort of thing before and got any advice or top tips before I get to work? I was wondering about things like maybe drilling it a little under size and finishing with a D bit for example. The finish needs to be reasonably good but not brilliant.

Many Thanks.

Edited By Buffer on 05/02/2022 16:36:41

Andrew Johnston05/02/2022 16:57:25
6601 forum posts
701 photos

When I needed a 1/2" hole through 250mm of EN1A I centre drilled, started the hole with a 12mm stub drill, then a jobbers drill and finally an extra long jobbers drill. Lastly I reamed with a 1/2" long series reamer as I needed a good finish.


Buffer05/02/2022 17:35:35
338 forum posts
153 photos

Thanks Andrew. I presume this was in the lathe and not the mill as you suggested above? Did the drill stay centred ok at the other end? I guess it would do being a 1/2 inch.

Andrew Johnston05/02/2022 18:42:30
6601 forum posts
701 photos
Posted by Buffer on 05/02/2022 17:35:35:

...I presume this was in the lathe...

Correct, it was done on the lathe. My mill didn't have enough headroom. The part has a cover on the end with a short 1/2" spigot. The OD of both part and cover are stock size. I can just feel a slight ridge between the cover and part. So I guess the runout of the hole is around 0.1mm or so.


All Topics | Latest Posts

Please login to post a reply.

Magazine Locator

Want the latest issue of Model Engineer or Model Engineers' Workshop? Use our magazine locator links to find your nearest stockist!

Find Model Engineer & Model Engineers' Workshop

Support Our Partners
Eccentric Engineering
Rapid RC
Eccentric July 5 2018
Subscription Offer

Latest "For Sale" Ads
Latest "Wanted" Ads
Get In Touch!

Do you want to contact the Model Engineer and Model Engineers' Workshop team?

You can contact us by phone, mail or email about the magazines including becoming a contributor, submitting reader's letters or making queries about articles. You can also get in touch about this website, advertising or other general issues.

Click THIS LINK for full contact details.

For subscription issues please see THIS LINK.

Digital Back Issues

Social Media online

'Like' us on Facebook
Follow us on Facebook

Follow us on Twitter
 Twitter Logo

Pin us on Pinterest