G-Wizard Calculator:
Fast, Easy, Reliable Feeds and Speeds


Join 100,000+ CNC'ers!  Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:

  • Our Big List of over 200 CNC Tips and Techniques
  • Our Free GCode Programming Basics Course
  • And more!


GCode is Complicated
G-Wizard Makes it Easy

When to Use a Spot Drill + 7 Useful Tips and Techniques

Feb 27, 2017   //   by Bob Warfield   //   Beginner, Blog, FeedsSpeeds, Techniques  //  21 Comments

Spot Drill

Machinists are familiar with spot drills–they’re stub length and have little or no flutes.  These little drills are designed to be extremely rigid so that they can precisely spot a hole for a twist drill.  Maximum meat in the shank keeps them on target.  The goal is use the spot drill to make a little dimple in the workpiece that keeps the twist drill from walking so that the hole winds up in the right place.

When Must I Use a Spot Drill?

Is a spot drill necessary every time an accurate hole is to be drilled?  It’s purpose is to ensure the hole is accurately located.  The short spot drill is very rigid, and the spotting motion is unlikely to deflect.

However, if you use a carbide drill, or a screw machine length drill, spotting is typically not needed.  The carbide itself is so rigid compared to HSS that the drill will go where it is pointed.  As a matter of fact, most manufacturers recommend against spotting either a carbide twist drill or an insertable drill because its easy to chip the carbide in the dimple.  Screw machine length twist drills are much shorter, so they’re less likely to flex as well.  In general, you’ll save a lot of time if you can avoid spot drilling.  Investing in a set of screw machine length twist drills is well worth it.  I hardly ever use the jobber length bits.

screw machine vs jobber length twist drills

Screw machine-length twist drills are shorter and more rigid than jobber length.  They don’t need to be spot drilled.

There are times when you won’t be able to avoid a jobber length drill because the hole is too deep for a screw machine drill.  In that case, you could spot drill to start the twist drill, or you could drill the shallow part of the hole with a screw machine length and then switch to the longer drill.  Either way you’re facing a tool change, so it’s six of one and half a dozen of the other.

Can I Use a Center Drill Instead of a Spot Drill?

A lot of machinists use center drills for spotting instead of true spotting drills.  Center drills are intended to be used to create a hole suitable for a lathe center.  They have a 2 part tip that has a small pilot as well as the larger countersinking area of the bit.  While center drills are available more cheaply than spot drills, they have some disadvantages.  The small pilot tip is very delicate for example, and if it breaks, the drill will quit cutting.  Not a happy thing if you’re running a job that involves spotting a lot of holes.  Another problem is the hole angle of a center drill is typically 60 degrees.  When spotting, you want an angle that is larger than the twist drill’s angle if possible.  The narrower the spot angle, the more near the outside diameter of the twist drill first contact will be.  If the twist drill’s flutes aren’t perfectly sharpened, one will contact the spot hole before the other and the drill will try to deflect.  This defeats the purpose of spot drilling and can result in a less accurate hole.  The broader angle of a true spot drill means the tip of the twist drill cuts first, which makes for a more accurate hole.  Lastly, the web of a spot drill is typically thinner than a center drill, so it cuts more easily and with less heat.

Spot drill (top) is a better choice than a Center drill (bottom)…

Should I Use a Drill Chuck or Collet Chuck?

The choice of whether to use a Drill Chuck or Collet Chuck for a Spot Drill or any other Twist Drill is a divided one, because we’re optimizing two parameters and there is a different choice for each.

For best accuracy, use a collet chuck for your spot drill and twist drills.  Traditional drill chucks are less accurate and setscrew endmill holders are worse.

However, for holding power, the drill chuck is the winner.  Here’s why:

  • The Drill chuck concentrates its grip in 3 places.  That grip is so powerful, it often marrs the shank of the twist drill if the metal isn’t hard enough to resist.  A Collet, by contrast, spreads the force evenly 360 degrees around the shank.  You can easily see why that leads to less grip.
  • The internal workings of drill chucks use wedges to create significant mechanical advantage when tightened.  This leads to a lot more gripping force than a collet achieves.

