Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

316 Stainless Plate


Recommended Posts

Does your stock have scale on it. if so cut flip cut flip rinse repeat until stable.

if the is not working I have had luck using 1/2 carb end mill dynamic milling aprox. 10% step over high speed style. sounds insane but doesnt seem to put stress in the material.  I think I was around 600 sfm 50-100 ipm ?

  • Like 1
Link to comment
Share on other sites

Double disc would be my 1st thought. Milling this would require a lot of back and forth flipping and such to make sure you were doing what you could to get the stress under control. Running it through a double disk machine will make it flat and give an awesome finish.

Here is one company that comes to mind: TCI Precision

 

  • Like 4
Link to comment
Share on other sites

That is a tough thickness to width ratio to keep flat in 316. Removing the scale on this plate really gets it moving all over the place, so you need to start with at least .375-.5" plate, machine the scale off and leave about +.04-.06" per side and let it warp, and then start working your way down to final thickness.

Grinding is tricky with 316; the reason 316 is usually used is for corrosion resistance, grinding will impregnate the material with iron that is embedded in the grinding wheel and coolant from working with ferrous materials. If you go the grinding route you will need to send the parts out for passivation, or you will learn that 316 can in fact rust.

  • Like 3
Link to comment
Share on other sites
1 hour ago, cncchipmaker said:

Our shop is having a very hard time keeping a .25 plate 17 inches in diameter from relieving itself and springing. Any thoughts on how to machine this stuff? Must be flat within .01 and keep within a .004 thickness tolerance.

What is the final thickness you need to be at?

What is the starting thickness before machining?

Cut/flip/cut/clip lather rinse repeat is usually the way to go.

Link to comment
Share on other sites

Grain flow is 90 degrees REALLY against you. Ask the guy who quoted it what he had in mind for a method...

Flip and flip and I'm thinking mill the thing on a vac table - this will eventually get you your parallelism. Cut it with high rake carbide but small diameter so not to stress the thing worse.

As for whether it will stay flat to 10 thou though is anyones guess I'm afraid.

  • Haha 1
Link to comment
Share on other sites
2 hours ago, Newbeeee™ said:

Grain flow is 90 degrees REALLY against you. Ask the guy who quoted it what he had in mind for a method...

Flip and flip and I'm thinking mill the thing on a vac table - this will eventually get you your parallelism. Cut it with high rake carbide but small diameter so not to stress the thing worse.

As for whether it will stay flat to 10 thou though is anyones guess I'm afraid.

You made a funny the person that quoted it was thinking it was a 5 minute job. 🤣  🤓  🕵️‍♂️

  • Like 2
  • Haha 1
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...