Titanium cutting

[THEE THAINZ™]

Run a Kennymetal Harvey 3 endmill.

Start at 265 sfm.

Should be able to go 300 no problem.

Keep you Chip load around. .0009" to .0013" per tooth.

8% of diameter for radial. 

 

[So not a Guru]

31 minutes ago, huskermcdoogle said:

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.

I would be very grateful for a sample file, I'll send you a solid tommorow. Thanks Husker!

[huskermcdoogle]

1 hour ago, So not a Guru said:

I would be very grateful for a sample file, I'll send you a solid tommorow. Thanks Husker!

Well i just modeled up a dummy file.  If your part is more detailed or this doesn't give you an idea of how to apply this technique, let me know and we can collaborate to make it work.  I didn't program it, but that part should be pretty self explanatory, once I give the sequence.

Note the mickey mouse ear corner.  That is what would be needed in all the corners, tab distance from the corner isn't terribly critical as you don't have to machine the entire perimeter or floor finish pass with the tabs exposed.

Sequence

1 - Use edge clamps to trap part down onto a flat plate. try not to flex the plate, but a little won't kill you depending on the part tolerance.  If you have vacuum capability, this would be a good alternative, just make sure it can't move in x,y, the vacuum will hold it down fine.

2 - Pocket out the back side, make sure to take note of the overcut in the one corner, if you have sharp outside corners you will have to make sure you face past the corner.  Note also that your pocket is going to be the tool corner radius plus .010-.020" larger than the finish profile of the part.  In this case we went .040" for a .03 corner radius.

3 - Face window frame, this will become your z datum for the next operation, so make sure to know where it is in relation to the pocket floor.  Preferably use the same tool...

4 - Drill Bolt down and locating holes, you will have to go through, or you will need to do half then flip and finish them before bolting it down.  Countersinks on opposite face are just for indicating which side is side two.  You don't need to use them if you don't want to, socket heads shouldn't be a problem for tool clearance.   Also, unless you have features on the first side that need to be located in xy to the second side, locators aren't 100% needed, the bolts will usually suffice, though I will say the tab thickness can be somewhat fussy as you are shooting for .005-.007" thick, sometimes thinner depending on shape and how many you need.  So a few locating dowels or shoulder bolts would be a good idea if it isn't too much bother, slip fit is fine.

5 - Bolt down and machine second side.   You can rough the perimeter at any time you want.  Slot past the far side by the sum of the two corner radii, leave your first side overcut +.010" on the wall.  This will create a good membrane, you can now finish all of the features inside the window.  Leave finishing your perimeter wall until last.  I suggest finishing flush with the bottom of the final part as that won't expose the tabs, and will leave just a little bit to cleanup in the last pass. 

6 - Then for your final act, you cut the same depth as the first rough perimeter pass on the final profile.  As you go around you will clean up the final little sliver and expose the tabs around the part.  When complete you should be able to break the part free, a little twist or dropping it on the bench should be enough to get it out.  If it isn't enough, your tabs are too thick, or too frequent.  A .375" long tab every 3-4 inches should be enough.

If this isn't clear, let me know, I'll make a super fast wax machining sample fail program. 

I will also recommend the harvi 3 endmills, they are great.  If you are over radial 20% engagement don't exceed 200sfm.  Under that you can start to increase dramatically as the radial approaches 5% or less.  If you have the machine behind them, you can remove a lot of material in a hurry at a 20% stepover.  As you have less machine, you make it lighter and go faster.  But for this part it may not be the best fit as it is thin.  For slotting the perimeter, you should be able to do that with a 1/4" Harvi 2 (5 flute) or Harvi 1 TE (4 flute).  Either will work, note that the Harvi 2 is not center cutting, but you can ramp 1-2 degrees, both should be capable of taking the perimeter full slot in one pass.  The 7792 feed can be used as a semi-finish facemill as long as you keep the feeds closer too conventional finishing feed per tooth.  Note that it won't finish flat all the way up to a shoulder by half the insert ic size.

