General advice on using reamers

[Jvizzi]

I'm looking for advice from anyone who uses reamers successfully on a consistent basis, that could maybe correct some possible misconceptions I have.

In my experience, using a reamer for production machining has always been a "last resort" or emergency choice. I have found them to be very unreliable in terms of producing a reliable size once you get below a total tolerance of .001". What I mean by that is during the course of a production run, you might have 10 parts in a row with the hole on size, then random outliers out of tolerance, and then more parts further in the run back on size. I also have had a reamer work out fine for one run of parts, then at the next setup a few months later, using the same part# tool from the manufacturer, it does not work out. I know these tools are manufactured with tolerances, but the variations in the feature sizes I have seen far exceed the manufacturing tolerances.

I also have found reaming to be unreliable for keeping a tight position tolerance, especially with modern GD&T where you may have .001 true position to 3 datums for a 2.00" length hole.

 

[michiganbuck]

Video in reaming buty I expect you know all this.
I think part heat is a significant factor in reamer size failure.

Machining Guide: Reaming Tool Basics - Kennametal

Reaming Machining Basics: Learn best practices to help ensure precision hole reaming in any material type. Learn more here.

www.kennametal.com

 

[YoDoug]

The category of reamers is pretty broad. HS or carbide tipped HS body, shell reamers, Padded or guided reamers, solid carbide, carbide head style reamers. They cut differently and all have different levels of tolerance and nuance to get the desired results.

The biggest advice I have to say is garbage in/garbage out. If you have an out of round, or out of position, or varying size pre-hole the reamer will not be consistent. Also feed can affect hole size, especially with HS or tipped reamers. Tool wear can cause HS reamer holes to grow in size.

We use Iscar Bayo -ream for press fit bearing pockets and hold +/-.0002 in production. We have the shanks mounted in dual contact shrink fit holders so they repeat well. We helically bore the hole to -.01" size before reaming with a 3/8 endmill that has cutter comp on and adjusted as needed.

 

[Mtndew]

For HSS reamers, the general rule of thumb is 1/2 the RPM of the HSS drill that drilled the hole, and double the feed of the same HSS drill.
I like Morse hss reamers, they seem to be pretty good.

https://www.morsecuttingtools.com/search/catalogue/group/6221

 

[Jvizzi]

For HSS reamers, the general rule of thumb is 1/2 the RPM of the HSS drill that drilled the hole, and double the feed of the same HSS drill.
I like Morse hss reamers, they seem to be pretty good.

https://www.morsecuttingtools.com/search/catalogue/group/6221

I've never heard a definitive reason why HSS reamer shanks are so long? is it that they are meant to be flexible as they run, or does it just have to do with some old standard of "blanks" used before the reamer is ground during manufacturing? or something else entirely?

I will say that most of my trouble with reaming has been with carbide reamers, and it seems to be because of the flexibility issue. If a carbide reamer does not flex at all, then that means any runout in the tool assembly is going to show up directly in the size of the hole, no?

 

[eKretz]

A longer reamer shank gives some amount of protection from runout in case a floating holder isn't used. While reamers don't generally cut on the sides, enough rubbing can cause a hole to go oversized and/or tapered. If you're doing large scale production, I'd absolutely use a carbide reamer. If you need tight size and location, use a post-drilling step prior to the reamer; either plunge with a slightly undersized endmill or bore, leaving your stock for the reamer. Coolant will usually ream a slightly smaller hole than oil with the same reamer.

 

[michiganbuck]

Reamers usually ream .0002 over the micrometer size, but some can be difficult to measure because one may measure not exactly straight across at exactly 180*
We used to have a fussy reamer manufacturer leave a portion of the web (area between the flues) intact to have a better place to measure.
The rotation of OD up or down grinding can the measure size to the actual finish hole size.
For some very fussy reamers, we finished turning in an adjustable bore with a fine diamond compound.

 

[Mtndew]

I've never heard a definitive reason why HSS reamer shanks are so long?

My guess is so that it can "float" to the hole position if you're off a tiny bit and it can't influence the size or location of the hole especially if it has some runout.
If you stub up a reamer, then you've essentially removed that from the equation and are rolling the dice on size because if the reamer is running out, it could make the hole oversize or out of round.

 

[DanASM]

I've never heard a definitive reason why HSS reamer shanks are so long? is it that they are meant to be flexible as they run, or does it just have to do with some old standard of "blanks" used before the reamer is ground during manufacturing? or something else entirely?

I will say that most of my trouble with reaming has been with carbide reamers, and it seems to be because of the flexibility issue. If a carbide reamer does not flex at all, then that means any runout in the tool assembly is going to show up directly in the size of the hole, no?

The longer reamers are made to have some sort of "flex" or "float" to them so they will self center as needed.

