forrest, are you there? anybody?
https://www.practicalmachinist.com/...ing-oversize-75483/?highlight=reamer+oversize
https://www.practicalmachinist.com/...ing-oversize-75483/?highlight=reamer+oversize
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
reaming on size
- Thread starter dian
- Start date
- Replies 38
- Views 4,048
i wonder what he ment by:
"I often Lay a hard Arkansas wedgie stone in the flute and gently stone a tiny negative rake on the reamer's edge. Stone a tiny bright line representing a 5 degree radial and axial negative rake at the cutting corner."
is he really saying to dull the edge? they always tell you not to run a reamer backwards to prevent this. is he simply saying to break the corner? (on a machine reamer.)
at the moment im looking for ways to make a reamer cut smaller.
"I often Lay a hard Arkansas wedgie stone in the flute and gently stone a tiny negative rake on the reamer's edge. Stone a tiny bright line representing a 5 degree radial and axial negative rake at the cutting corner."
is he really saying to dull the edge? they always tell you not to run a reamer backwards to prevent this. is he simply saying to break the corner? (on a machine reamer.)
at the moment im looking for ways to make a reamer cut smaller.
TGTool
Titanium
- Joined
- Sep 22, 2006
- Location
- Stillwater, Oklahoma
Meaning, you want to take a .2500" reamer for instance, and have it ream a hole to .2495"? Or just that your .2500" reamer is making a hole that's .2503" and you want to get it to quit going oversize?
Terry Keeley
Titanium
- Joined
- Oct 18, 2005
- Location
- Toronto, Canada eh!
I messed with this a fair bit and found that running the reamer in the lathe backwards and stoning the cutting edge works.
Do a little at a time and test.
Do a little at a time and test.
Mike1974
Diamond
- Joined
- Nov 5, 2014
- Location
- Tampa area
If you really need to ream and hold a certain size within a couple-few tenths, just order over under reamers until you get the desired size. Sure, it can get expensive, but reaming is like black magic to hit *the* size. Coolant, oil, feed, rpm, stock left, all play into effect....
PackardV8
Hot Rolled
- Joined
- Jun 4, 2006
- Location
- Spokane, WA
And the parent material. We're an automotive shop reaming valve guides and find it requires a specific reamer pattern and a specific diameter to end up with a desired spec for cast iron, powdered metal, bronze, silicon bronze, et al; the same reamer will cut a different diameter if switched to a different material.
Sometimes, even with the variety of reamers we have on hand, it requires honing valve guides to get to the tenths we want.
jack vines
eKretz
Diamond; Mod Squad
- Joined
- Mar 27, 2005
- Location
- Northwest Indiana, USA
Yes he's saying to just very gently add a 5° (or less) negative rake as a small land - small as in barely visible - just enough to see the glint when the light reflects off it. This will help prevent the reamer from biting in so hard and will also help make it cut ever so slightly smaller. Only do this if the reamer is cutting larger than it measures or if you need to clean up some light damage. And I stand by my recommendation on that thread (from 2006?!) of not touching the edge with a stone if you don't understand exactly what you're attempting to do...
Take care to check the outside land after stoning also, if a burr is raised you'll need to remove it. Carefully. Many new HSS tools come with a burr. If you check every tool you use and stone it carefully you can get some pretty substantially improved tool life.
Take care to check the outside land after stoning also, if a burr is raised you'll need to remove it. Carefully. Many new HSS tools come with a burr. If you check every tool you use and stone it carefully you can get some pretty substantially improved tool life.
Last edited:
Making really fine reamers is an art form. A commodity reamer may not be art.
CarbideBob
Diamond
- Joined
- Jan 14, 2007
- Location
- Flushing/Flint, Michigan
The OD of a reamer is circle ground. Making it cut smaller than the actual size not so easy.
Often a newer reamer will cut oversize for it's real dimensions. "Dulling" the reamer gets rid of this overcutting.