In the end, I recommend using the collets for smaller drills, say 1/4″ and under, and the drill chucks for larger diameters that need more holding power.

Collet vs Drill Chuck

Spot Drill Tips and Techniques

  • When you spot the hole, let the spot drill dwell briefly at the bottom of the hole to ensure a smooth surface for the twist drill.  G82 is typically a better cycle to use than G81 for that reason.
  • Have you noticed the similarity in shape between a chamfer tool and a spot drill?

Chamfer tools…

Well, you can chamfer just fine with a spot drill.  Give it a try, it might save you a slot in your toolchanger.

  • While we’re on the subject of what else you can do with a Spot Drill, try counterboring for flat head cap screws.

    Rather than spot drill, drill, and then countersink, let’s kill 2 birds with one stone. The one fly in the ointment is that the countersink spec for US flat head cap screws calls for an 82 degree countersink, whereas spot drills are most commonly 90 degrees. This immediately led me to produce the following little chart that lays it all out:

    First we have the size of the bolt, followed by the expected diameter of the head according to a manufacturer on the web. We can apply a little bit of geometery and realize that for a 90 degree angle, the cone of the cap screw is the hypoteneuse of a right isosceles triangle and 1/2 the head diameter is therefore the depth. Now a little trig and we can figure the error between the 82 degree countersink and our 90 degree spot drill’s countersinking. As you can see, it isn’t miniscule, but I doubt it is the end of the world either.

    Note that 82 degree spotting drills are also available, though in fewer sizes. They will be spot on with no error (sorry for the pun!). As far as I can see with a quick check, 82 degree and 90 degree spotting drills cost the same. You will have to buy a pretty good sized diameter spotting drill given that you need one at least equal to the head diameter of the flat head cap screw you end to spot and countersink with it. A 3/4″ diameter spotting drill is only good for 5/16″ and smaller screws. These spotting drills are not cheap, and cost about 2x what a countersink does, so you’d better be able to justify that with the time savings. I think I would learn to sharpen drill bits in short order if I was planning on doing very much of it.

  • So, we can spot drill, counterbore, and chamfer.  But guess what, there’s more!  You can also use your spot drill as a V-Bit engraver too!

Check out this video of a Nine9 NC Indexable Spot Drill spotting, chamfering, and more:

  • All bets are off when micromachining.  You can increase tool life considerably if you spot drill a dimple 5% larger than the micro-drill’s diameter.
  • If you’re going to do all these cool tricks with a spot drill, you’re going to need to do some geometry calculations.  Fear not, our G-Wizard Calculator has some awesome tools to help:

spot drill geometry calculator

Calculating depths versus diameters for various sizes…

The Calculator covers spot drills, center drills, counter bores, and more.  Plus, there’s even a database of fastener counterbore sizes:

flat head cap screw dimensions

Now here’s what’s even more awesome–you get these useful Calculators and a whole lot more entirely free and for life just by signing up for our free 30-day trial.  That’s right–those features go right on working when the trial ends.  Cool beans!

Sign up today:


For more Twist Drill Techniques, check out our Twist Drill Tips Page.


Like what you read on CNCCookbook?

Join 100,000+ CNC'ers!  Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:

  • Our Big List of over 200 CNC Tips and Techniques
  • Our Free GCode Programming Basics Course
  • And more!

Just enter your name and email address below:

Full Name
Email *
100% Privacy: We will never Spam you!

When to Use a Spot Drill + 7 Useful Tips and Techniques
4.8 (96%) 5 votes


  • Hi Bob,

    Great article. Maybe it’s because machining is only a hobby for me or because I’m from Denmark and there are some technical english I don’t quite understand, but could you explain more about the difference between a screw machine drill and a jobber length drill? Because I have no idea which category my drills belongs to. Maybe you could give an example. Like what is the typical length of a 10mm screw machine drill compared to the jobber drill?


