How to drill VERY accurate holes?

[Sperstad]

Hello people

Since I`ve got my IH mill, I`ve been doing some hole drilling in regular steel. But on some of the parts I`ve drilled, the hole need to be VERY accurate. Before I drill the hole I use a metal scriber to mark where I want the hole. But when I drill the hole with regular HSS drill bit, the hole often gets 1mm of center (where I made the mark with the scriber).

So the question is, how do I make VERY accurate holes with my mill? Do I have to use some other cutting tools?

[SBC Cycle]

Accurate location wise or hole size?

Use a center drill first, always. I have a few drills that are stout enough to punch a hole in steel without walking but my machine is also very rigid. Center drill just deep enough to get a small chamfer at the top of the pilot hole, then follow through with the drill.

If you are concerned about size you should take into account that most drills will drill slightly oversize. Look up some drill charts on the web and some of them will tell you the probable amount of oversize. If it really needs to be VERY accurate, drill the hole slightly under, then finish with a reamer.

Not sure of your application and would like to hear some other folks input but that's the way it's done here.

[M250cnc]

Sorry, but there is no way to drill holes "Very Accurately "

If you need accurate holes they need to be drilled, then bored to size.

If you need super accurate then they can be ground to size, using a jig grinder.

Phil

[Sperstad]

Thanks guys.

I meant accurate location wise. It don`t need to be extremely accurate, like 1/10mm in tolerance. So I think i will try to drill with a center drill bit first. I will buy some center drill bits and try that method.

But what about end mills, I guess there are some types of these that I can drill holes with? That way I only had to do one step to make the hole. What do you think about that?

[M250cnc]

You will not get very accurate holes with end mills

First they have to be designed for plunging.

Second unless your machine is very rigid the X & Y will get thrown around when you try to plunge. It will do this on a Bridgeport.

They "Endmills" will also drill slower than a drill if no pilot is used.

You can of course use an endmill after rough drilling to clean the holes up.

Phil

[mactec54]

Hi Sperstad

You want to use a spot drill not a centre drill, a centre drill will work but is not needed for drilling holes a spot drill is all you need

You can get a drill, mill, chamfer cutter combo, but this depends on the size you want to drill, there is not many sizes to choose from

[Karl_T]

Originally Posted by mactec54 Hi Sperstad You want to use a spot drill not a centre drill, a centre drill will work but is not needed for drilling holes a spot drill is all you need

He's right, spots are WAY better than center drills. For one step drilling a stub length spot drill in a collet or end mill holder (as opposed to a drill chuck) does very accurate work.

Karl

[Geof]

Have a look at this link:

http://hassaysavagecompany.thomasnet...ls?plpver=1001

You need a spotting drill, 90 degree if you want to spot the hole slightly oversize and leave a small chamfer after the drill hase gone in; 120 degree if you do not need the chamfer. In both cases larger than the largest hole you will be drilling.

Center drills are intended for drilling holes in the ends of shafts to turn them between centers on a lathe; these have the reduced diameter pilot and then a 60 degree taper section. You will find them described as 'combined drill and countersink' which is a nonsense name because they are neither.

You can use a center drill for spotting a hole but it is not the best choice, if you are following it with a carbide drill it is a bad choice. The pilot on a center drill has a fairly wide web for its diameter and in a drill press with some looseness this web can wander a little as it contacts the material so the alignment may not be ideal. Also the pilot is small and if it is used to simply make a small dimple this may not give good centering for a considerably larger diameter drill; which is why you will see it suggested that the center drill is taken deep enough to enlarge the hole on the 60 degree taper. This is a bad idea for two reasons: First, because you have a pilot hole the web of the final drill does not make contact with the material before it starts cutting full diameter so it does not get a self-centering and stabilizing effect; this means the drill can, and often will, chatter and wobble at the start of the hole giving a rough and tapered entry. Second, when a carbide drill is used this chatter will almost certainly chip the cutting edge leading to premature failure of the drill; it will also cause premature failure with HSS or cobalt drills but maybe not as quickly as with carbide.

Spotting drills are made for spotting holes to give a precise starting location for a drill. The web on a spotting drill is thinner than than that on a center drill pilot of the same diameter and the end clearance is reduced so a spotting drill has some tendency to self center. Spotting drills have no flank clearance and are not intended to go deeper that the angle on the tip which is why a diameter slightly larger than the intended hole size should be used so the spotting can be done to a diameter close to or slightly larger than the final hole. This shallow depth for the spotting drill means that the web on the final drill makes contact with material almost immediately and definitely before the drill is cutting at full diameter giving a much cleaner entry. When a 120 degree spotting drill is used a normal 118 degree drill makes contact on the web before the entire cutting edge is engaged giving the smoothest start possible and this is preferred for carbide drills. When a 90 degree spotting drill is used to spot deep enough to leave a chamfer then the corners of the cutting edge on the drill make contact with the spotted hole before the web makes contact. This can cause a little chatter before the web makes contact and is not good practice with carbide drills as it can cause chipping and premature failure; HSS and cobalt drills are more resist to chipping but slightly shorter drill life can be expected.

[BobWarfield]

What they said, but some other thoughts:

Definitely go spotting rather than center drill. I like to use stub length and larger diameters. You can only cut with the tapered point, so the hole has no idea the diameter and a larger diameter is more rigid.

Use a screw machine length twist drill. The shorter your twist drill the stiffer it is. If you need a really long length for a deep hole or to reach into a tight space, consider carbide. It is stiffer. You can go deeper just like with a solid carbide boring bar.

It's really painful to accurately locate center punched holes. I prefer to edge find some feature and let the CNC find the holes relative to that feature.

Make sure your drills are SHARP. It's amazing what a difference that will make. Also, based on the material, different end geometries can make a difference. Depends on your application whether it would be worth your trouble. Even just having a cheap Drill Doctor to keep the points sharp really helps.

Cheers,

BW

[Delw]

Originally Posted by Sperstad Thanks guys. I meant accurate location wise. It don`t need to be extremely accurate, like 1/10mm in tolerance. So I think i will try to drill with a center drill bit first. I will buy some center drill bits and try that method. But what about end mills, I guess there are some types of these that I can drill holes with? That way I only had to do one step to make the hole. What do you think about that?

for accurate location wise use a dial indicator.

[MrWild]

Times are achanging. I'm an old fart. Retired before some of the new stuff came in. (some? a lot of stuff) We used center drills for all important hole locations. Forthe most part they work well. A hobbyist with a full index of drills needs an inexpensive way to spot them with accuracy. Center drills do this quite well. I see now in the 21st century there is a better way, but the old way worked well enough that I don't think someone on a hobby budget actually needs a full set of spot drills, and a drill index.

Lots of reasons were given why center drills are a bad choice, but they will hold your hole within +-.002. If you need more precise than that, by all means, buy a set of spot drills. If the holes are merely for bolt clearance or tapped holes, a set of spot drills is a waste of money when a simple center drill will cover a wide range of drill sizes.

[irving2008]

How are you centering your spindle over the markings?

Its all very well having the debate of spot v centre drills (and I use both, but favour centre drills simply because I have several and they are cheap to replace), but the iisue seem to me to be that you are eyeballing the drill tip to the marking... before using a centre drill you still need to get the spindle accurately centred over where the hole needs to be... and for that you need a wiggler, or an edge finder if you can locate the hole relative to two perpendicular edges... unless of course you are relying on a DRO but then you wouldnt really need a mark, you'd just dial in the location...