I hate reaming!

[Oppiz]

I ofter ream small holes in aluminium. Most of the time for 1/8 dowel pin. Nothing ticks me off more than a reamer cutting big.

Do you use floating chucks when reaming? Do have any recommendations speeds & feed, predrill sizes.

[MACHINEMASTERG]

less is more .....

[robk]

quote:

---

Do you use floating chucks when reaming? Do have any recommendations speeds & feed, predrill sizes.

---

Floating chucks

Good quality collets only. I use solid carbide reamers so they're all stubby. We always tram them in also. If you're using HSS or carbide tipped for that matter make sure it hangs out quite a bit so it could "flex" to follow the hole. Make sure you have a good drilled hole prior to reaming it. I don't have a standard for pre-drilling sizes, but I tend to go about .015" smaller than the reamer.

[Mike Whitten CAD/CAM Contractors]

Reamers usually ream big for at least these three reasons:

 

-The tolerance is usually on the plus side(often +.0002) Allow for this.

 

-You are reaming too much material

 

-You have runout. Indicate and/or hang it way out. For most stuff I always just hang it out and ensure runout is reasonable. For faster speeds and speeds, you can choke up but you must have very close runout.

 

HTH

Mike

[Mike Whitten CAD/CAM Contractors]

For a .125 hole, I would drill .122, .120 would be the smallest.

[jeff]

I have found that the default speeds and feeds for reaming in aluminum are pretty good.

they seem faster than hell, but they actually work.

Also how much stock are you leaving for ream?

NO to the floating holder, hold onto as little of the reamer as possible so the shank will flex and find the hole location itself.

6000 rpm 9 ipm. in 6061 aluminum for 1/8 reamer.

[JazzBass]

I leave .002-.005 on the hole walls. Hold reamers in collets. Indicate them in. 1/8 = 180 sfm. /.005 ipr.

I don't use drill chucks.

[Roger Peterson]

I've done a bit of reaming in a variety of materials. I agree with Mike on a couple of points. Here is where I would look first:

 

1. a poorly drilled hole (off center, angled, egg shaped, or too big - caused by incorrect feeds and speeds, dull drill, or the failure to spot drill).

 

2. Make sure you let it cut some material - they are cutting tools not polishing tools. I'd say a min of .002 or .003 per side depending on material for .125" hole.

 

3. Unless you've plunged down the drilled hole with a boring bar or endmill never choke up on a reamer. Choking up's bad for hole sizes and reamer life.

 

4. Make sure you chamfer the hole. I've seen a lot of people try to skip this step, once they start crooked because of a burr or a chip you're done.

 

 

HTH

[CAM-mando]

I agree with everyone on the collets, flexible length and indicating the carbide.

 

I leave 1/64" for reaming down to about 3/16". Under that, I leave between .005 and .010 depending on drill sizes etc. +1 on the c/sink hole prep.

 

I am a proponent of drill, bore and ream any time true position is less than .005, size is less than .0007" or hole is very deep. Usually end mills work fine for boring. For production jobs we relieve about .005" diameter or so behind the cut.

 

Trying to hold close size when drilled holes have bad location (especially on deep holes) will cause you to go bald way too early.

[notso]

I have had lots of luck reaming .124-.1245 and .1255-.126 holes (press & slip fit for 1/8 dowels) in aluminum using GOOD QUALITY drill chucks. Spot & predrill hole .120, then ream, 600-1000 rpm 6-8 ipm. I've done 1000s of them +-.0005 on location. The place I used to work used 1/8 dowels to locate everything inside their machines.

[Tim Johnson]

+1 notso,

 

1000 rpm. 8 ipm. use a .120 dia. hole. Lower rpm tends not to wash out the hole (pull the reamer at the top). Prebore if location is less than +/-.002 and you're drilling with hss (shouldn't be necessary if drilling with carbide). For alum and a 1/8" reamer it doesn't really matter what holder you use as long as it's running true.

[Guest CNC Apps Guy 1]

I'm a Spot Drill, Drill U/S .003/.005 per side, Chamfer .003/.005 per side, Collet, Choke-Up, Indicate, Solid Carbide kind of guy.

Say that fast 10x...

[Kevangel]

When I was "younger" and building dies,(needing that perfect light tap fit on punches when installing them)we would buy a half-dozen reamers in the size range required and pick the one that gave the "perfect fit" then save it for that application including recording the rpm...i.e. the same reamer will cut different sizes at say 250 rpm and 800rpm-the higher rpm will cut larger. Also when working as a Moldmaker the shop owner told me you can run a reamer backwards and stone it, to make it cut tighter in an emergency..seems I have had some late nite success with that.

[Alvaro Gil - Cimquest-inc.com]

I think reamers suck. In most cases (shallow) I can get by by just doing a helical bore or a simple contour with an end mill. Make sure your post is set to IJK though, it will produce a rounder toolpath on a slower controler. For a 1/4" holes I use a 7/32 carbide endmill. Make sure you use wear comp so you can rapid in the middle of the drilled hole, or if you helical in you can do a small lead out and rapid out.

 

They come out perfect with the added convinience of cutter comp.

[Scot]

+1 Avon

[Fred Beard]

I have found that WD-40 works great with aluminum. Leaves a nice finish and won't drag chips when coming out of hole.

[Dan Schnars]

I have pretty good luck if I spot / drill like .120 .122 and then interpolate the finish diameter like .050 or .075 deep... Gives the reamer something to follow to get started... Works good here... I hold the reamer in a regular collet and just get as close as run out as I can... try that.

[Threept82]

I always center drill, drill and if need be I

end mill then ream but if true position is open

and size is important I double ream. Double reaming ensures a better size because finish reamer is removing a constant amount of material

from already smooth walls, unlike a drill.