how to use a fixed reamer on the mill to bore toolholder to size.

Help a novice please.

Shopmade toolholder is in the spindle, and the reamer is fixed to the table.

I was going to indicate axial and angular alignment, and grab the reamer a ways back on the shank to allow a little float.

7/16" 1144 stressproof toolholder, reamed to .438", the blind bored hole is .424", 1 1/2" deep, leaving .0075" per side to remove.


Suggestions on speed?

Also, can the reamer be used in a peck style, or does it need to go full depth one pass?

Remove it under power, or shut the spindle off? Reamer is a straight flute type.

The reamer will follow the hole that’s already there, so if you’re after concentricity I’d use a boring bar.

If you want it to be accurate bore it, period.

DavidScott said:

If you want it to be accurate bore it, period.

Click to expand...

The hole is bored in place on the mill spindle. So it is a concentric hole- but rough, and undersized. I was figuring the reamer would give a smooth accurately sized finish hole. Isn't that what they are designed to do?

Are you guys saying the odds of accurately lining up the reamer on a true hole and getting a good finish, are worse than boring it to size?

The boring tool could be reground to get a better finish, maybe- a power feed here would help a lot, but there is not one on this axis. With .0075" to play with, there is not a lot to experiment with, to get a clean cut.

Reamed hole size varies depending on how the reamer is used so boring is safer and more accurate on most machines. If you don't have power feed then that does make some difference. Does your quill move around? If so that would probably be a deal killer for boring. Can you feed smoothly and slowly? Kind of like using a lathe without power feed. You can still do a good job but it will be slower and require something from the operator. For best results carbide is a requirement.

DavidScott said:

Reamed hole size varies depending on how the reamer is used so boring is safer and more accurate on most machines. If you don't have power feed then that does make some difference. Does your quill move around? If so that would probably be a deal killer for boring. Can you feed smoothly and slowly? Kind of like using a lathe without power feed. You can still do a good job but it will be slower and require something from the operator. For best results carbide is a requirement.

Click to expand...

The machine is solid, I can feed smooth by hand, but carbide is a no go for light cuts on the 1144 - It works great for deeper cuts at a high feed rate and SFM, but smears with a light pass.

I will try the reamer, and if I screw it up, bore it out for a 1/2" holder and make another one.

so back to the original question- how fast on a 7/16" reamer?
All the way in and back it out under power, or stop it and back it out?
Peck it to clear chips?

I did something similar but not the same one time, on my second arrempt I made a hole in a plastic bottle lid that fit tight on the reamer shank so I could submerge the holder in cool tool while I reamed the part, I reamed on the way through, stopped the spindle and removed the reamer through the exit side so it only went through the part once. Mine was a guide hole for a fixture in 4140 so the rpm/feed wouldn't help much.

Recommended practice for reamers on a drill press is to use same SFM as a drill, but feed them faster and do not dwell or peck. Just push them through in a brisk fashion.

If I were doing this, having bored a concentric hole and wanting to ream to size, I would hunt up a floating reamer holder to ensure the reamer follows the hole even if you clamp it down a bit off-center. Floating reamer holders can, and certainly were, improvised in-shop when needed. 19th Century technique, if not earlier.

What they are saying is

A reamer will tend to follow the existing, drilled hole. If that hole is off center, then the reamed hole will also be off center. If the drilled hole is at a small angle, then the reamed hole will be at a small angle. The reamer FOLLOWS the existing hole. This is due to the fact that a reamer has many cutting edges that are more or less evenly distributed around it's axis. They all tend to push it toward the center and these forces will be more or less balanced. Also, like a drill bit, a reamer is not relieved to allow it to cut sideways like a milling cutter can.

A boring bar has only ONE cutting edge. It will cut an almost perfect circle,cylinder along the axis of rotation. The drilled hole is only there to provide the clearance needed for the boring bar to enter the hole. It can cut more on one side and less on another. It does NOT follow the existing hole.

So a reamer can make an accurately sized hole, but it may not be perfectly centered or at the same angle as the axis of rotation. The boring bar is preferred for making a hole that is both accurate in size and location and angle. But the reamer is a lot easier and faster to set up and use.

The odds of lining it up have nothing to do with it. Well, within reason anyway.

The reason for not pecking with a reamer is that motion will drag the chips up and down the hole. This can change their position in the flutes and possibly cause scratching of the reamed surface. Down and back out is best. And do not stop the rotation as you remove it as those edges can make lengthwise grooves in the reamed hole. This also shows another advantage of the boring bar which has a lot more room for the chips. So those chips are less likely to jam between the boring bar and the wall of the hole and produce scratches.

stoneaxe said:

The hole is bored in place on the mill spindle. So it is a concentric hole- but rough, and undersized. I was figuring the reamer would give a smooth accurately sized finish hole. Isn't that what they are designed to do?

Are you guys saying the odds of accurately lining up the reamer on a true hole and getting a good finish, are worse than boring it to size?

The boring tool could be reground to get a better finish, maybe- a power feed here would help a lot, but there is not one on this axis. With .0075" to play with, there is not a lot to experiment with, to get a clean cut.

Click to expand...