Also reamers have a back taper meaning that further up the shank they are smaller. Sort of like drills but drills have a much higher taper.
And then there is heat pushed into the part and material springback. If ones dulls or goes more negative the hole poked once cooled or out of compression can in fact be smaller that the actual reamer.
That one weird.
To do this rapid retract is needed and you can see it in parts that have been cut but you can not fit the original reamer into the finished hole. How can that be?
If there is too little stock for a reamer it tends to follow runout in the mount for size which is always there and act sort of like a wobbling endmill.
Too much stock and they just do not want to play. Then heat, bind, no life, all sorts of bad things.
If you want to go undersized from the current actual tool dia. you will have to attack that outside margin or play some very fancy tricks with stock compression and heat.
Bob
Often a newer reamer will cut oversize for it's real dimensions. "Dulling" the reamer gets rid of this overcutting.
Also reamers have a back taper meaning that further up the shank they are smaller. Sort of like drills but drills have a much higher taper.
And then there is heat pushed into the part and material springback. If ones dulls or goes more negative the hole poked once cooled or out of compression can in fact be smaller that the actual reamer.
That one weird.
To do this rapid retract is needed and you can see it in parts that have been cut but you can not fit the original reamer into the finished hole. How can that be?
If there is too little stock for a reamer it tends to follow runout in the mount for size which is always there and act sort of like a wobbling endmill.
Too much stock and they just do not want to play. Then heat, bind, no life, all sorts of bad things.
If you want to go undersized from the current actual tool dia. you will have to attack that outside margin or play some very fancy tricks with stock compression and heat.
Bob
hanermo
Titanium
- Joined
- Sep 28, 2009
- Location
- barcelona, spain
I like all the posts above and they mostly supported my learning.
Depending on depth, material, and size and quantity (and money) and tolerance, NONE of which are referenced at all, ...
For medium qty in medium material like alu brass and cast iron I would probably double ream while adjusting the reamers via abrasives of choice.
Si-cal paper on a plate would work fine.
I would end up with holes to spec, and charge for the tools and work and tests in nre.
Like always, *details* are imperative in engineering and manufacturing.
If I needed lots of holes very fast, very well, I could use a rigid custom diamond hone.
3000$ only, for 300k qty per year in auto apps.
Less that for lesser mortals.
The diamond hone is good to around 0.01 mm in tir and size (no idea about the corners).
Much better can be done with the second hone.
In anything engineering and manufacturing, better depends on quantity and money.
Provide both, and desired outcomes, and results can come out.
I could probably make a hole to 20 mm or 3/4" depth, through hole.
To 0.1 micron TIR and cylindricity.
For about 1m€, depending on the material and measurement and usage.
Depending on depth, material, and size and quantity (and money) and tolerance, NONE of which are referenced at all, ...
For medium qty in medium material like alu brass and cast iron I would probably double ream while adjusting the reamers via abrasives of choice.
Si-cal paper on a plate would work fine.
I would end up with holes to spec, and charge for the tools and work and tests in nre.
Like always, *details* are imperative in engineering and manufacturing.
If I needed lots of holes very fast, very well, I could use a rigid custom diamond hone.
3000$ only, for 300k qty per year in auto apps.
Less that for lesser mortals.
The diamond hone is good to around 0.01 mm in tir and size (no idea about the corners).
Much better can be done with the second hone.
In anything engineering and manufacturing, better depends on quantity and money.
Provide both, and desired outcomes, and results can come out.
I could probably make a hole to 20 mm or 3/4" depth, through hole.
To 0.1 micron TIR and cylindricity.
