reaming holes on the cnc mill (can of worms open)

Hi all,

We have a job where we have to ream four .2496" holes -.0001 +.0004 on the mill. The material is aluminum and the holes are .5" deep. I have read almost all the posts about reaming and have gotten conflicting answers on almost everything, so much so that a lot of people completely give up on reaming all together. I don't have much experience with reaming so here is a couple questions.

1. Should I use a free floating holder on the mill when reaming (like a tapping holder) or just stick the reamer in a fixed collet and indicate the reamer concentric? I am assuming the free floating reamer would allow the reamer to follow the hole better.

2. Some people said using oil can cause the hole to go oversize so you should instead use coolant. Others say you should use oil or WD-40. What is the correct answer? I am assuming coolant would be able to keep the part more cool than brushed on oil would but I don't know.

3. Should the reamer rapid out of the hole when finished cutting or should it feed out of the hole with a G01 move at the same feed rate as going in?

4. I read that you should leave .01 - .012 (sometimes as high as .031) in the hole for the reaming operation. Other people say you should leave about .004-.005 in the hole for the reaming operation? Which one is correct?

5. Should I use a carbide reamer or high speed/cobalt reamer? I am guessing the carbide reamer will cut a more precise hole, but it is aluminum so I am assuming a high speed reamer would do a good job. Enlighten me here.

6. For speeds and feeds, a lot of people say 1.5x the feed and half the speed of your drill. Is this true? What speeds and feeds should I run? I would think it would be depended on if you are using a HSS/cobalt or carbide reamer.

7. What size reamer should I buy for the job? Should I buy a reamer at the .2496 size or should I buy a reamer a couple tenths under in case it cuts big?

8. Should I countersink the hole before reaming to get rid of any burr at the top of the hole?

9. If a reamer has more flutes, does it cut more precise? Will a six flute reamer at .2496 cut to size better than a .2496 four flute reamer?


I wanted to say that we haven't done a whole lot of reaming (we ream holes occasionally) because my dad (owner of the business) likes to ream with drills. He used to ream a lot of holes with reamers where he used to work years ago and says sometimes they are more trouble than what they are worth. What he does is spot/center drills, drills the hole to a size about .010 from the nominal size, then runs the final size drill in the hole to get the final dimension. It usually lands us +-.0005 or closer. The final drill is typically a high end double margin 140 degree drill. Or if he wants a straight hole, sometimes he will spot/center drill, then rough drill, then run an endmill in there to straighten the hole out, then run a double margin 140 degree high end drill to get the final size. Is this something you all do?


Thanks,

Chris

Does nobody know?

I have no experience with reamers, but given that you're not getting any replies, here's what I'd do:

M.A.Ford has a line of reamers with good tech data: https://www.maford.com/SiteContent/...ter_Catalog Interactive Reamers tech data.pdf

Their 272 series reamers contain an off the shelf .2495" that may work perfectly for you. I'd call them up, explain your application, and ask what that would do what you need.

When I need to hold tighter than +/- .0005" I interpolate rather than use a reamer. Reamers are unpredictable on that scale; a little different coolant concentration or a change in the edge condition of the reamer can make a big difference in the size it cuts. Interpolating I can dial it in a tenth at a time.

mhajicek I agree we interpolate all the time but after reading a bunch of stuff on PM about interpolating close holes, a lot of people are against it for close work ( backlash). You also have to make sure your using ijk's instead of R's.

I was like that too (interpolating), when my mill was new. Now with a couple 1,000 spindle hours and a bit of backlash creeping in, I'm not so sure. I have n o means to measure roundness of an interpolated hole, so even if it gages correctly with pins, it might not be correct.

IME reamers are tame, as long as you do a couple things -- first, make sure they are running true. You can "tap them in" so there's no runout. Second, drill or interpolate to like 95% of final hole size.

I run ~30% of the RPM used for the drill, and like 2x the feed.

Regards.

Mike

There isn't really one correct formula or recipe to reaming. Rather, it's about adopting or developing a reasonably good procedure and making sure you always follow that procedure.

Doesn't matter if you're using a floating or rigid holder, but don't expect the same results if you change your holder, change the tool stickout in the holder, etc.

Doesn't matter if you're using oil or coolant, just keep it consistent.

Stock allowance is for you to figure out, as it'll affect the final hole size. A .250" hole will not behave the same as a .500" hole. Drilling alone will probably not give you repeatable stock allowance, nor very good roundness. Better to pre-finish after drilling with an endmill.

Countersinking before finishing is always a good idea regardless of the finishing method. If anything, it avoids the possibility of creating a burr on the inside of the finished hole.

mhajicek said:

When I need to hold tighter than +/- .0005" I interpolate rather than use a reamer. Reamers are unpredictable on that scale; a little different coolant concentration or a change in the edge condition of the reamer can make a big difference in the size it cuts. Interpolating I can dial it in a tenth at a time.

Click to expand...

Just out of curiosity... what kind of machine are you running? Can you really compete with a reamer at this size on hole geometry? What about reversal spikes and backlash comps? Is the machine really dialed in that much? When was the last ballbar test you've had on it and what did it look like?