  • Martin, thanks for commenting.

    Jobber length drills are the most common size. According to Wikipedia, they range from 9 to 14 times the diameter in length.

    Screw machine length drills, also called stub-length, are much shorter. Instead of 90 – 140 mm, a screw machine length 10mm twist drill should be 84mm according to my catalog.



  • Hello guys, I can add my 10 cents worth, gleaned over a 52 year career in toolmaking, and aircraft engineering. The widespread use for ??hundreds of years LoL! of the poor mistreated center drill, is fundamentally wrong, and as stated above, the smaller ones are fragile!

    The small pilot section is purely to give free space for the point of a standard lathe center, be it Live (revolving) or fixed dead center. For a lot of work, a nice little live center is miles ahead.

    When precision grinding it is normal to go with a dead center, and I have used that nasaty old White Lead, mixed with a little oil, as the lubricant.

    I digress, The concept of Spot Drills is a very good idea, as is the use of the short Stub length drills. Look in Machinery’s Handbook applied mechanics section, and see the formulas for deflection of a column. A twist drill, which is much weaker than a solid rod, be it HSS or Carbide, is relatively unstable because of those boring old laws of Physics!

    There is a lot of disagreement as to point angles; some manufacturers use I think around 90 degrees. Others match the angle to the following drill. There are many favoured angles for differewnt materials, but honestly, the good old 118 is a pretty good all rounder, especially for jobbing work or short runs. A most important thing is to pointr thin or web thin to get rid of that useless chisel edge, which really only flows the metal, it does not CUT. A very useful point is the Split point, where the web no longer exists, and becomes a secondary set of cutting edges. OK I am rather spoilt, and about 35 years ago, invested in a Swiss Christen precision drill and tool grinder, which with much tweaking, grinds what we need, a geometrically equal anbd opposite point, with the sams clearance angles. I know, most of you can hand grind any drill freehand, perfectly!!! REALLY? OK tro do in a rush, but I gave up long ago. I realise it is not feasible to have a special machine in t65he home shop, although there are several on the market.

    There are a few saving graces however! If you use ER series collets, you are on a winner, they are truly fabulous./ Particularly in a Milling machine. I can assure you that I have never overly liked Jobber length drills; they are too long for most applications. The stub length drills are worth acquiring a number of, as you do not need to spot drill , just save time by using these for most work. They are also available in split point. If you haven’t tried these, you are in for a very happy surprise. I havew been doing moderate runs of components for trhe last thirty three years with CNC.

    I retrofitted my Bridgeport with a Bandit control, and Ground thread ball screws and Stepoper motors on X and Y axes only. I left the quill or Z axis manual, and it worked out brilliantly for what I was doing. Three years later we added a Shizouka with a Servo motor Bandit control three axis and 40 NMTB taper with Bristol Erickson Quick change spindle nose nut.Yes, manual tool changes, but if planning is properly done, it is amazing how much work can be processed, when running these two low level machines!

    I was having trouble with the Z axis length of a twist drill in my preffered Albrecht drill chucks. These are4 fantastic. The answer to this was to adopt a couple of ER 32 chuck bodies and a few collets! I wanted to try out a logical idea, which is to grip the drill by the flutes, so we have a short overall length, and a far stiffer drill because of the much better L/D ratio. This works out beautifully, in practice, occasionally the oddbit of swarf will get tangled in the collet slot, but usuall no problems at all. These chucks are really quite excellent for holding slot drills, end mills, and drills. They are ava8i9lable with a dead stop screw in back of holder.

    I can also say happily, that after the two Dearly loved Bandits went to God, and spares not available, I had to go big time and buy a Vertical nMaching center with BT-40 tooling, 10,000 RPM spindle one tonne capacity and one meter in X. and 24 tool magazine. I cannot claim to be madly in love with the Fanuc control, itr really is a headache compared to the Bandits!

