Reamer Feed & Speed in AISI 304

[Leandro]

I am not succesfull with the results when i use a reamer in Stainlesteel.

Cann somebody recommend me usuall feed & speed values for this material.

I will take a 1/4" reamer.

 

Thanks

[Sbarner]

My usual rule of thumb for reamers is 1/2 the speed and twice the feed as a similar size drill. I assume this is a high speed steel reamer? If it were me, I would probably run this at 400 RPM and 10 inches per minute. I would use oil, not coolant to lube the reamer. Also, what size of hole are you drilling to begin? Usually I use 5-10% less than the finish hole size, but in this case, I might take that down to 2-3%. Perhaps 15/64" drill. That's just me. I'm certain that others on the forum have a far better grasp on reamers.

[Dave.L]

quote:

---

I am not succesfull with the results when i use a reamer in Stainlesteel.

---

In size, finish, tool life?

 

Many factors influence the outcome of reamed holes. The amount of material to be removed by the reamer plays a HUGE factor and as I always preach, get the info from the manufacture of the tool, that's your best bet.

 

BTW, nothing wrong with oil but it's not always practical. We use coolant 100% of the time (soluable oil) and have very good results.

[Sbarner]

quote:

---

BTW, nothing wrong with oil but it's not always practical. We use coolant 100% of the time (soluable oil) and have very good results.

---

+1 Dave.

[Dave Perron]

From the machining data handbook.

 

this is is for cold drawm 304 ss 22-275 bhn ( to be safe, in the case of no certs)

 

Roughing reamer HSS 60 sfpm @ .005 ipr ( only if needed)

 

finish reamer carbide 50 sfpm @ .004 ipr

 

use water soluable and pre-drill to .242 ( c drill)

[jeff]

I never have any luck with reamers either.

I typically run them @ 50sfpm and around .004 ipr but they always ream about .001 oversize.

[Dave.L]

quote:

---

but they always ream about .001 oversize.

---

Maybe because the reamer is running out within the holder, hard to tell.

 

We have found that the amount of material the reamer removes makes a huge difference on the hole size outcome. Less is not more. As a rule of thumb, and only a rough guide, we find that reamers need approx. .005" per side.

 

Again, we always get the info from the tool manufacture.

[Bruce Caulley]

quote:

---

1/2 the speed and twice the feed as a similar size drill.

---

+1 I can never understand why some people treat a reamer like a boring bar.

 

As for size issues I have sometimes found that not leaving enough material for the reamer will produce an oversized hole. If I have dialed in the reamer and the drilled hole is straight and true and I am still getting an oversized hole I will reduce the drill size slightly.

 

Bruce

[Leandro]

Usually I am not succesfully in size.

Often I get slight oversize.

I agree with Dave the amount of material to ream made a huge difference.

Thank you very much for your suggestions.

[Justin Beebe at Folsom Tool]

I am reaming .192 diameter holes in 304 on a job now with great success. 750 rpm and 5.0 ipm . This is my process:

 

Drill to .177 diameter (4.5mm Guhring series 5514)

Plunge holes with a .1875 carbide endmill

Ream to .192 diameter with a 4 flute carbide tipped reamer

 

I am using coolant only and I made sure the reamer was indicated true. I usually like to leave a little more for the reamer but in this case it is working fine. When holding tight tolerances with reamers +-.0005 I usually order a few different brands and test them in a bridgeport to see what size they actually ream to before putting them in the machine

 

HTH

[horsepowered]

For a .250 reamer in 304 I would run 700 rpm with a 9.0 ipm feed and a .236 drilled hole. I make sure that the reamer runs true and let it hang out as much as possible from the collet face.

[mig]

horsepowered, you mean HSS reamer ?

[horsepowered]

Yes HSS

[jeff]

quote:

---

and let it hang out as much as possible from the collet face.

---

Same here.

[left coast lefty]

Check out the lead on the reamer and the chamfer of the drilled hole. Make sure the chamfer is slightly larger than the finish diameter.

 

quote:

---

We have found that the amount of material the reamer removes makes a huge difference on the hole size outcome. Less is not more. As a rule of thumb, and only a rough guide, we find that reamers need approx. .005" per side.

---

It depends upon the diameter. A .125 ream needs a .120 hole, a .50 ream is best around .484. I drill .0595 for a .0625 ream.

 

[ 02-19-2010, 05:35 PM: Message edited by: left coast lefty ]