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:

index drill on a lathe


Recommended Posts

6 minutes ago, JParis said:

It's slow, I know...hopefully as it settles in you can start bumping it up...

316L typically isn't bad but yeah, I have had some rough times with it on occasion....usually it's "where" it's made...

🇨🇳 When I worked for trueline valve corporation, the buyer told me it is cheaper to buy a completed part from china, than the cost of the Material here, but the Material quality is not the same.

Link to comment
Share on other sites
17 hours ago, Rocketmachinist said:

What am i doing wrong when drilling with indexable drills on a lathe. I am using through coolant and all the speeds and feeds from the book. Also no pecking, but still I blow up an insert about every hole. 316L stainless, 3/4 inch walter drill.

What indexable drill? This could have a big impact on speeds and feeds.

Link to comment
Share on other sites
  • 2 weeks later...

Unless you have a really light edge prep on the insert, you are just barely feeding enough not to rub.  I'd be starting at about 0.004" - 0.005", and trying not to exceed about .008" in 316.  But that will depend mainly on the insert.  There will be a sweet spot with the feed rate that will be recognizable by the way the chip curls.  You surely know what to look for there.  If it isn't breaking you need a different insert topology.  Life will be dramatically better regardless of surface footage if you are making a proper chip.  Once you get a good chip you can start to tune the spindle speed for productivity.

JP's recommendation to slow down is a good one.  But depending on the insert grade, 85sfm is too slow and might cause built up edge.  I'd start at 125SFM.  I've found if you can't get a reliable process at least 125 SFM in most of the common stainless materials with carbide.  Something other than the tool and its parameters are the problem and you need to start looking for a workaround...  Unfortunately, the tool and operating parameters are typically all you can change..... so after you have verified your setup is good and your turret is running on center (drilling off center on x is ok, but excessive y will blow it up every time) then it's time to go hunting for parameters that get the job done.

Take a cut, and get it out of the cut before it fails.  Examine the inserts for signs of chipping or excess heat.  If too much heat and you are say around .006" ipr, slow the sfm down.  If it's chipping, either it's instable and bouncing around and you need more feed, or it's not hot enough and you are getting built up edge at which case you need more sfm and very possibly a little more feed to generate just enough heat in the cut.

Ideally with a insert drill like that you want to create just enough heat that the center insert doesn't chip out, but the outside insert isn't burning up.  Typically I will spec a tougher grade for the inboard insert and a more wear resistant grade for the outboard insert.  If you are using the same insert for both, lean toward the tougher grade, all you will sacrifice is life and overall productivity, but it should be stable/reliable.

Oh, one last thing.  You can't have too much coolant with these drills.  Higher the concentration the better typically.  They typically have large coolant holes and most pumps / delivery lines don't do them justice to get any pressure at the flow rates they allow.  At 3/4" it shouldn't be bad.  But when you start getting around 1.5" and larger, a 3/16" or 1/4" copper line isn't really optimal....

Happy holemaking.

  • Like 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...