    However the ten k spindle is fabulous and almost silent with 11KVA driving it. I have purchased a number of ER collet chucks and sets of collets. They may not be the answer for High speed machining, but that is a field to be very wary of, it is costly in overheads and maintenance, and a spindle may only last for a couple of years. I think for the larger shops.

    Another tip for drilling brass, particularly sheet or thin sections. A normal drill will grab savagely, and rip through it, often causing damage! Be very careful here, the hands will always lose the fight, sometimes catastrophically! The way to tame the drill, is to take a slip stone say triangular, fine grit, and stone a thin flat on the cutting edge parallel to the axial length, or even a degree or three negative. Only about 0.005 inch is nee4ded, and the top rake disappears and the drill behaves! It is a good idea to keep a few commonly used sizes in a tin just for Brass.

    A few words on myself. noiw a one man shop, with a long involvement in Aircraft Engineering, tool andd gauge making, general jobbing work for a diverse range of customers. My personal interests run to Model Engineering (wonder when I will get time to build a couple of radial engines, and a 5 inch gauge Steam loco? And long term Ham Radio. ( VK2-TQ ).

    Remember that one often needs to improvise and persevere with tooling that is far from ideal. No point in spending lots when doing a handful of components, but well worth while when doing a larger quantity.

    I hope a few thoughts have provided some help to a few of you guys. A small toolroom is very similar to the Home Shop Machinist at the end of the day!

    So, greetings from the Colonies

    • Stephen, I am a hobby jack of all trades, I am now making up a duplicating machine. I got all the steel component plasma cut and baulked at having the holes laser cut because I was not aware laser could now cut 20 mm plate and the plasma is too inaccurate anyway These bars form a parrellogram and in all take 12 x 47 mm bearings. The holes for these bearings and shaft holes have no tolerance they must be exact. I had originally planned to weld all the parts together and drill the holes in one pass but then again I am not so sure that the drill will cut true and not wander. I may start on the mark and find that the drill deviates as it passes through seperate layers. If I go down this track do I start with a spotter drill and use a series of spotter drills with the same angle until I get a fairly large start center for the 46.5 mm drill I have. I can find nothing on the web or in fitting and machining book
      Cheers Vaughn Gunthorpe

      • I know this wasn’t directed to me, but I’ll throw in my two cents worth anyway. Drilling these holes sounds like an expensive proposition. I don’t see a lot of 47mm (or slightly undersized) drills floating around out there. Not to mention for a really good fit you’d also need an appropriately sized reamer. Assuming you have (or have access to) a mill, a boring head would probably be no more expensive, and provide a lifetime of very high quality custom sized holes.

  • Hi Bob,

    Thanks for the answer. Mine 10mm split tip drill is 132mm so it must be the jobber type. When I go to my professional tool shop and ask for a spot tool, they just look funny at me and hand me a center drill. And they sell tools to many machinists.
    Next time I will ask for a stub-length drill.

    Another question. How deep should the spotted hole be?

    • Martin, make the hole just deep enough so its diameter is just shy of the hole diameter. Use G-Wizard’s geometry calculator to figure out how deep that is.

      I like to use a 1/2″ spot drill and use it to spot a variety of hole sizes. You’re just looking to create enough of a pocket to guide the tip of the twist drill.

      You can mail order a spot drill. Get 2 or 3 and they’ll last a long time. I have a carbide spot drill around here somewhere that I bought for tougher materials, but I seldom use it.



    • Hi Martin, what you need is a NC-bor in danish, NC-spot drill, call me and i will send you a picture of different types. 40787875.

  • Assuming your spotting drill is actually a broader angle than your twist drill, is there any reason not to go a bit deeper to produce a kind of pre-chamfer for your hole?

  • Hi

    If you are drilling a large quantity of holes that don’t require a CSK or custom chamfers you can eliminate the need for spot drilling by using special geometry 3 flute drills made by Titex or Fenn tools.