Not saying it can't happen. You're at what, 2 1/2 diameters with a 3/16 max cutter or 4 diameters with an 1/8th tool in aluminum. I can imagine it, but haven't tried such a thing. Do you go around twice to clean any traces of comp starting and stopping? Or perhaps to clean up some slight tool flex under-size at the bottom of the hole? Maybe not at this size/depth ratio or material, but in general? Just curious... really.

Orange vise, that is why we will sometimes finish the hole (a hole that is +-.001) with a three flute or double margin drill to ensure roundness and straightness

13engines said:

Just out of curiosity... what kind of machine are you running? Can you really compete with a reamer at this size on hole geometry? What about reversal spikes and backlash comps? Is the machine really dialed in that much? When was the last ballbar test you've had on it and what did it look like?

Not saying it can't happen. You're at what, 2 1/2 diameters with a 3/16 max cutter or 4 diameters with an 1/8th tool in aluminum. I can imagine it, but haven't tried such a thing. Do you go around twice to clean any traces of comp starting and stopping? Or perhaps to clean up some slight tool flex under-size at the bottom of the hole? Maybe not at this size/depth ratio or material, but in general? Just curious... really.

Click to expand...

It's a 2015 Haas VF-3SS with a TR-160Y trunnion. We have it laser and ball bar calibrated once a year, last ball bar in X/Y showed about .0003" out of round at 4" diameter and 40 IPM. Last holes I did were .1205" +.0008"/-0" x 1/4" deep in Ti grade 5 at about 6" away from the center of rotation. Holding the tolerance was trivially easy, and there were no axis reversal marks that I could see or measure. I interpolate around cylindrical bosses all the time, and never get any reversal marks that I can see or measure.

13engines said:

Just out of curiosity... what kind of machine are you running? Can you really compete with a reamer at this size on hole geometry? What about reversal spikes and backlash comps? Is the machine really dialed in that much? When was the last ballbar test you've had on it and what did it look like?

Not saying it can't happen. You're at what, 2 1/2 diameters with a 3/16 max cutter or 4 diameters with an 1/8th tool in aluminum. I can imagine it, but haven't tried such a thing. Do you go around twice to clean any traces of comp starting and stopping? Or perhaps to clean up some slight tool flex under-size at the bottom of the hole? Maybe not at this size/depth ratio or material, but in general? Just curious... really.

Click to expand...

My HS VS40 will hold round better than a tenth. No backlash comp traces cause it pretty much doesn't use it. The numbers are something like 0, 1, 3. Some of my other machines , those get boring heads which is what I would suggest to the OP if his machine can't interpolate well enough.

I'm actually interpolating 5/16" dowel pin holes on it as I type this

It's hard to beat heavy double column iron with big pre-tensioned screws

We have a daewoo 3 axis mill that we interpolate with all the time. It is deadly accurate. There is a titanium part we make that has tapered radial holes (bigger on inside, smaller on outside) that we got a custom tapered (dovetail like) endmill for. The tolerance is very tight because the customer spins the 10" part at 21,000 rpm (almost supersonic). The machine holds it all day long. A picture of a similar part with the radial holes is attached to this post.

I am sure we could interpolate the .2496 hole x .5 deep, but I thought it was a little small and deep for that. I thought a reamer would work better.View attachment 313745

Do you guys rapid out of the reamed hole or retract with a g01?

cgrim3 - somewhere in the pool of posts you found about reaming was me asking "does aluminum shrink?"

The real answer to your question (which OrangeVise alluded to) is you need to develop a process, test it, and remember what your learned. (If you only have costly workpieces to test on this will get unpleasent fast.)

It *is* possible for a reamer to produce a hole which is undersized (really, I've done it) - that hole may also be badly lobed.

Good machines CAN interpolate really well, sometimes. And things like tool deflection and spring passes matter.

Bryan_machine yes one of the posts I found was you asking if aluminum shrinks so should you rapid or not out of the hole. You are right though. We are going to have to develop our own process and figure out what works best for us.

Just the other week, we reamed MP-35 super alloy on the lathe (very small hole) and the holes were within a couple tenths. We used a floating holder for that. But there are a lot of variables and we will have to figure them out, one by one

I found a great reaming guide online. Check this out.

https://www.hannibalcarbide.com/documents/cost-effective-reaming-guide.pdf

Also, does anybody have experience with garr reamers? Are they any good?

Spot ,drill, stab, ream,dead spindle retract,hole done,or 1000 holes done.
have we forgotten how to install press fit 1/4 dowel holes??
Gee wizz.
peace
or rtump iffin ya pree fur.
Gw

This is insane, just interpolate the damn holes and be done with it. It's a 1/4" hole 1/2" deep, roll a 3/16" end mill spin it to 12k and that's that. Why beat it to death?

Greg White and plastikdreams....thank you for the rude responses. No need for that here. As you can see from my first opening post, I am trying to get the details, since the devil is in the details. Yes....I can take a reamer and just plow it through no problem. In fact, I did this very thing on 20 parts last week on the lathe and the holes turned out good. But if you read my opening post, I am trying to gage the processes of everybody here on PM since there is a ton of conflicting information on how to actually go about it. Yes I have successfully reamed quite a few holes. But I want to get to the bottom of the PROPER way to do it.

Is this such a bad thing? Remember, you catch more flies with honey, not vinegar.