Sign in to follow this  
jeff

Invar 36--gravy or nightmare?

Recommended Posts

We have some parts to turn and maybe mill out of this stuff. Any tips for general turning and milling/drilling? 

 

Share this post


Link to post
Share on other sites

It is just abrasive and tough, but machinable. Use recommend SFM and I would start at .01 for roughing per rev on turning and .003 for finish turning. For milling .0015-.003 per tooth and start with 5 flute tools can even go up to 9 flute tools if you need to go real deep with some cuts.

  • Like 1

Share this post


Link to post
Share on other sites
5 minutes ago, 5th Axis CGI said:

For milling .0015-.003 per tooth and start with 5 flute tools can even go up to 9 flute tools if you need to go real deep with some cuts.

That really depends on tool size...though doesn't it always.

I've had to mill slots with .012" endmills..... 3x's deep.....let's just say we went through A LOT of tools to get that order done....

Saying you need to machine it is just such an open ended question in my experience...

 

Share this post


Link to post
Share on other sites

I just saw the print, and it's just a turning job, some pins that are 4-5" long and have a journal the majority of the length with a #8-32 thread at the end.

Stock size is 1-1/4" dia or so

Share this post


Link to post
Share on other sites
56 minutes ago, JParis said:

That really depends on tool size...though doesn't it always.

I've had to mill slots with .012" endmills..... 3x's deep.....let's just say we went through A LOT of tools to get that order done....

Saying you need to machine it is just such an open ended question in my experience...

 

Yes, but just throwing something out to see what sticks. 😉

  • Like 2

Share this post


Link to post
Share on other sites

Thanks guys, we're going to use Sandvik grade 1105? and start around 175SFPM. 

Oh and these get knurled too. That should be fun.

Share this post


Link to post
Share on other sites
2 hours ago, jeff said:

Thanks guys, we're going to use Sandvik grade 1105? and start around 175SFPM. 

Oh and these get knurled too. That should be fun.

1105 is their "generic grade". It is going to wear quickly more quickly.

I much prefer their 1125 grade. It is superior for "harder materials", but the 1115 grade is also good.

Entering Angle can be used to help control chip thickness. A 45 degree entering angle, or less, is good if you have the option to specify. If you use a typical CNMG style 80 degree insert with 5 degrees of side clearance, then your entering angle would be 85 degrees. But often based on part geometry, we don't have that luxury.

If you opt to rough with a round insert, you can use the Dynamic Turning path to get better tool life, and faster metal removal. Plus, depending on your settings, you can use the Chip Break function to keep the chips from wrapping on your tool or part/spindle.

  • Like 2

Share this post


Link to post
Share on other sites

image.thumb.png.d5ac10ca30d29d9e2af71a030b6c86c1.png

This is a calculation for a CCMT Insert, with .031 Corner Radius.

I was trying to get the SFM below 680, but the calculator was giving me grief.

I would think 200-400 SFM would be a good starting point. You might need to get it up to higher SFM values, in order to get the heat into the chip. You'll also want to be sure you are taking a big enough DOC that you're hitting the chip breaker.

 

  • Like 1

Share this post


Link to post
Share on other sites
14 hours ago, Colin Gilchrist said:

1105 is their "generic grade". It is going to wear quickly more quickly.

I much prefer their 1125 grade. It is superior for "harder materials", but the 1115 grade is also good.

 

It could be the 1125 grade, (I'm a mill guy). I was relaying information to our lathe operators.

  • Like 1

Share this post


Link to post
Share on other sites

We use 1025 for sandvik

 

Free machining is not bad

Class 7 stinkums. I try not to drill it

Share this post


Link to post
Share on other sites

On the drilling and tapping side, solid carbide drills 100 sfm .001 per tooth, 30% peck depth. Tapping; Form tapping works the best for Invar. 15/20 sfm coated forming tap.

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
Sign in to follow this  

  • 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