Cutting really straight holes?

mikey said:
It's always wise to really think things through, especially the first time you do something or when the project is a long time in the making. You did fine; discovering you screwed up after you screw up is not that much fun.

I wanted to tell you that when you need a hole to be fairly straight (drills only make fairly straight holes), try not to use a pilot drill unless the drill is large, like over 5/8". Pilot drills are properly sized when their diameters just span the web of the main drill. Hence, they are sort of bendy and flimsy so when drilling pressure is high enough they will wander. Accordingly, the main drill that follows will also wander. Using the main drill alone requires more pressure but if you pay attention you will see and feel it cutting. I tend to prefer a little less speed and a little more feed pressure to keep the drill cutting continuously. It produces less heat, less wandering and more accurate holes.

Remember too that reamers will follow the pre-reamer hole. If the pre-reamer hole bends, the reamer will bend to follow it. If you need a hole that is accurate and straight, bore it. Reamers are best used when a good finish is required. Ideally, they also produce accurate holes but only if the proper pre-reamer drill is used and the reamer is sized correctly for the material and the hardness of that material. I have a lot of reamers but often find that I don't have the exact size I want so I learned to bore accurately.

There is a lot more to making holes than you might think. You asked the right question, Trav.
Click to expand...
The cure for reamer wandering, which is due to the chamfer on the end of the reamer is to use jig bore reamers; they look like an end mill and cut on the flat end, and they do not have OD clearance like an end mill.
 
Spot, drill, then ream to size.
This is about the most common operation that you will ever perform in a machine shop. Buy a spotting drill, a twist drill slightly smaller then the finished size and a chucking reamer of the desired size.
There is no magic involved, this is done millions of times per day in shops world wide. If the machine you are doing it with is inconsistent then you will need another machine but the tooling is simple and easy to use, also inexpensive as far as tooling goes. If the part has features that you have failed to mention such as internal grooves, back spot facing and internal under cuts the tooling costs will increase considerably.
 
For an accurate sized hole, with a nice finish, in the location you want it, understand the following:

A drill is for removing bulk material. It does not make a hole to an accurate size, in the location you want it, or to a nice surface finish.

A boring bar is for making holes in an accurate location. It is quite possible to use a boring bar to make a hole to an accurate diameter, but it is not necessarily easy. However, machinists use jig bore machines to make extremely accurate holes of the desired diameter in the desired location. Takes skill and a jig borer or similar. A boring bar is not usually used for starting holes or for hogging out material.

A reamer will finish a hole to a pretty accurate size, there is some operator skill necessary for trying to hit a diameter within a couple tenth thousandths on demand, but it is fairly easy to hit a diameter within .0005" with a reamer. A reamer does not start holes, does not remove bulk material, and does not establish the position of holes.

A regularly used process for making pretty accurate holes, in the desired location, with the correct diameter, and with a good bore finish, repeatably, is by:

1. Spotting a hole with a spotting drill.
2. Removing bulk material with a drill.
3. Boring the hole to establish the correct location.
4. Reaming to establish the finish bore size and surface finish.
Chamfering the hole is optional, but common, usually done as part of step 1, or after step 2 or step 3.

I was describing the process for doing accurate and repeatable work, with a high rate of success. Most work does not need to be anywhere near this fussy. Sometimes, most times in my case, I just want to punch a hole in a part. My purpose in presenting this is to show the advantages and disadvantages of the various hole making tools, and how they interact so each step of the process provides each tool's strengths and avoids each tool's shortcomings.
 
Like cutting an item to the correct diameter on a lathe, a boring head+bar setup will change the hole diameter by twice the offset of the boring head. The dial on my boring head sort of alludes to this, yours may not.

To (hopefully) silence some quibblers out there, I am referring to the actual offset change. Some lathe cross slide dials are graduated in terms of diameter change, some aren't (mine isn't); and I suspect boring heads are the same way. Could get even more interesting if you've got both instances in your shop. Fortunately for me, my lathe and boring head use the same convention so I don't have to worry about it.
 
homebrewed said:
Like cutting an item to the correct diameter on a lathe, a boring head+bar setup will change the hole diameter by twice the offset of the boring head. The dial on my boring head sort of alludes to this, yours may not.

To (hopefully) silence some quibblers out there, I am referring to the actual offset change. Some lathe cross slide dials are graduated in terms of diameter change, some aren't (mine isn't); and I suspect boring heads are the same way. Could get even more interesting if you've got both instances in your shop. Fortunately for me, my lathe and boring head use the same convention so I don't have to worry about it.
Click to expand...


Something to be aware of for sure. Both my lathe and boring head are graduated in diameter change. But there are a lot of tools out there that read the movement amount directly, so you get radius change for circular work. You have to know your tools. And, ideally, all your tools use the same convention. :)
 
This made me smile. I've been using a Sherline lathe for about 30 years and the dial is calibrated for cuts on the radius, or half the diameter. My Emco lathe is the opposite; it is calibrated for cuts off the diameter. The Criterion boring heads I have are calibrated for cuts off the diameter, too.

I cannot tell you how long it took for my old fart brain to adjust to the machine or tool in use. When I first got my Emco lathe I took a cut, measured and had this stupid(er) look on my face - WTH, I know I dialed in that cut and its still too big! Embarrassing but I did it again and got half the result I expected. THEN it dawned on me that the Austrians had calibrated the dial "wrong". So yeah, you gotta' know your tools!
 
And to think I was just going to drill holes with drill bits for my plinth project and call it good. :grin:
 
You must log in or register to reply here.
Back
Top