Dan_AKA_ROY

304 Stainless Steel

Recommended Posts

Any suggestions (tips)? First time I ever cut this stuff.

 

I'll need plenty of coolant flow, watch for tool wear..that I know.

 

I'm machining (milling) a cylinder stock, 6" diameter, 4" height. Will machine down 3" then pocket thru the bottom (1" material). I'll machine at least half of the stock off.

 

I'll use 1/2" flat 4 fluter for the bottom pocket, and 1/2" ball 4 fl. for the material above the pocket (carbide endmills) (will use rough and finish surface parallel toolpaths, appr. 30 deg walls)

 

MC is giving me 1.5632 IPM at 977 RPM for the 1/2" ball, 2.444 IPM at 1,222 RPM for the 1/2" flat. Right now I have depth cuts at 0.125" deep with a 75% stepover for the 1/2" flat, and 0.15" depth cuts 0.4" stepover for the parallel rough using 1/2" ball. Takes a lot of machine time, might need the lower the stepover to 0.25"?

 

Kinda using an educated guess.

 

And what would you suggest for the plunge rates? I'm going with 1.5? Don't have ramp or helix entry options for the parallel rough toolpath..

 

Any input would be appreciated!

Share this post


Link to post
Share on other sites

a variable helix end mill and use a dynamic toolpath with no coolant , just air blast.

This is one of the best way to cut this sticky stuff , i cut 304 flame cut about everyday here and this is the best way

 

run the EM at about 3000RPM and 60-80 IPM at 10-12% stepover

and the BM at the same speed but at 7-8% stepover

 

this will get the job done much faster than your numbers ;)

Share this post


Link to post
Share on other sites

Thanks Goldorak,

 

However, 1.) Our VMC doesn't have air blast setup, though we could improvise (our routers use air). 2.) I'm on X2, hence no dynamic toolpaths available.

 

But good advice! Much appreciated! I believe we're gonna upgrade soon (buying a Wire EDM soon)

Share this post


Link to post
Share on other sites

you should be able to get the same speed with surface rough parallel

 

 

for the air , on our mazak VTC200 we simply tie an air hose to the spindle with a ball valve next to the control

 

then add a program stop to turn it on and off

Share this post


Link to post
Share on other sites
run the EM at about 3000RPM and 60-80 IPM at 10-12% stepover

and the BM at the same speed but at 7-8% stepover

 

Gotcha. I'll do that! The speeds and feeds given in MC are dog slow, 15 hour rough cut. :blink:

 

What about stepdown? I'm guessing with a smaller stepover, I can go deeper - say 0.2"?

 

What about the first pass when the tool fully engages in the material? How would you do that? Increase "Adjustment to top cut" in the Cut Depths tab?

Share this post


Link to post
Share on other sites

Gotcha. I'll do that! The speeds and feeds given in MC are dog slow, 15 hour rough cut. :blink:

 

What about stepdown? I'm guessing with a smaller stepover, I can go deeper - say 0.2"?

 

What about the first pass when the tool fully engages in the material? How would you do that? Increase "Adjustment to top cut" in the Cut Depths tab?

 

 

i will set it to the maximum tool flute length, don't be afraid of it, the toll will survive :D

just pay attention to the first pass, many times you got to extend the starting surface to avoid to get a 50% step over on the first pass

Share this post


Link to post
Share on other sites

Yep.. That sounds right.. I started using the IMCO M525 Enduro endmills and get a lot better tool life.. I cut 304 all day..

 

Except I do use coolant... With the Enduro 5 fluter I'm running a 1/2" at 3050 RPM and 105 IPM.. 1.25" depth of cut... 10% stepover..

 

The dynamic contouring toolpath is just awesome.. I love it.. It's changed everything in my shop.. Cycle times are way down. Tooling costs are way down..

Share this post


Link to post
Share on other sites
The dynamic contouring toolpath is just awesome.. I love it.. It's changed everything in my shop.. Cycle times are way down. Tooling costs are way down..

 

What he said above. Roy upgrading to x5/6 with dynamic toolpaths and opti-rough will pay for itself in no time. See my sig for what folks are running 304 at.

Share this post


Link to post
Share on other sites

What he said above. Roy upgrading to x5/6 with dynamic toolpaths and opti-rough will pay for itself in no time. See my sig for what folks are running 304 at.

 

 

i can say that we cut around 33% of tooling cost and cut about 25-30% cycle time per part when we compare conventional method and dynamic method

 

the optirough by itself can cut the programming time by 75-80% for the roughing portion

Share this post


Link to post
Share on other sites

First time ever cutting 304 SS?

It can go smoothly, or it can go bad, and when it decides to go bad, it will go fast lol.

 

Hanita Varimill's love 304SS, give them a try.. you said that you don't have air blast, so flood coolant and make sure its a constant blast, not intermittent otherwise it will gum up on the tool in a hurry,

You can use HSS drills easily, but need to run them about 50% as fast as say 1018,but of course carbide is the way to go.

Share this post


Link to post
Share on other sites

it can go bad, and when it decides to go bad, it will go fast lol.

 

when this happen, you get a nice stainless mushroom melted to the end mill in about 3-4 seconds :D

Share this post


Link to post
Share on other sites

when this happen, you get a nice stainless mushroom melted to the end mill in about 3-4 seconds :D

 

Yep, and it's a nice red glowing ball of fire.

