[hall6ppc]

Need some advise on machining 17-4 PH SS condition A ( 35C Hardness), I have a job to machine out of this material .This is a mill job that will be done on a HAAS VF-1. What is a good SFP to run a carbide end mill (.500) at ?

Thanks

[stevo1]

I would start in the range of 200-230SF and .001-.003chip

It's not the fastest but we were mainly concerned with tool life.

Stevo

[Mr Dontech]

check this out.

http://www.whitney-tool.com/assets/PDFs/35.pdf

hope this helps
Steve K.

[cdlenterprises]

35 HRc sound real hard for 17-4 condition A. That level hardness is usually acheived at an H1000 or H1050 condition. i would double check the material specs and make sure you know exactly what you're cutting. We run a lot of 15-5PH H975 which is 36-38 HRc. We'll regularly run coated carbide ball end mills at around 425 - 500 sfm for 5-axis contouring.

[hall6ppc]

35 HRc sound real hard for 17-4 condition A. That level hardness is usually acheived at an H1000 or H1050 condition. i would double check the material specs and make sure you know exactly what you're cutting. We run a lot of 15-5PH H975 which is 36-38 HRc. We'll regularly run coated carbide ball end mills at around 425 - 500 sfm for 5-axis contouring.

I am not exactly sure what the condition is but I do know that the engineer that I am doing the work for says it will be from 35 to 37 RW c . I will be using un coated carbide to do the milling . Most of the cuts will be facing cuts and side milling cuts . How much would you reduce the sfm for uncoated carbide? Also I will be using cobalt m42 drills for the holes do you have any suggestions for them ?

Thanks for your help !!

[hall6ppc]

check this out.

http://www.whitney-tool.com/assets/PDFs/35.pdf

hope this helps
Steve K.

Thanks Steve this helps ALOT !!

[little bubba]

35 HRc sound real hard for 17-4 condition A. That level hardness is usually acheived at an H1000 or H1050 condition.

I don't know why they call it annealed, its not, its solution treated, ready to be precipitation hardened, and yes it is that hard in the annealed/solution treated condition.

My suggestion, get it heat treated first, 17-4 in an H1150 increases its machinability by about 50%. In the annealed condition it is gummy and nasty and acts sort of like 304, but more manageable. Heat treated it actually acts more like a heat treated 4xxx. The gumminess goes away, it doesn't stick, machines very well dry, doesn't work harden like a 3xx stainless.

Even if you need it heat treated to an H900, which is mid to high 40s on the C scale, it will be easier to machine than when its annealed/solution treated.

Don't be scared of it, its a wonderful material, machines very well. Heat treated, treat it like an alloy steel. It will give you beautiful finishes.

Uncoated carbide, annealed, 200sfm wet, drill 30-40sfm.

Heat treated, (don't know what HT you might have) 200-250 sfm dry. drill 40-60sfm.

Coated carbide on HT material, 275-375 sfm. Inserted facemill I'd push into the 450-500 range.

Make sure you know exactly what you are working with, makes a lot of difference, even if you have to smack the engineer upside the head.

[hall6ppc]

I don't know why they call it annealed, its not, its solution treated, ready to be precipitation hardened, and yes it is that hard in the annealed/solution treated condition.

My suggestion, get it heat treated first, 17-4 in an H1150 increases its machinability by about 50%. In the annealed condition it is gummy and nasty and acts sort of like 304, but more manageable. Heat treated it actually acts more like a heat treated 4xxx. The gumminess goes away, it doesn't stick, machines very well dry, doesn't work harden like a 3xx stainless.

Even if you need it heat treated to an H900, which is mid to high 40s on the C scale, it will be easier to machine than when its annealed/solution treated.

Don't be scared of it, its a wonderful material, machines very well. Heat treated, treat it like an alloy steel. It will give you beautiful finishes.

Uncoated carbide, annealed, 200sfm wet, drill 30-40sfm.

Heat treated, (don't know what HT you might have) 200-250 sfm dry. drill 40-60sfm.

Coated carbide on HT material, 275-375 sfm. Inserted facemill I'd push into the 450-500 range.

Make sure you know exactly what you are working with, makes a lot of difference, even if you have to smack the engineer upside the head.

Thanks for the info, I machined the parts with the speed you recommend and all went well !

[leggazoid]

http://www.widia.com/images/widia/pd..._EN%28f%29.pdf

Check this out!