What is the trick to reaming on CNC mills? I have done everthing from speed & feeds to making sure clean holders, collects & ect.
Thanks, Bill Johansen

I assume you are getting oversize holes, Bill?

One thing: you need a very accurate collet chuck to hold a reamer straight (as if you didn't know:) ). A regular 3 jaw drill chuck is not likely accurate enough.

Thing two: the closest fit I have found with reaming is created when using WD40 for a lubricant. It will cut .0005" smaller than most any oil, tapping fluid or synthetic water based coolant.

Thing three: try using a floating tap holder to drive the reamer. If it will enter the hole properly, it should follow what was there. I'm referring to something like an ER16 collet system for tooling like this.

.....and

Thing four: Proper hole size before reaming. Common mistake of leaving too much stock for the reamer to remove.

Thing five: Proper feeds/speeds. Changing them won't help much. Using the correct SFM and FPT will always give you a consistant hole size.

Thing six: The reamer will follow the hole. So if the hole has led off a bit the reamer will follow and ultimately give you a bad hole. Try running an end mill (or boring bar) thru the hole after drilling to 'straighten' up the hole.

And as HuFlungDung said, make sure your collet system is good. Put an indicator on the reamer to make sure it is running true. And use the lube!

Originally posted by Bill
What is the trick to reaming on CNC mills? I have done everthing from speed & feeds to making sure clean holders, collects & ect.
Thanks, Bill Johansen

The "trick" is experience. ;>)

What material are you having a problem with ?

What is the feed and speed you are using ?

Have you thought about double drilling. I frequently do
this.

Are you sure your leaving enough material for the reamer to
clean up the hole with ?

You might also note that I frequently use a 3 jaw chuck.
Even if the reamer runs out a little it will follow a
drilled hole. With the crap tooling our shop has though, I
do frequently have to double drill and then ream to get what
I want.

Hope this provides a little food for thought and let us
know how you make out,

jon

I will be reaming 6061-T6 90% of the time. I am waiting for reamers to start testing. We will c-dril, drill 31/64, G13 to leave .004 per side, ream .5010. Speed & Feed for the reamer is at 2600rpm and 40ipm, this is in the ball park so we can test. We have a floating tap holder should i G13 the hole to .5000 to get a good start ?
Thanks, Bill Johansen

Have you thought about double drilling. I frequently do
this.



+1, double drill that sucker to get a better starting condition for the reamer. Also, all other suggestions are good.

In alum, I generally run reamers at 300 RPM and 3-5 IPM on anything under .25, and a little slower for anything bigger.

I have also found that you can change the dia by a few tenths by adjusting the speeds/feeds; Keeping the reamer in the hole longer with more revolutions will make it bigger, etc.

'Rekd

Double drill i will try 1/16 under & then 1/64 under during my test.
Thanks, Bill Johansen

reaming

To get the best results size, finish and location. I use recommended tool relief on reamer, proper speeds and feeds and lubricant. The reamer following the hole is very true and double drill. one drill just follows the other and results are usually a hole that is not round. I use an undersize end mill after the drill to insure proper shape of hole along with size and location. When possible I center drill large enough to leave a chamfer to help start the reamer into hole and reduce chatter. good luck hope I was a help

woodsmith, good advice. The reason I double drill is to make the hole concentric, not straight. If I have a problem with the drill walking, I will EM it. Otherwise, just double drill to remove the 'bell mouth' that often occurs when drilling.

BTW, I notice a new thread that appeared to be a reply to this thread, it had the same contents, so I removed it. If you intended a new thread, lemme know and I'll gladly restore it. (Mayhaps this is a good candidate for someone to post in the Tech section??)

you are correct about the duplicate post. I am new to this type of forum and appreciate your help in getting that removed for me. The tech post part I will leave up to you. Thanks

Oh, the reamer has to be perfectly sharp :D Don't guess, use a magnifier to inspect the cutting corners. If there is any visible damage, to only a few teeth, it will ream oversize.

If the edges are worn from a lot of use, or difficult cutting, then the reamer will score the hole, because, as you may know, the flute lands of a machine reamer are non-cutting. The land is a guide for the tool. Only the chamfered corners do the cutting.

What's a floating tap holder? :confused:

Originally posted by woody5
What's a floating tap holder? :confused:

Its a wooden tap chuck :D

Actually, it is a chuck that is designed to hold a tap, with some spring loaded flexability in the radial and axial direction. It is commonly used to compensate for lead errors between the tap and the feedrate of the machine's Z axis.