This works well with larger deeper parts as well, makes it such that you don't need a fixture and can bolt it up to a tombstone or grid plate pretty easily.  you end up having to stand on you head for a minute figuring it out.  But once you get the sequence nailed, it makes it much easier to make the part than having to build a fixture.  Just make sure you can spec the material for the process instead of having to fit it into what they gave you.  It can save tons of time and money if you are only making low quantities.  Extra material is cheap in the grand scheme of things if it affords you process flexibility, and speed by not having to make a fixture you use once and throw on the shelf.  You can also use this tab method in a dovetail vise if you have probing and want the tab cleanup to be much easier.

 

Tab Sample.x_t

[So not a Guru]

10 hours ago, huskermcdoogle said:

Pocket out the back side

I'm assuming this is with the 7792, is a helical entry ok?

[huskermcdoogle]

1 hour ago, So not a Guru said:

I'm assuming this is with the 7792, is a helical entry ok?

Yes, but make sure you keep the helical diameter above 1.75xd.  You are better off doing a profile ramp, with 75%+ radial engagement, then 40 or 60% as you pocket out.  If you have life issues due to lack of rigidity, switch from climb to conventional cutting. 

Take a look at page V20 in the catalog link below.  This is an example table of what you can do for ramping with these cutters, it is layed out by cutter. this page is for the D12 cutters.  You may want to look at the smaller D09 cutters with the ramping chart on page v13.  Also note with the 7792 don't exceed 80% of the ap1 max depth of cut per pass.  So for a D09 insert .047" is the max suggested depth of cut.  I would suggest the XDLT##-D411 insert in KCSM40 or X500 grade if the first one isn't available.

https://catalogs.kennametal.com/Master-Catalog-2018-Vol-2-Rotating-Tools-English-Inch/V20/

[88Matt]

What type of Ti is it? S&F will depend on it I've found.  6Al4V vs 6Al6V for instance.

[So not a Guru]

2 hours ago, 88Matt said:

What type of Ti is it? S&F will depend on it I've found.  6Al4V vs 6Al6V for instance.

6Al4V

[Matthew Hajicek - Singularity]

Sorry I'm late to the party.  We do 6Al4V bone plates on the trunnion on the Haas.  I've been using Helical and Harvey cutters with good results.  Dynamic roughing with a 1/2" x 1.25" 7 flute .030" radius bull (27287) and Helical's recommended parameters i get five hours of tool life, in a shrink fit holder with 1000PSI TSC.  I got some Kennametal Harvi 3's and some of Helical's new Ti specific cutters but haven't had a chance to try them yet, didn't want to change the proven process in production.

[crazy^millman]

40 minutes ago, Matthew Hajicek - Conventus said:

Sorry I'm late to the party.  We do 6Al4V bone plates on the trunnion on the Haas.  I've been using Helical and Harvey cutters with good results.  Dynamic roughing with a 1/2" x 1.25" 7 flute .030" radius bull (27287) and Helical's recommended parameters i get five hours of tool life, in a shrink fit holder with 1000PSI TSC.  I got some Kennametal Harvi 3's and some of Helical's new Ti specific cutters but haven't had a chance to try them yet, didn't want to change the proven process in production.

Had a customer not pay for work we did about 6 years ago when we gave them a program to cut TI using HST toolpaths. Said there was no way a tool could hold up for 5 hours in Ti. Now anything less than 5 hours people think your slacking. 

[htm01]

17 hours ago, Matthew Hajicek - Conventus said:

Sorry I'm late to the party.  We do 6Al4V bone plates on the trunnion on the Haas.  I've been using Helical and Harvey cutters with good results.  Dynamic roughing with a 1/2" x 1.25" 7 flute .030" radius bull (27287) and Helical's recommended parameters i get five hours of tool life, in a shrink fit holder with 1000PSI TSC.  I got some Kennametal Harvi 3's and some of Helical's new Ti specific cutters but haven't had a chance to try them yet, didn't want to change the proven process in production.

we about doubled using the Helical Ti specific cutters

and that's with a HAAS, if we had real machines watch out

[Leon82]

Also cut the mill scale off first from both sides

[rchipper]

I have had success machining similar parts using 2 sided tape as mentioned above.