EPAIII said:

What they are saying is

A reamer will tend to follow the existing, drilled hole. If that hole is off center, then the reamed hole will also be off center. If the drilled hole is at a small angle, then the reamed hole will be at a small angle. The reamer FOLLOWS the existing hole. This is due to the fact that a reamer has many cutting edges that are more or less evenly distributed around it's axis. They all tend to push it toward the center and these forces will be more or less balanced. Also, like a drill bit, a reamer is not relieved to allow it to cut sideways like a milling cutter can.

A boring bar has only ONE cutting edge. It will cut an almost perfect circle,cylinder along the axis of rotation. The drilled hole is only there to provide the clearance needed for the boring bar to enter the hole. It can cut more on one side and less on another. It does NOT follow the existing hole.

So a reamer can make an accurately sized hole, but it may not be perfectly centered or at the same angle as the axis of rotation. The boring bar is preferred for making a hole that is both accurate in size and location and angle. But the reamer is a lot easier and faster to set up and use.

The odds of lining it up have nothing to do with it. Well, within reason anyway.

The reason for not pecking with a reamer is that motion will drag the chips up and down the hole. This can change their position in the flutes and possibly cause scratching of the reamed surface. Down and back out is best. And do not stop the rotation as you remove it as those edges can make lengthwise grooves in the reamed hole. This also shows another advantage of the boring bar which has a lot more room for the chips. So those chips are less likely to jam between the boring bar and the wall of the hole and produce scratches.

Click to expand...

To clarify---- The reamer will follow a hole bored in place on the mill. The hole is straight and true, to the limits of my measuring equipment. The hole diameter top to bottom is constant, that shows it is parallel with the mill table. (the mill head is horizontal, I am feeding with the table Y axis.)
The surface finish is rough, however, and on an unhardened piece of steel that is going to wear quickly, as the ridges break down. I also have questions about my ability to use a small diameter boring bar on a deep hole and keep it a half thousandth over.

The floating reamer holder- that sounds like a good idea- this is a device that allows slight axial and angular float, so the reamer exactly follows the bored hole?
I would like to see how they are made, how they work- I am imagining a reamer, secured in a block that has ways, sort of like an x-y table but without a leadscrews, with the reamer secured on the z axis, so it can move in x and y but not in Z .
Is that the idea, or am I completely off the rails here?

If you're working on a horizontal, you're feeding in the Z axis if boring a mounted toolholder with table travel. X is spindle side to side location, Y is spindle up and down. Z is table in and out. If you have spindle travel in and out also that's normally W.

eKretz said:

If you're working on a horizontal, you're feeding in the Z axis if boring a mounted toolholder with table travel. X is spindle side to side location, Y is spindle up and down. Z is table in and out. If you have spindle travel in and out also that's normally W.

Click to expand...

Vertical-horizontal type with the head flopped so the spindle is parallel with the table. So if the axis designation changes with the head movement, I am feeding in Z- in along the spindle bore. I had no idea that the designation changes with the head orientation. What do I call it if the head is at 45 degrees?

Very/most often a reamer will follow the same center line and path as the drilled/bored hole and cut about .0002 over the micrometer checked reamer size. The reamer has an OD circle land and so after just a little chatter /rub at the start will be like a bushing follow tool because of the circle land OD.Good to end the reamer feed before the end of the full per hole size. Micrometer check neat the cutting end because reamers very often have about .0002 back taper going away from the cutting end. A hot reamer will cut a little over the micrometer size. Hot part can also change the expected size.

In some rare cases the flutes are not exact across from each other so the micrometer check can be a little off, this is deliberately done in some reamer designs and so if it appear to be this way a test ream should be performed. Some times the across flutes are marked with a dot on two flutes.

Well if it's a rotating head, you are running a vertical mill with a rotated head, not a horizontal. In that case you decide as you go I suppose...

'' how to use a fixed reamer on the mill to bore toolholder to size. ''

Let's start with the basics, ...what's the tolerance on that bore / hole?

stoneaxe said:

The floating reamer holder- that sounds like a good idea- this is a device that allows slight axial and angular float, so the reamer exactly follows the bored hole?
I would like to see how they are made, how they work-

Click to expand...

I'll see what photos and scans I can come up with. It will probably be a couple of days.

Limy Sami said:

'' how to use a fixed reamer on the mill to bore toolholder to size. ''

Let's start with the basics, ...what's the tolerance on that bore / hole?

Click to expand...

I would like .0005" over 7/16", so a 7/16" shank tool can slip in. The reamer is .438", exactly .0005" over. Maybe a .4375 reamer would be better? I was a bit concerned that if the hole is exactly .4375, the tool would not slide in, and the next step up on on reamer size would just skid , instead of cutting.

Tolerance- now that I do not know- loose enough so a .4375" tool can slide in, and not be sloppy. There will be a set screw to retain the tool. I figured to drill and tap for that last, if for any reason the bore is slightly off set, I can put the set screw on the other side to help compensate.

Well, it worked fine. Was a bit worried about chatter, so ran the spindle real slow at 130 rpm, flooded the drilled hole with lube and wrapped a 3" piece of 1/8" lead solder around the reamer shank so it would not ring.(vibrate)

Cool, thanks for letting us know as so many of these are left open ended.