    These drills will save you many hours of production time on large batch sizes.


  • Hi

    Forgot to add. Never discount custom tooling. Many companies supplying quotes to BAe Systems didn’t get the contracts because other competitors reduced the number of ops required.

  • […] also CncCookBook – When to use a spot drillCromwell Industrial is the only supplier I’ve found that sells spotting drills, these are […]

  • […]  Pilot holes can help for large holes.  For accuracy, you may want to “Spot Drill.”  This article tells when and if you’ll need to spot drill.  You’ll need a special “Spot Drill” cutter to perform the spot drilling.  Some […]

  • Hi Bob,

    I purchased some cobalt twist drill bits and was wondering whether they suffer from the same problem as carbide i.e. do they chip if I use pilot holes or is it safe to drill a small guide hole? I’ve got some steel that I need to cut a pocket in and the object is too big to fit into my CNC machine so I’m planning on doing it the old fashioned way with lots of holes and then finish it off with a file.



    • Dmitry, cobalt will behave just like HSS.



  • We’ve been using the Nine9 brand of index-able Chamfer/spot drilling tools for a couple years now (everything from a 6mm diameter cutting edge up to a dia. 22mm).
    Very productive tool in tough work environments.

  • All good information though I assume we are only talking about drilling perpendicular to flat surfaces. I found the large spotter angles recommended here not so perfect for drilling intosmall shafts and tubes, as the chamfer is very elliptical leading to an interrupted cut that shakes to drill on entry. In this case the small pilot of a center drill tip while avoiding the 60deg countersink does work well at stabilising the drill. Using the shortest possible length drill is more critical in this scenario than perpendicular surfaces. Now going off centerline brings up even more challenges for deflection.

  • On the question of drill chucks vs collets.

    I avoid Jacobs chucks for carbide drills as they cannot bite into them, so the fingers of the chuck tend to flow and warp and permanently lose accuracy and grip quite quickly. Never use them for drill-mills or anywhere side forces are found.

    With collets, try to buy twist drills that are laser engraved not punched or at least stone off the raised letters and numbers. Collet grip is enhanced by managing the friction. Clean the collet and tool with a no film degreaser like Windex. Clean the holder and nut with a lubricant like WD-40 spray. Once a collet chuck is loosened assume grit has travelled from the slots to the tapers. Never re-tighten without cleaning. Seen lots of hastily assembled collet holders slip but not once when using this cleaning protocol.

    For pure downward thrust, the chuck is always the quickest setup option.

    Hazards: CNC keyless chucks have double or more grip than Jacobs keyed chucks or mechanical collets but the grip lines make the HSS drill unsuitable for collets in the future. Remember that HSS drills are very slightly back tapered making the shafts smaller than the tip, thus they fit loose in end mill holders resulting in oversize holes.

  • Hi BW,

    I’m just getting into hobby woodworking and I’m still building my arsenal of tools. Might be a silly question, but since you mentioned you can CSink with a Spot Drill, what stops me from spotting with a CSink?


    • Nothing, in principle. The cutters have similar geoemetry. The main thing is the included angle for a spot drill. Keep the angle larger than the twist drill’s angle for best results.

    • Another consideration is the tip. Not all counter-sinks cut at the center.

Leave a comment


Do you want to be a better CNC'er in 37 Seconds?

Get Better Tool Life, Surface Finish, and Material Removal Rates Fast.

It's that easy. You can install and get results in a matter of minutes.


Start Now, It's Free!



  GW Calculator

  GW Editor



  Deals and Steals

CNC Blog








     Feeds and Speeds

     G-Code Tutorial

     CNC Machining & Manufacturing

     DIY CNC Cookbook

     CNC Dictionary

CNC Projects


     Machinist's Search


     Online Groups


     Reference Data


     CNC Dictionary


     Tool Brands


     Hall of Fame

     Organization: Soon!





     Our History

     Privacy Policy

All material © 2016, CNCCookbook, Inc.