For about 1m€, depending on the material and measurement and usage.
so should the red facet be stoned on the edge like this?
edit:
it is a 16 mm H7 reamer. H7 is 0/+18µ. reamer measures 16.013 in front and tapers back to 15.993. H7 reamers are standard, anything else is much more expensive. the hole it cuts with ethanol is 16.035. i used a 15.5 drill making a 15.7 hole and also bored to 15.6 mm. no difference. im looking to get a 16.005 hole.
so actally the reamer is cutting at the relieved corners only. my idea would have been to reduce the lands at the corners. any thoughts?
no idea if the lands are ground circular, if they are i cant see it. at the moment im only practicing for a 30 mm reamer ($$$). i getting the impression that a hand reamer would cut a smaller hole.
edit:
it is a 16 mm H7 reamer. H7 is 0/+18µ. reamer measures 16.013 in front and tapers back to 15.993. H7 reamers are standard, anything else is much more expensive. the hole it cuts with ethanol is 16.035. i used a 15.5 drill making a 15.7 hole and also bored to 15.6 mm. no difference. im looking to get a 16.005 hole.
so actally the reamer is cutting at the relieved corners only. my idea would have been to reduce the lands at the corners. any thoughts?
no idea if the lands are ground circular, if they are i cant see it. at the moment im only practicing for a 30 mm reamer ($$$). i getting the impression that a hand reamer would cut a smaller hole.
donie
Diamond
- Joined
- May 17, 2003
- Location
- Walla Walla Wine and Wild Turkey
Forrest Addy had a huge collection of stones, and used them to great advantage on all his cutting tools keeping them sharp, and I mean sharp!
I will mention this, if you have a cutter grinder with a motorized workhead, end mills can be circle ground on the flutes, so just the end cuts, these can be adjusted to closer tolerances and better finish then jobbers reamers.
I will mention this, if you have a cutter grinder with a motorized workhead, end mills can be circle ground on the flutes, so just the end cuts, these can be adjusted to closer tolerances and better finish then jobbers reamers.
swarfless
Cast Iron
- Joined
- Aug 31, 2005
- Location
- South Australia
Just try Forrest's method EXACTLY as he describes .. the negative rake on the cutting bevel reduces the reamer's tendency to 'hog' i.e. there is less tendency for the cutting edge to initiate a chip that goes deeper than the cylindrical surface of the reamer body,meaning larger diameter than the cylinder. That's the trick .. to prevent the over-enthusiastic 'bite' of a sharp reamer. Your diagram is correct. The reamer acts more like a scraper thusly treated.
eKretz
Diamond; Mod Squad
- Joined
- Mar 27, 2005
- Location
- Northwest Indiana, USA
That is the idea. However, as I noted earlier, keep that "5°" angle as minimal as you can. It doesn't need to be specifically 5°. Less is fine, definitely not more. Also be sure to check for burrs! Any existing or any that you make when you stone that flute. Remove them carefully with a fine stone. A well-worn-in Arkansas is good.
And your lands will be circular ground if you have a reamer meant for use in a machine tool. The only time they're not is for some hand reamers or something like a bridge reamer. Circular lands make the reamer follow the existing hole, so it mainly only cuts at the junction of the lead-in chamfer and the land unless there's some amount of misalignment.
Terry Keeley
Titanium
- Joined
- Oct 18, 2005
- Location
- Toronto, Canada eh!
A 16mm reamer cutting 1.5 thou oversize outta the box?
I'd be looking at my setup/process before I started messing with the reamer.
Runout? SFM? Amount of stock removed? Cutting fluid/dry? Stop in the hole and retract? etc.
What material are you working with?
I'd be looking at my setup/process before I started messing with the reamer.
Runout? SFM? Amount of stock removed? Cutting fluid/dry? Stop in the hole and retract? etc.
What material are you working with?
TGTool
Titanium
- Joined
- Sep 22, 2006
- Location
- Stillwater, Oklahoma
He's working with millimeters so only about .0008" oversize.
Setting it up to cut slightly smaller than the the diameter at the large end will require some thought. Cutting it back to where the body is the size you want and re-grinding the cutting flats would be one idea.
