What's new
What's new

Face milling Super duplex split pump casings

msayani2

Plastic
Joined
Feb 9, 2015
Location
United Arab Emirates
We have some new jobs in our shop for machining of split pump casings. We have to face, drill and then threadmill these parts.

Currently we are facing major issues in face milling. We run a 100mm/4" Sandvik R390 cutter with 2040 grade R390-17 sized inserts with 1.6 mm corner radius.

The material is Cast Super Duplex Stainless Steel. Any one have experience facing these types of parts? Our tool life and speed is very less.. VC is close to 30m/min and Fz = 0.15mm/tooth.

I was thinking of using a positive rake round button inserted tool(with single sided inserts) so that i would get more edges and high tool life.

Anyone have any experience which tool brand and grade is best for this kind of application?

Also, note that after drilling and facing, we do some pressure testing, after which we need to further remove 0.001 in off the face prior to delivery.
 
I'm glad it's not me!!

You're going to struggle using a Facemill into cast Duplex. I might try using an Endmill to get under the cast surface. But I think using round inserts is a great idea.

R
 
If i was to be facing super duplex. I'd have a 45degree approach tool not a 90degree.
id be trying 80m/min about .12-.15 a tooth for starters. With a good 2.5mm plus depth of cut (to get under the skin)
With a tip check after each pass.

This is with a WNT tool and 2135 grade tip, see below.

Zerspanungswerkzeuge | WNT Online Shop
 
I machine 2205 & 2507 super duplex quite often and I have the same RA390 except in 25mm/1" with same grade inserts and I've had terrible experience with it, even on SS316.

So anyways, as the other guy said, you may need to go to solid carbide. I know it sounds nuts, but if it is feasible (based on part size) I'd recommend solid carbide.

My goto is YG1 V7 INOX end mills. I use same feeds/speeds as they recommend for stainless (315 sfm) and I get great tool life. Be sure your depth of cut is high enough to get under the surface.

For plate/bar (not cast) parts, we use a Mitsubishi WSX 3" facemill with MP7140 inserts. ap 1.6mm - 2mm at 550sfm. We've had no luck on cast duplex with these inserts.

For drilling, I've given up on conventional drill bits. I've tried all the big brands, but it is just not worth the risk of an expensive drill bit breaking inside of an expensive super duplex part. I use 3 flute Kennametal GoMills and just helix bore the hole. One 1/4"/6.3mm 3 flute end mill costs me ~$15 and can make hundreds of holes in 2507. Compared to a $90+ drill bit that will fail catastrophically when no one is looking.

However if your mill has the torque & rigidity and you need large holes drilled, then go with ISCAR DR drills with 808/908 grade inserts. This is what I use on our lathes, last count we got about 200x 1"/25mm holes at 2"/50mm deep. That's 15 meters for ONE insert edge. Feeds/speeds are exactly as recommended by ISCAR for M3 austenitic/martensitic stainless. This is done on a 20hp/15kW lathe with 10bar coolant.

If you try this on a 40 taper mill, you will crack those inserts really quick. Most 40 taper VMCs do not have the Z axis thrust force to maintain a constant feed rate.
 
Hey There, I had the same issue, i work with castings all day . All sort of types of materials. We switched to sandvik about a year ago and it was a great improvement except on the duplex/stainless. We figured out that S40T Grade is the best for duplex we run it dry with about 100 vc m/min with 0.2mm a teeth and it easily cuts 3-5 mm deep with 70 % of the cutter engaged , Depending on fixture of course.. but its a great we have super long tool life and super finished . We use this grade in the R390 with 0.8 radius( 20mm till 80mm ) and we use the r245 and R 345 Face mills also with the same grade. Hope this will help you out!.
 








 
Back
Top