It has a little bit of radial float, too, so it will allow the tap to align itself with a slightly out-of-position hole. Thus, it will work in the same way with a reamer. It is not necessarily the ideal answer, because the tool does wobble a little until it gets started.

Originally posted by Bill
I will be reaming 6061-T6 90% of the time. I am waiting for reamers to start testing. We will c-dril, drill 31/64, G13 to leave .004 per side, ream .5010. Speed & Feed for the reamer is at 2600rpm and 40ipm, this is in the ball park so we can test. We have a floating tap holder should i G13 the hole to .5000 to get a good start ?
Thanks, Bill Johansen

That's a bit fast, Bill. In 6061-T6 reaming a .501 hole I would start at about 688 RPM (90 SFM) and about .012 per rev feed, which would be about 8.25 IPM in this case. Your stock of .004 per side is pretty good. I usually shoot for .004-.006 per side.

I can't stress enough the importance of having a 'good' hole before you ream it. The reamer can only do so much and making sure the pre-reamed hole is good will insure consistency.

...and never run the reamer backwards when retreating out of the hole.


Dan

+1 E-STOP
On the speeds & feeds

Also a floating reamer holder is what your after.
A tap driver is a diff. tool.

PEACE:D

Originally posted by E-Stop
That's a bit fast, Bill. In 6061-T6 reaming a .501 hole I would start at about 688 RPM (90 SFM) and about .012 per rev feed, which would be about 8.25 IPM in this case. Your stock of .004 per side is pretty good. I usually shoot for .004-.006 per side.

I can't stress enough the importance of having a 'good' hole before you ream it. The reamer can only do so much and making sure the pre-reamed hole is good will insure consistency.

If he's double drilling he should be able to go with less
than .004 to .006 per side. The reason I say this is I often
have to make dull reamers work / last and the less they have
to cut the more they last. Ahhh...you learn so much working
in a small job shop which won't spend a penny on tooling,
machine repair, modern CAD/CAM, proper coolant upkeep, etc.

Of course I'm probably the only one that has to deal with this
situation. LOL :>)

jon

Hu I have seen your mention of using WD40 on several occasions, do you have good results on other machining uses?
In the firearm business I do my level best to see that no one uses it.
I do like the smell though:D

I was also kinda taken back at the slow speed and feed recommendations on the reaming of aluminum, having very little experience reaming I would most certainly have started much faster.

Thanks for the tips
Ken (Shea)

Originally posted by jonbanquer
If he's double drilling he should be able to go with less
than .004 to .006 per side. The reason I say this is I often
have to make dull reamers work / last and the less they have
to cut the more they last. Ahhh...you learn so much working
in a small job shop which won't spend a penny on tooling,
machine repair, modern CAD/CAM, proper coolant upkeep, etc.

jon


I think you are confused. What's this about a small shop?

Originally posted by Ken_Shea
Hu I have seen your mention of using WD40 on several occasions, do you have good results on other machining uses?
In the firearm business I do my level best to see that no one uses it.
I do like the smell though:D

I was also kinda taken back at the slow speed and feed recommendations on the reaming of aluminum, having very little experience reaming I would most certainly have started much faster.

Thanks for the tips
Ken (Shea)

Hi Ken,

No I don't like to use WD40, but I use it because it seems to work good with reaming. It can also keep a cutter from clogging when doing engraving or small endmill work in aluminum.

I hear it attracts moisture and causes rust after it evaporates. Is this why you do not recommend it?

To the group I have not had time to do testing for the reaming, got asked to work on another project, High Speed Machining of O-1, already talked to Hardmill and set me up.
Thanks again for all the info,Bill Johansen

"I hear it attracts moisture and causes rust after it evaporates"

You heard right Hu, it will absorb atmospheric moisture after a while, the higher the humidity the quicker it happens. It does make for a fairly good/cheap cleaner and flushes out rust well. WD40 is about 50 years old so its technology is outdated at best. I hear they manufacture 1,000,000 cans a week for the USA alone, pretty impressive actually but I will pick another product for firearms.

I'm trying to ream an accurate hole in a 1/4" thick 6061 Al pulley that I'm making. The finished hole size will be 0.500. How much should a leave for the reamer. Currently the hole is 0.478 which means the chucking reamer will have to ream 0.011" - is this about right? The work is being done in a lathe.

Thanks,

Bob