First try at reaming a hole

Neo6 · Oct 21, 2014

Still in my quest to make the perfect hole, I end up buying a lathe Grizzly G0602 now I need to learn how to use it, just finished doing the break in now I am waiting for the oils from ENCO didn't know it need it specialized oil, is a pain to find Mobil Vactra No 2 and Mobil DTE Heavy/Medium where do you guys look for this stuff locally?
I want to make a 2.1mm hole with a smooth inside surface with no tool marks in stainless steel, the holes is straight through 27mm long.
On a past post some people gave me suggestions in how to do this, the first suggestion to try is going to be a reamer so I am guessing I drill the hole at 2mm and ream it at 2.1mm, sounds right?
here is my question should I use a floating reamer holder? Is this a must? If so what floating holder do you folks recommend? Also I know there is many different drill bits what type of drill bit do you folks think I should be using? And could you guys please give me suggestions in where to buy this items. Thank you.

egpace · Oct 21, 2014

Neo6 said:
Still in my quest to make the perfect hole, I end up buying a lathe Grizzly G0602 now I need to learn how to use it, just finished doing the break in now I am waiting for the oils from ENCO didn't know it need it specialized oil, is a pain to find Mobil Vactra No 2 and Mobil DTE Heavy/Medium where do you guys look for this stuff locally?
I want to make a 2.1mm hole with a smooth inside surface with no tool marks in stainless steel, the holes is straight through 27mm long.
On a past post some people gave me suggestions in how to do this, the first suggestion to try is going to be a reamer so I am guessing I drill the hole at 2mm and ream it at 2.1mm, sounds right?
here is my question should I use a floating reamer holder? Is this a must? If so what floating holder do you folks recommend? Also I know there is many different drill bits what type of drill bit do you folks think I should be using? And could you guys please give me suggestions in where to buy this items. Thank you.

If your tailstock is aligned you don't need to float it.

You can get almost anything on Amazon...

Amazon.com: Mobil Vactra No 2

PS ixnay on the izzlygray in your posts.

18my · Oct 21, 2014

Dunno about you guys but I find reaming finish to be crap. I always try and bore things where possible. Iscar make a picco bar that could do it from each end. Pico r/l 050.2-15. Sandvik/simtek also make similar tools. If reaming is a must I would put it in a floating holder and leave a minimum of 0.2 to 0.3 in diameter.

* edit Sorry should mention i use metric

tdmidget · Oct 22, 2014

18my said:
Dunno about you guys but I find reaming finish to be crap. I always try and bore things where possible. Iscar make a picco bar that could do it from each end. Pico r/l 050.2-15. Sandvik/simtek also make similar tools. If reaming is a must I would put it in a floating holder and leave a minimum of 0.2 to 0.3 in diameter.

Obviously you don't know how to ream. LEARN!. READ! This site is full of info . Use it.

Neo6, these oils are the most common in the machine tool industry. Get away from Autozone and such and learn what oils really are. The Oil companies have product and interchange charts that will give you a great insight into what is what in oils.

Neo6 · Oct 22, 2014

You guys never disappoint thank you, I already order the oils from ENCO as I mention before I was just curious what type of shop would carry those products I know an auto-part shop won't.
Thank you 18my for the Pico, that looks cool would I need a holder like this High Precision Finish Boring - BIG Kaiser what kind of holder would you use with that tool? Also as you mention it would need to be bored from both sides since it can't reach the entire length of the hole that makes it tedious I am trying to make it less complicated. Once more thank you for the help.

extropic · Oct 22, 2014

First of all, creating a STRAIGHT 2.1mm hole through 27mm of even the most machineable types of stainless steel is a non-trivial task in my opinion. But then, you didn't say it had to be straight, just smooth.

Next issue, I presume that the desired hole is in a piece of bar stock (very inexpensive) so trial and error is a non-problem.

Boring the hole from both ends of the part is a knuckle head suggestion for a newbe. You are very likely to end up with the two holes not being precisely aligned due to run out induced by rechucking the part. You haven't specified the finished hole diameter tolerance or surface finish (µinch or µm) requirement. Be that as it may, a reamed hole is an inexpensive operation (≈$10 for the reamer?) and should produce a hole of more consistent size and finer surface finish than drilling. Just put the reamer in the tailstock chuck, lube it and go for it. I'd run the reamer at the same RPM as the drill. What is the correct RPM for a 2.0mm drill in UNKNOWN type of stainless? Look it up.

