Reaming Speed???

[Brendan P]

I come up with 550 rpm and 8.25 ipm

45 sfm

[Müřlıń®]

quote:

---

How 'old school' is old school? I've been running reamers that way since the early '80s.

---

.....late 70's.

[Sai]

Brenden How did you calculate the speed and feed. Is there some kind of formulae???

[chris m]

(3.82 x SFM)/dia = RPM

 

IPT (inches per tooth) * # of teeth * RPM = IPM

[Sai]

what is 3.82 ?? What will the formulae be for AL ans Stainless Steel?

[Thad]

3.82 is a constant for all materials.

 

Thad

[chris m]

The formulae are the same for all materials, the Surface Feet per Minute is what changes based on workpiece material, cutting tool material, type of operation, etc

[Brendan P]

I use a cd rom program that I purchased a while back from a company called Cut data.

But thad and chris are right.The sfm is what counts between naterials

[TFesta]

( Allan )

The rule of thumb I was taught in my apprenticeship days was half the speed(rpm) and twice the feed(ipm).

-----------------------------------------------

 

Thumbs up Allan, that all ways works.

[billystein]

I don't think you can go too slow on rpms, I normally start reamers at 100-200 rpm no matter what the material. feed at 2-3 for harder matals, 5 for aluminum.I will also use g81 cycle. the longer the reamer stays in the hole the more it takes. also I have never indicated a reamer.the reamer will follow the existing hole.

if you do it this way and it still comes out oversize it usually means the reamer is bent.

billy

[Joel Walker]

Stop the spindle at the bottom of the hole before you take it out,it will hold size better, and the tool will last longer.

 

I agree with TFesta on the feed and speed

[Joel Walker]

Sorry I agree with allen, no offence TFesta (LOL)

[ChuckM]

I'm with Psychomill and Murlin in that I always run them on the "faster" side. Or so I've been told.

 

In 1018 I'd program 70-80 sfm (856-978 rpm) and 2-3 times the feed of a good HSS drill. In this case, anywhere from 10.7-18.3 IPM. I'd probably opt for a letter "N" drill (.302).

 

In a production setting I'd start on the high side and see what happens. If I can nail the size and the finish is acceptable, then that's what I run. Either that, or I try pushing things a little harder to see what the limit is. I can't imagine reaming a number of holes in a production setting at 3-4 IPM.

 

Sai,

I have a formula I use for reaming. It's not based on anything scientific but it hasn't failed me yet. At least... it gives me a baseline to start from.

 

non-ferrous brass, aluminum, etc., I use a feed constant of .024

 

mild steel .020

 

high strength alloys, etc., .016

 

Easy enough to remember?

 

I then take the drill diameter and multiply it by the constant, then multiply that value by 2 or 3 (2-3 times drill feed). That will give us our feed in IPR. Multiply that by the rpm.

 

3/8 reamer in 1018 @ 70 sfm = 713 rpm

.375 x .020 x 3 = .0225

713 x .0225 = 16 ipm

 

Then I go up or down in feed from there.

 

-Chuck

[CAM-mando]

quote:

---

2/3 drilling RPM and 2-3 times drilling feed.

 

It is a reamer not a boring bar.

 

Bruce

---

I'm with the Shark

[jeff]

I use the ME Consultant for all my hss drilling and reaming speeds n feeds.

Works great.!

I think it's on the FTP.