I use solid carbide on smaller reamers and use HSS shank with brazed carbide tipped reamers when sizes go above 3/8 or so. I use reamers all day every day for 10's of thousands of parts and they are very consistant. The only time I ave issues is when the oil gets low and sputters at the cutting edge. Carbide usually plows right through it without issues.

The Floating holder is key. https://www.ebay.com/itm/275800421032

 

[Limy Sami]

IME You can never run too slow for consistant reaming ..........or have too much lube. .......works for me!

 

[michiganbuck]

End sharpening a reamer is best done with the but end on a dead center and the cutting end in a bushing, or held between two dead centers.
Holding a reamer in a collet or a chuck for sharpening is a poor method.
Generally, 8 to 12* is a good primary clearance, and more for aluminum. Perhaps 10 to 15* and more primary can be ok.
At one time, a chatter-avoiding finish reamer was one having one end tooth .0005 higher than the other flutes that were all the exact same height..
Often a reamer end will be set below the center for getting clearance, as this setup swings to a lesser angle, the clearance diminishes, so looking/checking at the OD on the OD circle land should be the OK way to check clearance..rolling under an indicator is the exacting way.
I think it is good to grind the secondary end clearance first and then grind the primary. This way, the ends are more accurate in height, and less heat is generated at the cutting edge.
Sharpening a gang of reamers, it can be good to have a two-step (height) tooth rest finger so to more quickly go from primary to secondary clearance... often an angle of a half degree is needed to keep the primary land straight, a marked strip on masking tape no the swing table is better than looking at the protractor.

For many cutters grinding the secondary first and the primary last helps top keep teeth more all the same height as wheel wear is a prime cause of tooth height variance..better that you lind width changes a little than the tooth height.

 

[???]

I ream a lot of holes with great results, steps below.

• Indicate all tooling used to less than 0.01mm TIR.
• Spot hole with NC spot drill.
• Drill 0.2mm undersized.
• Interpolate 2mm deep in bore with end mill. Hole will be .03mm undersize with most solid carbide tooling.
• Ream hole.

Hocut 795 at 7 percent concentration. Procedure used for all my reaming from 3mm to 12mm holes. I'll check speeds and feeds and post them when I'm back at work. I only use a floating reamer holder in the CNC lathe, all VMC reaming is with ER collets holders.

 

[gbent]

Biggest consideration is hole size before reaming. The tighter the tolerance on rough hole size, the more consistency in reamed hole size. I plan on 1-2% of finished diameter for reamer allowance.

A reamer is not a locating tool, it is a precision sizing tool. It will follow the existing hole.

If a reamer is to stiff it will act like a boring bar. If a reamed hole is bell mouthed most likely the reamer has a runout problem.

 

[MilGunsmith]

The old-timers used to say that you could change the finished hole size by changing cutting lube. A thin oil vs. thick grease.

 

[???]

The old-timers used to say that you could change the finished hole size by changing cutting lube. A thin oil vs. thick grease.

Old school tapmatic with trichlor would give a mirror finish undersized hole. Tapping paste mixed with oil would be slightly oversized. We used motor oil for sprue bush holes because we removed them a lot for polishing and refacing, the reamer would cut quite a bit oversize but finish wasn't the best. Straight flute reaming is very similar to scraping in that the reamer doesn't have rake. As someone else said hole size is heavily influenced by the amount of material removed.

 

[michiganbuck]

Dull drills can work harden certain steels, and so have an effect on how well a remer holds size

 

[Patriot Gearhead]

As Gbent stated "a reamer is not a location tool". A HSS chucking reamer will only follow the existing hole. so special care should be taken with location and straightness of drilled hole. the only exception is jig bore reamers. A jig bore reamer will cut on location and will not follow existing hole. I don't have much experience with carbide reamers. Whether they cut their own or follow an existing hole.
As for size, the following factors all contribute to the finish size.

• Reamer size
• Reamer sharpness
• RPM
• Feed Rate
• Amount of material left in hole.
• Type of cutting lubricant.

If your consistent with the factors listed above, your hole size is repeatable exclusive of wear.
Find what works for you and stick with it.

Go Make Chips!

 

[michiganbuck]

The length of tooling can be important If a machine is out of tram or the travel is not straight. the spot/location can be different going from drill to reamer.

 

[eKretz]

And for the love of all that is holy do not store your reamers (or any other edged tools) with the edges smacking into each other.

 

[BobH]

As for size, the following factors all contribute to the finish size.

• Reamer size
• Reamer sharpness
• RPM
• Feed Rate
• Amount of material left in hole.
• Type of cutting lubricant.

For dummies like me how would each of these factors affect the hole size? Higher RPM = bigger or smaller and such. Handy information to have when a hole needs to be just a little off size. Bob