If you're not satisfied with the results of a reamed hole, there are many other options available but drill and ream first. Experience is a great teacher (if you're paying attention).

powderhorn · Oct 22, 2014

It would help if you would put in the city/area that you are in, instead of USA. Check your phone book for machinery suppliers, industrial supplys, or your tool dealer. Give them a call and ask questions. here in southern Nevada, we have one store as a supply source.

Garwood · Oct 22, 2014

I run reamers in decent collets and run them a bit slower than a twist drill with 50% or so more feedrate. I found the cheap import reamers aren't usually made very good and buy quality name brand ones when the job is important.

I ream a lot of .375 drilled holes to .3930" 1.27" deep and run 300 RPM and 5 IPM in 6061 for a good, predictable size and finish. It could probably be done faster, but that's what I've had work fine for several years now.

Neo6 · Oct 22, 2014

Thank you gentleman, you are all awesome. I will stick with drill and ream first, I will get some supplies and give it a try.
Powderhorn, I am in Southern Nevada too, are you talking about Mcfadden Dale hardware? Or do you have another go to store for your supplies?

18my · Oct 22, 2014

tdmidget said:
Obviously you don't know how to ream. LEARN!. READ! This site is full of info . Use it.

Neo6, these oils are the most common in the machine tool industry. Get away from Autozone and such and learn what oils really are. The Oil companies have product and interchange charts that will give you a great insight into what is what in oils.

lol so you're trying to tell me you can get a reamer to get AS GOOD or BETTER finish than a boring bar? I'd love to see that.

Don't know what's so knuckle head about boring it? Yes I'm using a cnc lathe, but runout is minimal.i have done this in the past on small holes specifying tight tolerances on diameter, straightness and concentricity using solid carbide micro boring bars and had great success, it all comes down to the parts application. Obviously if it's not that critical do it using the cheapest means possible.

michiganbuck · Oct 22, 2014

Be sure the drill cuts to the correct size and not over size.. you might take a test drilling in a piece of scrap or drill a pre -hole a bit smaller first.

2.1mm=.0827

2mm=.0787

This chart does not go that small but might give some ideas:
http://www.hannibalcarbide.com/documents/pre-ream-drill-size-chart.pdf

Mechanola · Oct 22, 2014

I ream to very smooth surfaces, not much straighter than the bore is, at half the boring speed and still less feed. That way I make very thin and small chips. Cutting oil is a must. There’s a variety of reamer designs for different materials and tasks.

If the bore must be very straight and round, I hone it. To have a straight bore from the start the drill needs to have flutes of very exactly identical length and very precisely symmetrical angles. The alternative is the single flute cannon drill.

To drill out I use three-flute tools that centre themselves but I can hardly improve on straightness with such. Larger diameters can be turned out with the specialty that the tool is pulled, not pushed. Results in better straightness as well.

I make bores, not holes.

Enjoy reaming!

hanermo · Oct 22, 2014

Here is some info ..
2.1 mm to 27 mm is 13:1 length to width ratio, a *very deep hole*, akin to gun drilling.
This is what makes it hard, even the drilling may or may no be hard (breaking drills, easily stuck in hole and wont come out).

Reaming "a hole" so it "looks good" is very easy.
Getting the hole start at the right place, and especially the hole end at the expected end, may be very difficult !

And this depends only on your tolerances.
E.g. no tolerances, round workpiece in lathe, and only spec is 2.1 mm hole indicates;
- Hole is through hole, like a clearance for a bolt/bushing etc. Medium hard/Easy, dfficulty 4/10.

Now, if the hole must be done to +0.01 mm/-0.01 mm, and it must be straight, it still ie relatively easy, as this is typical reamer accuracy.
BUT...
The drilling is unlikely to be straight, to within 0.01 mm +/-.
(With normal drills).

It will wander (around some 0.01 mm over 27 mm length) and end up not in the center where it started, in the center of rotation of the workpiece.
This error might be 0.1 mm, or 0.2 mm, or so, in the 2.1/27 mm scenario.
If this matters, then the job is about 8/10 hard, and costs about 5x more to do.

If you need a more accurate hole, you could need to use a high grade solid carbide drill.
This drill will be quite expensive (20-50 $ easily).

If you need even more accuracy, in hole endpoint location, you could then first pre-bore for the hole.
Again, expensive tooling (micro sized), and some experimentation.

So, this could easily be a 9/10 or 10/10 difficulty hole.
And you could easily need 200-400$ or more in "stuff", to do this.
And a day or so of work, and 3-4 tries, to get it right.
Depends on tolerance desired.

Here are some suggestions in tools, per degree of tolerance.

1. Brand name drills from any industrial supplier. McMaster, Misumi, etc.
1.1. Same for reamers.
Maybe use 2 reamers for better results.
This will make it straighter and a better size. 0.2 mm first time, 0.1 mm second.

