danielm

Titanium spd/fd for HSM request

Recommended Posts

Can people please chime in with cutter type and spd/fd combinations for peel mill or z-level milling of 6al-4v that they have found to work well?  I've looked at the dynamic database and there's just not a whole lot there.  

I feel like asking for this kind of info may be dangerously close to asking for a post considering how delicate it is to get Ti to cut just right.  Me personally....I'll put up anything that I've found to work really well.     *I am using one 1.25 insert cutter and solid carbide  .500" (flat) down to .250 ball.

**Is anyone using ceramic for 6al-4v?

Thanks in advance!!

 

 

 

For you guys that are rocking Inconel....this one's mine:

We run a 718 Inconel job faster than I've seen anywhere.

 

Here's the recipe:

1) 1.25dia X 3flt Kennemetal Facemill (.25rad inserts)

2)Kennematal ceramic inserts: KIPR125RP43540

3)4584 RPM and 41.25 IPM.

4).100" axial cut

5)Full dia cut

6)Run dry!

 

Oh yes..

 

7)50 taper horizontal mill.

 

You will see the prettiest color of orange-red chips spewing off the cutter. The work doesn't get hot and you get great cutter life.

 

  • Like 2

Share this post


Link to post
Share on other sites

I'm cutting Ti6Al4V bone plates on a Haas VF-3SS with a trunnion, CAT40 15KRPM.  I rough with a Helical 3/8" 7 flute 3/4" LOC .020 radius (HEV-SR-70375-R.020), 3" shrink fit holder, 3540 RPM, 146 IPM, .025" stepover.

I'm going to be running a comparison soon, between that, some new Helicals with a new coating, and some Kennametal Harvi III cutters.  I'll report my findings when I have them.

 

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites

200% depth of cut 450 sfm .005-.006 per tooth with 6 or 7 flute tool and 7% step over. Hydraulic Chuck and 1000 psi on good solid fixtures. Average of about 300 minutes of tool life. Melin VXMG7-1616 .03R with nACRo coating has been holding up better than the Harv III for one customer we have.

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites

With Ti, I like to make sure the cutter is taking a chip. I like Ron's numbers. Sweet spot is 5-7% radial engagement. Make sure you are leaving that 5% radial value as a finish pass amount. Get lots of flutes. 7, 9, 11, I've even seen a 19 flute tool that is supposed to be engineered for HEM cutting of Ti.

Really pay attention to maximizing flute length. 2 : 1 is optimal.

450 is aggressive for Ti, but that's the advantage of the HEM technique. If you experience issues, drop SFM first, before dropping the feedrate.

For super simple starting points, use 400 SFM, .005 per tooth, and 5% stepover. That should work with almost any decent "off the shelf" carbide tool.

Since you're taking advantage of Chip Thinning, the easiest way to speed the process up is to increase the number of flutes.

  • Thanks 1
  • Like 4

Share this post


Link to post
Share on other sites

This is great information.

Thanks for sharing !

  • Like 1

Share this post


Link to post
Share on other sites

I'll play :)

For a while my go to cut strategy in Titanium with a .750 5FL Helical brand end mill  (1.62 LOC, .12R)  has been:

8% Step over, up to full step down,  525 SFM, .0045 chip load ( 2676 RPM, 60 IPM).

  • Like 1

Share this post


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

I'll play :)

For a while my go to cut strategy in Titanium with a .750 5FL Helical brand end mill  (1.62 LOC, .12R)  has been:

8% Step over, up to full step down,  525 SFM, .0045 chip load ( 2676 RPM, 60 IPM).

How many minutes will the tool hold up before needing to be replaced?

Share this post


Link to post
Share on other sites

>>>How many minutes will the tool hold up before needing to be replaced?

 

Cutter life is a big deal for this customer.  Also they are very concerned about over working a 40T spindle and premature spindle taper issues.

They are using heat shrinkers that stick out a long ways 10" with a shrinker extension.  Cutter run-out needs to minimized and it seems cost is not an issue.

Are hydraulic mill-chucks with extensions better for minimizing runout? 

 

 

Share this post


Link to post
Share on other sites
12 minutes ago, danielm said:

>>>How many minutes will the tool hold up before needing to be replaced?

 

Cutter life is a big deal for this customer.  Also they are very concerned about over working a 40T spindle and premature spindle taper issues.

They are using heat shrinkers that stick out a long ways 10" with a shrinker extension.  Cutter run-out needs to minimized and it seems cost is not an issue.

Are hydraulic mill-chucks with extensions better for minimizing runout? 

 

 

That ratio to taper is a bad combination if they are worried about premature taper issues. That calls for HSK-100 or CAT-50 or at least Big-Plus with that reach if they are doing a lot of roughing. 

  • Like 1

Share this post


Link to post
Share on other sites
29 minutes ago, C^Millman said:

How many minutes will the tool hold up before needing to be replaced?

Tool life of over 120 minutes, and this has  been observed on multiple different parts.  Our spindles are either 50 taper or HSK 100 and we use heat shrink holders with thru-tool coolant.   The speed and feed that I stated we use is also the speed and feed you should get if you enter the parameters into HSM advisor.  I think HSM advisor feeds and speeds are right on for titanium.

Share this post


Link to post
Share on other sites
1 hour ago, daryl_y said:

Tool life of over 120 minutes, and this has  been observed on multiple different parts.  Our spindles are either 50 taper or HSK 100 and we use heat shrink holders with thru-tool coolant.   The speed and feed that I stated we use is also the speed and feed you should get if you enter the parameters into HSM advisor.  I think HSM advisor feeds and speeds are right on for titanium.

Look to the Kaiser Big Plus Chucks with Through the Spindle Coolant. We have seen 20% to 40% longer tool list because of the dampening these chucks offer that Heat Shrink doesn't.

We recommend all of our customers to purchase HSM Advisor it is a great product.

Share this post


Link to post
Share on other sites
On 22/01/2018 at 11:44 AM, daryl_y said:

Tool life of over 120 minutes, and this has  been observed on multiple different parts.  Our spindles are either 50 taper or HSK 100 and we use heat shrink holders with thru-tool coolant.   The speed and feed that I stated we use is also the speed and feed you should get if you enter the parameters into HSM advisor.  I think HSM advisor feeds and speeds are right on for titanium.

Cool! Thanks for great feedback!

I am trying to build an online database for cutting data within HSMAdvisor called Cut Cloud.

Would be really great if you guys could contribute to it by rating and uploading cuts.

Its really easy to use. Just click on the stars on the Speeds and Feeds panel. Enter some cut info and click Submit.

I think having access to real proven data would be a great help for everybody.

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