Reaming

[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

[HuFlungDung]

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.

[E-Stop]

.....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!

[jonbanquer]

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

[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

[Rekd]

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

[Bill]

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

[woodsmith]

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

[Rekd]

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??)

[woodsmith]

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

[HuFlungDung]

Oh, the reamer has to be perfectly sharp 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.

[creative_mind]

What's a floating tap holder?