Also note that the drilling gets harder, as the depth/width gets smaller (which if why double reaming may not be the right choice).

2. Solid carbide drills. Iscar, Sandvik, etc.
3. Micro boring bars, with (2).

I wrote it out, so that you get some idea how hard this can get, and why some may get impatient with these questions from a new guy.
Research will reveal all this stuff, but you may not know to look for things like
deep hole drilling
running 2 reaming cycles
solid carbide drills
micro boring bars
etc.

Please let us know;
grade of stainless planned (303, 304,316L, etc)
tolerances aimed for
what tools you tried
how it worked out
pics

The better you document the appreciation of (sometimes very valuable) help you get, the more help you will receive in the future.

18my · Oct 22, 2014

I have used solid carbide drills and carbide micro boring bars in 316 ss plus a variety of other materials with great success and achieving tolerances of +/- 0.01mm are very achievable as well as high surface finish. But as both you and I mentioned it all comes back to the application of the hole/bore. Do it using the cheapest means possible for the desired result. Since I have literally shitloads of solid carbide drills and carbide micro boring bars at work I use them when necessary.

Terry Z · Oct 22, 2014

To all dump the carbide drills and try a NACHI SG drill. These work so well and last a VERY long time. First time I used one it was so quiet with the flood coolant I thought it was getting pushed up into the collet and not drilling! So a good straight drilled hole I have good results reaming. I always run a coax indicator on the pocket I am holding the reamer in just to be sure it is true to my spindle. Have a good day making chips!

Bobw · Oct 22, 2014

Neo6 said:
You guys never disappoint thank you, I already order the oils from ENCO as I mention before I was just curious what type of shop would carry those products I know an auto-part shop won't.

Look for oil companies... I'm in the middle of pretty much nowhere with a very small population and I have at least 2 places I can go to get all the funky oils I need.
One is aligned with Chevron, the other Shell. If they don't have something overly funky they can usually get it the next day out of El Paso... They also sell cheap
kitty litter. Problem is, they tend to sell 5 gallons as the minimum, so if you only need a gallon, mail order is probably your best bet.

dgfoster · Oct 22, 2014

michiganbuck said:
Be sure the drill cuts to the correct size and not over size.. you might take a test drilling in a piece of scrap or drill a pre -hole a bit smaller first.<>/QUOTE]

To the OP:
Buck mentioned an idea here so casually that its importance might easily be overlooked.

If you want to drill a hole on-size, you are much more likely to get a final result that is close to the nominal size of a drill if you first drill the hole with a drill that is just slightly undersize. Then finish the hole using the "correct" drill. The second drill will act more like reamer and is more likely to cut very close to on-size than if you just push the "correct" drill on down through the material without predrilling. This process does not solve your present problem, but it is worth knowing about. Using that technique would make it less likely that your pilot hole for boring or reaming will be oversize---uggh.

Denis

Conrad Hoffman · Oct 22, 2014

I ream a lot of stuff on a manual machine and a guy with CNC and a boring bar can beat me every time for geometry and surface finish. But the OP hasn't got a CNC, nor do I. IMO, all reamers weren't created equal and a lot of the cheaper ones are junk. I'd go carbide. I like M.A. Ford for the smaller sizes. Be sure to pick a series designed for what you want to ream. Good oil. At 2-3 mm you won't be going that slow, but slower than you'd drill. Even under the best of circumstances, reaming tends to give slightly lobed holes compared to boring or honing.

Mcgyver · Oct 22, 2014

Neo6 said:
here is my question should I use a floating reamer holder? Is this a must? .

No. Standard reamers have the length of shaft they do so there is enough flex that they will follow the existing bore regardless if held slightly eccentric.

To ream a hole, run 50% of regular speed, use dark cutting oil, and both feed and extract slowly.

Accuracy, no tool marks, straight, round, etc are just words without tolerances put to them - there is no such thing as perfectly straight, to size, round or no tool marks. There are a lot of ways to make a hole all of which have a get different results and with different costs, but all are constrained by by achievable tolerance.

HuFlungDung · Oct 22, 2014

One thing I've learned about reaming: if you start with the hole a few thousandths smaller than the reamer, the reamer will make the hole bigger.

First try at reaming a hole

Aluminum

Hot Rolled

Cast Iron

Diamond

Aluminum

Stainless

Aluminum

Diamond

Aluminum

Cast Iron

Diamond

Stainless

Titanium

Cast Iron

Cast Iron

Diamond

Diamond

Diamond

Diamond

Diamond

Similar threads