Advice on Hard Reaming

Shop Supply Guru · Jul 30, 2020

As many of you know I sell tooling and I try to be a resource for my clients. I have good success selling Walter DC170 drills for drilling 50’s Rockwell material. This drill has no margin so it’s pretty tough. My client has had good success with these drills but now would like to try hard reaming. They would like to drill then ream a .1885” hole. The hole is a .500” through hole. So far I plan on drilling 4.7mm/.185” then reaming with a carbide reamer. Probably a Coated Harvey tool.

Anyone have advice or words of wisdom?

Orange Vise · Jul 30, 2020

What's the diameter tolerance?

How many holes?

Milland · Jul 30, 2020

I'd tell them to be ready to swap out reamers for resharp on a regular basis if this is a production job. I'd also reduce amount left for reaming to ~.005" or .006"/side, to lower torque. Coating shouldn't be too thick, sharper edges will cut down on force.

This might be an application for a CBN one-pass hone, especially if high production.

Scruffy887 · Jul 30, 2020

I thought Hard Reaming was for an apprentice that screws up to often. Silly me.

Fal Grunt · Jul 30, 2020

I have no experience with this on a production basis, so take this with a large grain (or bucket) of salt.

I was spoiled, most of our precision tooling had location holes or details wire edm’d or jig ground. However we occasionally had to improvise. I found that jig reaming, in the old school fashion, with a YG (?812?) or 5057 (I’d have to do some looking to refresh the numbers) yielded excellent results in both accuracy and surface finish.

I typically tried to use a tool with either a corner radius or chamfer.

This was a range of 54-68 Rc steels with a few 72’s thrown in.

macds · Jul 30, 2020

I know youre asking about hard reaming, and I have limited experience with it aside from for ejector pins. Not particularly excited about it myself.

If this is a production operation, and tolerance is important, I'd recommend looking into a burnishing tool.

Rick Finsta · Jul 31, 2020

I just used one of the Harvey units on a 44HRc production job following their speeds and feeds, and their stock allowance. 5mm Drill followed by a 0.1990" Reamer. Made all the holes to size but only 40 parts 1" deep.

Flash Gordon · Jul 31, 2020

I recently tried just what you described. Material 4140 heat treated to Rc 42.
Drilled .312 diameter with carbide drill, then reamed .3170 diameter by .25 deep using good quality carbide reamer.
This is a production job, running in a 40 taper HMC.
I got about 30 holes before the reamer started to cut undersize.
Didn't pan out for me.

Milland · Jul 31, 2020

Flash Gordon said:
I recently tried just what you described. Material 4140 heat treated to Rc 42.
Drilled .312 diameter with carbide drill, then reamed .3170 diameter by .25 deep using good quality carbide reamer.
This is a production job, running in a 40 taper HMC.
I got about 30 holes before the reamer started to cut undersize.
Didn't pan out for me.

That's a pretty small allowance for reaming (like the post above), you need some material to allow proper chip formation (which at the cut edge, involves some amount of "cracking"), too little and you start burnishing the cutting tool edges.

I guess some times it works (previous), and sometimes it doesn't (yours).

1953chevB · Aug 2, 2020

Funny I was re-training my self on ytube videos about reaming.
FYI
Your competition (Nachi) sells a high precision 3 flute carbide drill that can omit the reaming. I have no personal experience
So trial and error required.
I am not a reaming expert. I prefer to have parts hone or jig ground. But have had suppliers who have had good luck with using carbide helical flutes.
With the stock, feeds and speeds specified
On the manufactures catalog.
Half the RPM and feed of their drills.
Any low alloy steels like 4140 is know for toughness, any thing above 40 HRC
Is going to chew up tools.
Videos I watched were very informative
Slow the RPM entering the hole to prevent
Seizing or distorting.
Same exiting the hole. Turn off the spindle and retract. Pay attention to the feeds and speeds of the mfg caroling.

Shop Supply Guru · Aug 2, 2020

Thanks for your advice everyone. I found Komet has a series of reamers for hardened materials called Fullmax H. Looks like minimal edge prep on it. Seems like a large margin which makes sense.

I’ll let you know the results of this trial!

Shop Supply Guru · Aug 2, 2020

1953chevB said:
Funny I was re-training my self on ytube videos about reaming.
FYI
Your competition (Nachi) sells a high precision 3 flute carbide drill that can omit the reaming. I have no personal experience
So trial and error required.
I am not a reaming expert. I prefer to have parts hone or jig ground. But have had suppliers who have had good luck with using carbide helical flutes.
With the stock, feeds and speeds specified
On the manufactures catalog.
Half the RPM and feed of their drills.
Any low alloy steels like 4140 is know for toughness, any thing above 40 HRC
Is going to chew up tools.
Videos I watched were very informative
Slow the RPM entering the hole to prevent
Seizing or distorting.
Same exiting the hole. Turn off the spindle and retract. Pay attention to the feeds and speeds of the mfg caroling.

I sell Nachi tooling. They are an awesome brand not a lot know about. Particularly their powdered metal drills and carbide flat bottom series. Some of my clients have had amazing success in drilling small diameter holes on angled surfaces with their flat bottom series.

Hit me up if you need a distributor :cool:

woodsrider845 · Aug 2, 2020

O.k. At this point in life, it may be to little to late, but....

Don't lie to her. Be honest. I mean, she knows it's gonna hurt.

Have few drinks with her. Teach her some deep breathing.

Then spit and a running start.
Just make sure your aim is on point, for both your sakes.
....and we all know, after a hard reaming, your gonna come out of it with shit on your dick.

litlerob1 · Aug 2, 2020

Shop Supply Guru said:
As many of you know I sell tooling and I try to be a resource for my clients. I have good success selling Walter DC170 drills for drilling 50’s Rockwell material. This drill has no margin so it’s pretty tough. My client has had good success with these drills but now would like to try hard reaming. They would like to drill then ream a .1885” hole. The hole is a .500” through hole. So far I plan on drilling 4.7mm/.185” then reaming with a carbide reamer. Probably a Coated Harvey tool.

Anyone have advice or words of wisdom?

Reamers are for other stuff. Not stuff I do. Except ejector pin holes sometimes. There are different ways to get Round, Straight and on size holes, and do it faster, more consistently and with better location.

Is the customer stuck on Reaming? Or are they open to different approaches.

R

TeachMePlease · Aug 3, 2020

If I had to try that, I'd call MAFord and describe exactly what I wanted to do. Their reamers are pretty awesome, never tried to ream something that hard with them before, though: Series Display - M.A. Ford

Shop Supply Guru · Sep 1, 2020

We worked up a custom reamer with a left hand spiral right hand cut and it worked well for the application. My client got through the 20 holes needed for the job with one reamer and plan on using the reamer again for repeat jobs. We ran very conservative 30 SFM at 1.2 IPM. As a reminder this was a .1885” hole in 58 HRC 400 series stainless. We pre drilled at .185”.

RJT · Sep 2, 2020

I like carbide tipped reamers (instead of solid carbide) because they can withstand slight mis alignment. And use a good sulfur based cutting oil (not water based coolant).

Mtndew · Sep 2, 2020

Boring with CBN isn't an option?

Advice on Hard Reaming

Hot Rolled

Titanium

Diamond

Titanium

Titanium

Hot Rolled

Stainless

Aluminum

Diamond

Cast Iron

Hot Rolled

Hot Rolled

Hot Rolled

Diamond

Diamond

Hot Rolled

Titanium

Diamond

Similar threads