Best reaming practices question!

[Micmac1]

Reamers, especially cheaper HSS ones tend to ream oversize .0005-.001 from my experience, we usually order a remer sized to very smallest allowable tolerence of the hole and usually that works for us ending up middle-high of tolerence. carbide remers for smaller holes tend to hold much tighter tolerences than that. We dont use reamers in our lathes since, well we dont have many parts that need to be reamed, and we bore most of our stuff, no Y axis either on our lathes. With our mills tho for anything super tight that cant be bored we ream, and have had good luck with floating reamer holders, but also use er32 regularly. Biggest things are start hole size & concentricity, follwed by speed and feeds. I think the old school way of reaming is 1/2 the drill speed and twice the drill feed for reaming.

 

[michiganbuck]

Reamers are the simplest cutter to sharpen and can be ground on the simplest manual machine. A shop running a production part and dulling a hundred or a few hundred reamers a month should invest in a simple Tc grinder. In-house reamers should cost less than $3.oo. each to sharpen.

Good/best to sharpen between centers.
Next, best is the nose (end) in a bushing and the tail on a center.
Poor to very poor is the reamer held in a collet or a chuck.

 

[Milling man]

Reamers are the simplest cutter to sharpen and can be ground on the simplest manual machine.

I have big doubts that an inexperienced person, even with a good manual sharpening machine, will be able to sharpen the cutting edges of the reamer well. The tooth pitch is not uniform (to combat the effect of a multifaceted hole). A reamer not sharpened very accurately will make the holes less accurate and possibly less rough.
If someone has hundreds of reamers a month, I would suggest taking them to a sharpening center. With such a batch, the price of sharpening one piece will be small.

 

[michiganbuck]

it would take me very little time to break in a mechanically inclined person to proper reamer sharpening.
Set up buying a used machine likey under $6K .. likely pay back to zero in a few weeks.
It is not uncommon to pay 50% of the new cost for resharpening. For a shop buying high-quality reamers, resharpening can be a high expense.
To buy 5/8 HSS might cost $50+, and a carbide over $100.+ so the 50% cost would rack up to big bucks quickly.

Bargain reamers cutting .0005 and .001 over are very likely to poorly end sharpened and doing almost all the reaming with one tooth.

 

[michiganbuck]

Also consider the corner angle of your reamer and the number of teeth.
If you divide axial the feed per revolution by the number of teeth what might be your chip thickness be? A HSS reamer might like a .002 to .004 cut per tooth.
The corner angle also reduces the chip thickness. With your axial feed of .oo4, your chip thickness with a 30* corner or a 45* corner will be less than .004

Your material might favor a 275 to 400 RPM with a HSS reamer so you might try that with a per tooth chip load between .002 and .004 .

The .625 finish size may be better served with about .015 for the reamer to take, .007 on a side
Standard size drills might be 37/34 leaving .017, or a 15,5mm leaving .015 to take. That is about where I would start the figuring.
And then I would take a look at the reamer wear land and consider pulling the reamer at perhaps a .015-.020 wear land and note the parts number at that. I might log the hole size check at every 50 or 100 parts to see if some number of parts makes a significant change in the hole size.

But I'm a grinder guy so the other guys who have more CNC reamer use experience may narrow it down quicker than me. From the grinder side you want to get the total expected error down to about .0002 and then increase your reamer size to the maximum, with safety to that size. This is so that you can resharpen to near taking 3/4 inch off the reamer length before it is undersized into back-taper. And, yes the reamers have good quality sharpened ends so every tooth is taking a cut.

 

[maguilera]

Currently the reason we are doing a reamer is the speed in which they want to make the part. It's simply faster then using a boring bar even though we have them in multiple sizes.

I have a genuine question, how does reaming with HSS is faster than boring with a carbide insert?

I don’t know the details of your setup, part geometry or the limitations of your machine. But for this operation, what you could do is drill with 15mm and then do a finishing pass to 15.875mm(0.625in) with a boring bar at 250m/min (≈820 SFM) which at this diameter would be around 5000RPM and a feed of 0.12mm/rev (≈0.0047in/rev). These parameters will give a linear velocity of 600mm/min (23.62 IPM), which is much larger than the 6-8 IPM you need to use for reaming with HSS on 1144 steel.

Cheers

 

[michiganbuck]

A good reamer setup can't be beaten for speed and reasonable accuracy, often to make parts to -0 +.0008. (and with lapped reamers even closer.\, lapped and they can be JoBlock tolerances in the millionths.)
A good way to buy reamers is by the dozen and specify the size.

For the op, he may wish to be .0003 short of the hole high limit or .0003 above the part low limit..or someplace in between and giving the reamer maker a .0002 spread ( if the part spc allows).
Special Drill and Reamer of Michigan might be a place to get a quote. (plus they will talk to the customer to help engineer the size or method.)

 

[gustafson]

Everything I was going to say has been said, less rpm, more chip, float