Share this post


Link to post
Share on other sites

Yep. They are awesome (dynamic toolpaths). I've been experimenting with them at home (X5 HLE).

 

I think we are going to upgrade very soon, but that doesn't help right now. They're looking into purchasing a Wire EDM, so I got the quote for the add-on cost and also for upgrading (on X2 mill L3 now).

 

I'm gonna try different approaches, different toolpaths and see how it goes. Too busy with other stuff now, so I'll have to wait till late afternoon. With the parallel toolpaths, the bit would fully submerge during the first passes.

 

Endmills coming today, tomorrow at the latest. 4 flute helical EM and BM's. I am a bit concerned with the flooding. No enclosure on our VMC and I have to watch to make sure the flood pressure doesn't decrease.

 

Thanks for all the advice. I'm taking a close hard look!

Share this post


Link to post
Share on other sites

Down & dirty: This may break a few safety rules but a Mag base on the side of the spindle will get you a quick air blast set-up. A split bushing or shims may be required to lock the tubing. A few strategically place coat hangers to to hold the air line up and pay attention to those tool changes.

Share this post


Link to post
Share on other sites

Resurrecting this from the past :)

 

I am working with 321 SS and it has given me nothing but headaches and melted tools. How similar in machining concept, speed, and feed can I be to what was discussed in the above posts?

 

I was going to go ahead and try a variable helix, 4-fl, carbide E.M. at S3000, F70., step over .050", DOC .750" People said this worked well on 304 and I am reading that they are similar to each other with the exception of Ti being added to 321.

 

Also, while on the subject. I know you have to get a nice, deep, radial cut to keep from generating heat and work hardening. I can do that for pocketing and roughing but what about surface finishing? I cannot have a large stepover due to surface finish requirements and I am afraid of heating up the tool while removing a little at a time.

 

Thanks for any and all help!

 

Lans

Share this post


Link to post
Share on other sites

well if the part has geometry inducive to really burying the cutter consider dropping down to a HSS corn cobb rougher.

1. wear will be very predictable.

2. MRR will be good depending on how well tools can be buried in material. some instances can beat the pants off "high speed" methods.

3. no chipping or breakage as with carbide.

 

sometimes "slower is faster". if you're just trying to get through a few parts, this would be my method

Share this post


Link to post
Share on other sites
and I am afraid of heating up the tool while removing a little at a time.

the beauty with HS method's small stepovers is you have small angular engagement which gives less time to heat-up.

 

F70. might be too slow@3000rpm.

maybe F100. (how many flutes?)

 

check Rizzo's database. that stuff WORKS!!!

Share this post


Link to post
Share on other sites

the beauty with HS method's small stepovers is you have small angular engagement which gives less time to heat-up.

 

F70. might be too slow@3000rpm.

maybe F100. (how many flutes?)

 

I am using a 4-fl variable helix E.M. F70. @3000 is SFM of 393 and IPT of .006". Going up to F100. puts it at IPT .008". Were you referring to the ball tooling only at F100? Or the roughing E.M?

 

Thank you !

Share this post


Link to post
Share on other sites

The stainless section of Rizzo's database lists speeds and feed in the 5000rpm and 50-100 ipm range, mostly showing use with coolant. this is at 10-15% stepover.

looks like my 100ipm@3000 would be too optimistic for your 4 fluter......

 

make sure your variable helix tool has some tip treatment; either a chamfer (hanita varimill) or corner radius

Share this post


Link to post
Share on other sites

.050" radially on a .500" endmill might be a bit aggressive, although you didn't mention diameter.

if this is the size, don't be afraid to drop down to the .02" stepover. A reduction here is your safety-net.

Share this post


Link to post
Share on other sites

Those sfm those guys are running are pretty high, but everyone is about the same. Also 10% (.050) seems standard. Goldorak has a ton of experience with this I know. Check out his comments.

 

IMHO you gotta use feed override to really tune it in. Don't forget to enter your results into the form (in my signature).

 

Thanks fellas!

Share this post


Link to post
Share on other sites

Thank you again mkd!

 

I am in fact using a .500" E.M. Looks like I will go S3000, F70, S.O. .030" on the roughing, square end.

 

F100. S5000 S.O. .010" on the ball finish tool. Crossing fingers!

Share this post


Link to post
Share on other sites

Those sfm those guys are running are pretty high, but everyone is about the same. Also 10% (.050) seems standard. Goldorak has a ton of experience with this I know. Check out his comments.

 

IMHO you gotta use feed override to really tune it in. Don't forget to enter your results into the form (in my signature).

 

Thanks fellas!

 

Thanks a ton!

Share this post


Link to post
Share on other sites

FWIW... These parameters rocked it! F70.0 IPM, S3000 RPM, .050" Stepover, .750" DOC. Ran through all of our parts on one E.M. and did it much faster than previously.

 

Thank you for the help guys!

  • Like 1

Share this post


Link to post
Share on other sites

i ran a batch of parts in P20 (slightly hard 4140) on one .500" guhring endmill. All after i'd been roughing copious amounts of aluminum with that cutter.

 

140ipm and 5300rpm in P20, thank to Rizzo's database.

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now


  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us