[So not a Guru]

On 7/22/2020 at 9:52 PM, huskermcdoogle said:

If this isn't clear, let me know, I'll make a super fast wax machining sample fail program. 

I thought I understood how this would work, but, using the recommended radial DOC of 0.17", I cannot get the corner reliefs cut without creating huge radii. Also, the 0.17" leaves a high ridge in the profile entry. How important is it to use that parameter?

Would you mind taking a look at this and pointing me in the right direction?

 

Ti_test.mcam

[So not a Guru]

On 7/23/2020 at 2:33 PM, Matthew Hajicek - Conventus said:

1000PSI TSC

I wish we had this on our machines!

 

[huskermcdoogle]

1 hour ago, So not a Guru said:

Would you mind taking a look at this and pointing me in the right direction?

Zeke,

Drop your min toolpath radius to 10%, that should get you into the corners with the overcut radii that you have.  You can leave the stepover at 27%, that should be fine, you can go up to the flat diameter on the end of the tool.  Then I would change to use a custom entry profile, and draw a line or racetrack oval in the middle such that you rough out a long slot down the middle before stepping out, this will be much more efficient.  If you want to make the corner cuts smaller, feel free to make it such that the feedmill barely gets over the corner ( end diameter, not periphery), then come back and rest machine with a 1/4" endmill.  No hurt in that whatsoever.  In fact, just getting the skin and initial roughing with the 7792, and then finishing .005-.007 off the floor with a 3/8 or half inch isn't a bad idea anyway, as you will be able to feed faster with a 3/8 six flute for finishing anyway. Use a 75% stepover.  Start around (3/8") 150 sfm, .280" woc, .007"doc, .0017ipt. 

Don't forget to draw in your support tabs like I modeled on the sample model.  The extra material on the first side is a bit thinner than I have ever done, but I think it should still work.  Worst case you end up with conventional tabs.

I'm a bit slammed schedule wise today, but if you want to peck away at this today, and upload another file this afternoon.  I can take a look at it tonight when I get back home and provide more feedback/make adjustments if needed.

HTH

Nick

[So not a Guru]

4 hours ago, huskermcdoogle said:

upload another file this afternoon

I worked at it a bit, I'm pretty slammed today as well, this is where I'm at right now. I'm going to bring a copy home, but I don't know if I'll be able to do anything with it, I've got to go to a wake for a friends son tonight.

Ti_test.mcam

[huskermcdoogle]

7 hours ago, So not a Guru said:

I worked at it a bit, I'm pretty slammed today as well, this is where I'm at right now. I'm going to bring a copy home, but I don't know if I'll be able to do anything with it, I've got to go to a wake for a friends son tonight.

Ti_test.mcam

Here is what I would suggest.

As you are doing horizontal tabs per lack of extra thickness.  I would add a drilled start hole for the periphery pass so you aren't ramping the endmill, no sense in beating up that tool.  I also added drill holes where it ramps back down on the back side of the tabs.  Should help end mill life quite a bit.  Along with that I added a rough and finish pass of the profile before we cut the tabs in such that the tab op has as little cutting pressure as possible so as to not break the tabs.  It will probably need some tweaking/tuning, but it's at least hopefully a solid foundation to stand on.

ti_test.zip

[So not a Guru]

12 hours ago, huskermcdoogle said:

Here is what I would suggest.

Thanks Nick, the material will be here next week, I'll let you know how it works out.

Zeke

[So not a Guru]

On 7/27/2020 at 9:08 PM, huskermcdoogle said:

It will probably need some tweaking/tuning, but it's at least hopefully a solid foundation to stand on.

Nick

The material came in 0.020" to 0.025" thick, so I followed your earlier suggestion of facing of both sides and it has worked flawlessly! We are turning the inserts every 10 parts & changing the 2.5mm drill every 20 parts. I cannot believe the Harvi 2 1/4" cutter has cut 50 parts without any noticeable wear! We are going to swap it for the next part#, just to be safe.

Thanks again to you, and this forum at large.

[huskermcdoogle]

3 hours ago, So not a Guru said:

Thanks again to you, and this forum at large.

Happy to help.