Help achieving 32 finish turning 8620

J

Jay Fleming

Hot Rolled

Joined

Aug 7, 2014

Location

Noble, OK

• Feb 27, 2019

• #1

I've got Iscar CNMG 432 and VNMG 331 inserts available. I don't remember the grade or chip breaker right off. Buying new inserts right now isn't feasible. Part finished diameter is 6.35". If I take a .010 cut at the recommended .002 IPR, the finish feels smooth but is cloudy. This is at about 500 SFM. Do I need to turn the speed up? Increase the DOC? I can always sand the part if absolutely necessary but I'd rather finish in one step.

Thanks.

Sent from my SM-G960U using Tapatalk

 

K

kevin66

Aluminum

Joined

Apr 1, 2015

• Feb 27, 2019

• #2

I would bump the speed up to at least 800SFM and see what happens from there.

 

G

guest

Guest

• Feb 27, 2019

• #3

32 finish .0312 tnr .0056 ipr.

.0156 tnr .004 ipr.

Surface Finish

 

G

Guest

Guest

• Feb 27, 2019

• #4

I don't think your DOC is deep enough for the nose radius of your tool.

 

J

Jay Fleming

Hot Rolled

Joined

Aug 7, 2014

Location

Noble, OK

• Feb 27, 2019

• #5

I forgot to mention that I was using the VNMG 331 and got the bad finish. I'm going to a .020 DOC and .0035 IPR (.004 according to HSM Advisor is a 43 finish). We'll see what happens.

Sent from my SM-G960U using Tapatalk

 

J

Jay Fleming

Hot Rolled

Joined

Aug 7, 2014

Location

Noble, OK

• Feb 27, 2019

• #6

Ran the parts at 800 SFM, .020 DOC, .0035 IPR. The finish is magnitudes better than before but it still look like the material is tearing i.e. small specks in the finish. I only have these two parts, so I'm not worried about it anymore.

Sent from my SM-G960U using Tapatalk

 

D

Dan from Oakland

Titanium

Joined

Sep 15, 2005

Location

Oakland, CA

• Feb 27, 2019

• #7

try shutting off the coolant for the finish pass. 8620 tends to be gummy and this might do the trick. up your speed as well. run your coolant concentration higher if the no coolant does not do it.

 

J

Jay Fleming

Hot Rolled

Joined

Aug 7, 2014

Location

Noble, OK

• Feb 27, 2019

• #8

Disregard my last statement. The parts met spec but now they need to be thinner. I get to turn the OD again. I'll try Dan's suggestion on one and see. I'll probably use a new insert just to be safe.

Sent from my SM-G960U using Tapatalk

 

A

AARONT

Stainless

Joined

Feb 19, 2013

Location

Madison, WI

• Feb 27, 2019

• #9

I agree on uping the SFM. Do you have a profilometer to validate the Ra? You can have a cloudy finish and still be under a 32Ra.

 

G

Guest

Guest

• Feb 27, 2019

• #10

When I encounter gummy material giving surface finish issues my default is to finish turn with either a sharp tool or very small nose radius like .002-.005.

 

J

Jay Fleming

Hot Rolled

Joined

Aug 7, 2014

Location

Noble, OK

• Feb 27, 2019

• #11

AARONT said:

I agree on uping the SFM. Do you have a profilometer to validate the Ra? You can have a cloudy finish and still be under a 32Ra.

Click to expand...

No I dont. The first surface that had the cloudy finish ended up not being critical. It felt smooth to the touch, but probably a 63 or so. The second surface was and it turned out better. Due to a change, I have to redo both surfaces, so I have a shot at cleaning up the first surface too.

Sent from my SM-G960U using Tapatalk

 

litlerob1

Diamond

Joined

Nov 4, 2013

Location

Utah, USA

• Feb 27, 2019

• #12

.02" DOC is only .01" per side. That isn't enough. You need to be at minimum the radius of the tool. I usually go more though.

I realize you probably don't have that much material left now, but next time.

R

 

J

Jay Fleming

Hot Rolled

Joined

Aug 7, 2014

Location

Noble, OK

• Feb 27, 2019

• #13

litlerob1 said:

.02" DOC is only .01" per side. That isn't enough. You need to be at minimum the radius of the tool. I usually go more though.

I realize you probably don't have that much material left now, but next time.

R

Click to expand...

I meant .020 DOC radially, so enough for my .0156 radius. Now I have plenty, like .200 per side to get through, for my next operation.

Sent from my SM-G960U using Tapatalk

 

Orange Vise

Titanium

Joined

Feb 10, 2012

Location

California

• Feb 27, 2019

• #14

I'd be at 1000+ SFM in any annealed carbon steel, and as others have said, minimum radial DOC equal to the radius of the insert.

You can go even faster with cermet.

 

litlerob1

Diamond

Joined

Nov 4, 2013

Location

Utah, USA

• Feb 27, 2019

• #15

Jay Fleming said:

I meant .020 DOC radially, so enough for my .0156 radius. Now I have plenty, like .200 per side to get through, for my next operation.

Sent from my SM-G960U using Tapatalk

Click to expand...

For a Finish pass I would do 800-1000 SFM and .05" DOC, just for the Finish though. That would need a new corner, using worn corners and trying to get a good surface finish is like herding cats.

R

 

Q

qrovin

Aluminum

Joined

Jul 28, 2015

• Feb 28, 2019

• #16

How are you measuring the finish ?
I think first you need to measure what number your finish is currently at .

We did some 8620 recently and ran it at 750 speed at .004 ipr . Doc .02 and got we were getting under 32 finish .
Finishing tool was .016 radius tnmg .

I know some people will lynch me for that but it worked , finished 50 parts indexing finishing insert twice .

Mitutuyo profilometer is handy in this kind of jobs.

 

B

BSCustoms

Cast Iron

Joined

Dec 29, 2014

Location

WA

• Feb 28, 2019

• #17

you want to get the heat INTO the work for a finer finish. Heavier finish cut at a higher SFPM and slower feed.

you have enough info from those above to have good success. get after it.