Titanium cutting

[So not a Guru]

We're quoting some Ti parts, they are basically flat parts made from 1/4" plate. They must be machined down to 0.197" thick, then the profiles cut.

Anyone have any good recommendations for endmills, speeds & feeds? I've done a bit of Ti work, but not thin stuff like this and I'm concerned about tool life.

[lowcountrycamo]

Tool life will be tough, as you are only cutting with the end.  I use a 3/8 .5loc 5flt from imco for things like that.   They are cheap.  Also  ti that thin always warps so you might have to face both sides first.  That is what kills you on run times with jobs like these.

[gcode]

Blanchard grind the plates to .197" first?

[So not a Guru]

36 minutes ago, gcode said:

Blanchard grind the plates to .197" first?

We would have to outsource that.

I would think holding the blanks would be a challenge, due to the thin size & being non-magnetic.

[JParis]

54 minutes ago, So not a Guru said:

We're quoting some Ti parts, they are basically flat parts made from 1/4" plate. They must be machined down to 0.197" thick, then the profiles cut.

Anyone have any good recommendations for endmills, speeds & feeds? I've done a bit of Ti work, but not thin stuff like this and I'm concerned about tool life.

Sight unseen I'm spitballing here...

As noted, Blanchard grinding is a good option...if you can get larger plates, drill screw down holes, make a fixture with deeper profile channels  so you can distribute the depth cuts along the tool  Z axis...can help...

Tools, use a good grade of carbide, 4+ flutes....speeds and feeds depend on the grade of Ti....

[So not a Guru]

1 minute ago, JParis said:

if you can get larger plates, drill screw down holes, make a fixture with deeper profile channels  so you can distribute the depth cuts along the tool  Z axis...can help...

That is basically how I am considering doing it, not sure if I'll be able to utilize deep channels too much as I'll need to use tabs, they are flat with no holes, sop I've got to tab them.

3 minutes ago, JParis said:

Tools, use a good grade of carbide, 4+ flutes....speeds and feeds depend on the grade of Ti....

Yeah, I was thinking of 1/4 - 3/8 5 flutes, it's 6AL-4V, so probably around 180sfm $ 0.0008ipt.

[htm01]

https://www.helicaltool.com/products/titanium-6-flute-corner-radius-variable-pitch

Helical just came out with some Ti specific end mills , work well.

non-coated carbide usually works best

[So not a Guru]

2 minutes ago, htm01 said:

non-coated carbide usually works best

Really? I would have never tried that!

I'm really concerned about slotting thru this thin stuff

[Leon82]

Double disk grind

[Rstewart]

You'll be $$$ ahead if you outsource to get them ground by some means to thickness.

They're gonna warp like a SOB peeling .053" off the face with a mill

[So not a Guru]

9 minutes ago, Leon82 said:

Double disk grind

No one near us has the machine for this and the delivery date won't give us the time to outsource it across the country. Great to know about for the future though, thanks.

[So not a Guru]

6 minutes ago, Rstewart said:

They're gonna warp like a SOB peeling .053" off the face with a mill

Yes sir, that is my biggest concern.

[gcode]

2 hours ago, So not a Guru said:

We would have to outsource that.

I'd crunch the numbers

it's grinding cost vrs  machine time, payroll time and endmill costs.

If what you are doing isn't working and you are burning $400/hour worth of endmills and making bad parts, OP grinding starts to look real cheap .

If I have to endmill Ti, I try to use endmills with a big corner radius, preferably twice the intended depth of cut for thin plate work.

That gives you a tougher cutting edge, some chip thinning and the corner radius helps push the stock down into the

fixture.

Sometimes pocketing from the inside out works best

Depending on how big the plates are, you may want to consider a vacuum fixture.

 

[So not a Guru]

The parts are fairly small, the largest blank size is 15" x 6". Thanks for the pocketing suggestions!

[heavychevy2155]

If your going to pocket inside to out, I would try dynamic with a custom entry.  Just a line in the middle will do, also give it some additional slot width.  I just don't like helixing in and recutting chips in Ti.  I use custom entry on just about anything I can, you can play around and really reduce some cycle time and it can make for some pretty cool paths.

[Guest]

3 hours ago, So not a Guru said:

That is basically how I am considering doing it, not sure if I'll be able to utilize deep channels too much as I'll need to use tabs, they are flat with no holes, sop I've got to tab them.

A roughing pass with osciliation/ramp could spare you some tool wear, ramp tabs would be ideal

Double sided tape would let you skip the tabs

[So not a Guru]

5 minutes ago, byte said:

A roughing pass with osciliation/ramp could spare you some tool wear, ramp tabs would be ideal

I didn't realize I could use oscillation with tabs.

2 minutes ago, So not a Guru said:

I didn't realize I could use oscillation with tabs.

Tabs greys out when oscillate is selected.

[Guest]

10 minutes ago, So not a Guru said:

Tabs greys out when oscillate is selected.

They are, it would require 2 operations, the first a roughing pass until the depth of the tab height and the 2nd a 2d contour, that's how we do it

[Leon82]

We use a kenametal face mill when we fly cut TI. It has the 4 sides under at 45 degrees. They always have 2 heat treats thought. 

Usually we glue it to a plate with epoxy to keep it free

[So not a Guru]

3 minutes ago, Leon82 said:

Usually we glue it to a plate with epoxy to keep it free

We glue with Loctite 380 on a lot of stuff, but the operators have a hard time with it. What epoxy are y'all using?

[Leon82]

7 minutes ago, So not a Guru said:

We glue with Loctite 380 on a lot of stuff, but the operators have a hard time with it. What epoxy are y'all using?

Locktite 5 min. Wait about 20 to 30 before cutting

[huskermcdoogle]

Use a 7792 feedmill for the facing to thickness.  As for how to do it.  Sometimes depending on shape it is best to skim one side, drill bolt down and locating holes in the window frame, then pocket the backside .125 deep x .03-.05 over the shape of the part with .005"-.010"x.375" vertical tabs every 3-4 inches.  Then flip back over onto locators and profile the part down, exposing the tab's, leaving the window.  Break out and sand/deburr off the very small tabs.

If you need a better explanation.  Let me know, I can make a sample file if you can supply me with a dumb solid sample.  The big thing here is the extra material.  But it is dead xxxx simple, and usually you won't have a problem with the parts moving much.  The extra material is paid for by eliminating a ton of screwing around.

[Rstewart]

5 minutes ago, huskermcdoogle said:

Use a 7792 feedmill for the facing to thickness.  As for how to do it.  Sometimes depending on shape it is best to skim one side, drill bolt down and locating holes in the window frame, then pocket the backside .125 deep x .03-.05 over the shape of the part with .005"-.010"x.375" vertical tabs every 3-4 inches.  Then flip back over onto locators and profile the part down, exposing the tab's, leaving the window.  Break out and sand/deburr off the very small tabs.

If you need a better explanation.  Let me know, I can make a sample file if you can supply me with a dumb solid sample.  The big thing here is the extra material.  But it is dead xxxx simple, and usually you won't have a problem with the parts moving much.  The extra material is paid for by eliminating a ton of screwing around.

Not the one looking to figure this out, but I would like to see your example if you have the time.  Not exactly sure I'm following you entirely.

[So not a Guru]

25 minutes ago, huskermcdoogle said:

7792 feedmill

Is this the Kennemetal product?

[huskermcdoogle]

1 minute ago, So not a Guru said:

Is this the Kennemetal product?

Yes