Titanium Tooling Suggestions

[Mic6]

I have a job coming up, the stock is 6 x 6 x .75 thick. The part is 4.375 x 5.00 x .388 thick. (It's too late, the material has been ordered) I'll be using Varimills for the outer contour and the .2 deep pocket. Can I just use basic carbide drills/spot drills. Wanted to use a carbide 140° spot drill. As for threadmills, should I use a single point or full form? 6-32 and 4-40. The top edge has a .250 radius. I was thinking I should surface this radius rather than using a carbide corner rounder. Any suggestions for a facemill/style for a nice finish? I currently have a Mits 2" BDX. What say you?

[jeff]

Man, it's been so long since I've machined Titanium, but I'm pretty sure you want full form threadmills.

As for a facemill, I used a Sandvik R390 with decent results.

[mayday]

6 x 6 x .75 thick

 

cute little part. I run so much Ti, its like Aluminum annymore. Facemills? Ceretizit or Dijet with button inserts. Carbide everywhere else. milling 125 - 200 SFM about a .001 per tooth

drilling about 25 SFM

[MIL-TFP-41]

I believe Mitsubishi does make a coated grade for Ti in the BDX cutter....should work well. Run a dynamic path around the outside to rough it in....you will be amazed how fast it comes off.

[Goldorak]

+1 for ceratizit , they got a special insert for titanium that can cut forever, about 50x longer than it's closest competitor we try (iscar)

sandvik's ra390 was far behind

[taperlength]

Use a full form threadmill with staggered teeth.

[ReDEyZZ]

Use a full form threadmill

 

+1 You'll need a spring pass or a finish pass as well to hold size usually. On all roughing ops use LOTS of coolant if possible, to high of a SFM and you'll mess up your carbide tool. At Just the right SFM they can last a long time, it's a much finer line with TI.

[jbreth]

We cut lots of titanium! I have gone to high speed machining. We run a Kennametal Harvi 2 12mm x 32mm flutes. We are taking a full axial depth of 32mm sfm 500 (5093 rpm) chip load of .009 per tooth (183.3 IMP). The radial engagement is a max of .006 with an average tool life of 290 min of cut.

The Metal Removal Rate equals 1.4 cubic inches per min. We were only getting .5 Cubic inches per min with a 1/2" Vari Mill and the tool life is nowhere near what the High Speed Machining can do.

As far as thread milling we use Carmex 3flt Mini mill thread mil. We have used their thread mills all the way down to 1-72.

[mowens]

Don't you have to be careful with Ti to not take too light of a cut? Maybe that's old school now. We use to make sure we had enough of a chip load so we weren't just rubbing.

 

Also, if you have a cutter with a specific geometry you have to use a deep enough DOC so the geometry can fully engage and do its' job properly

[Guest CNC Apps Guy 1]

I did 2-56 blind holes in Ti... Single tooth profile, 3 passes, 2 rough and 1 spring.

 

10RPM @ 10IPM. TiAln coated.

 

HTH

[greenxman]

i cut it once and awhile but i don't want to beat the spindle or buy $$$ tooling i work in a low cost spending. so my answer is hss /cobolt with ticn like a 3/4 -1. only costs about 20 - 45$$ and will last o long time .had to rough out some big parts then that down to tooth picks. did 7pc with 1 endmill and then used it on another job.

 

just my 2 cents

[left coast lefty]

I am trying to dynamic mill Ti 6AL-4V with a 1/4" 4 flute coated Hanita stubby. Can anyone suggest RPM, feedrate and stepover? We are eating them up pretty fast.

[Josh Kinney -Elite Engineering]

350SFM (5,348RPM)

75IPM

0.015" Step Over is where I would start. Around 5-8% Step Over is good.

 

You should be able to go a lot faster. Around 125-175IPM. But to be on the safe side...

[mkd]

i cut it once and awhile but i don't want to beat the spindle or buy $$$ tooling i work in a low cost spending. so my answer is hss /cobolt with ticn like a 3/4 -1. only costs about 20 - 45$$ and will last o long time .had to rough out some big parts then that down to tooth picks. did 7pc with 1 endmill and then used it on another job.

 

just my 2 cents

 

+1

 

cheap HSS corncobbs can have surprising results! i've buried 1-1/4" DIA five fluters on 3 spindle Cincinnatis, etc. not super exciting slowly chugging through, but the parts HIT THE FLOOR (sometimes the tools too). much easier to apply and program for the inexperienced. they last hours!

i've attended Boeing conferences where some "smart dude" claimed to run 400-500 SFM as a good shop rate/ tooling cost trade-off. I don't see it. i tried it. 60 second tool life on a $400, 20mm 10 flute is just stupid and .006 stepover seems questionable at best.

[Jeremy Herron@DBS Solutions™]

cute little part. I run so much Ti, its like Aluminum annymore. Facemills? Ceretizit or Dijet with button inserts. Carbide everywhere else. milling 125 - 200 SFM about a .001 per tooth

drilling about 25 SFM

 

 

Wes, do you have an insert number for the Ceratizit?

[left coast lefty]

350SFM (5,348RPM)

75IPM

0.015" Step Over is where I would start. Around 5-8% Step Over is good.

 

You should be able to go a lot faster. Around 125-175IPM. But to be on the safe side...

 

Thanks! I'm only going 50 IPM, so I should be really safe.

[Josh Kinney -Elite Engineering]

Just remember sometimes going too slow will cause excessive heat and wear out tools. Faster is sometimes better. I usually adjust the step over and feed together to find the best tool life.

 

http://www.volumill.com/files/ACTC_White_Paper_1.pdf

[jbhunter]

+1

 

cheap HSS corncobbs can have surprising results! i've buried 1-1/4" DIA five fluters on 3 spindle Cincinnatis, etc. not super exciting slowly chugging through, but the parts HIT THE FLOOR (sometimes the tools too). much easier to apply and program for the inexperienced. they last hours!

i've attended Boeing conferences where some "smart dude" claimed to run 400-500 SFM as a good shop rate/ tooling cost trade-off. I don't see it. i tried it. 60 second tool life on a $400, 20mm 10 flute is just stupid and .006 stepover seems questionable at best.

 

mkd,

 

I think I have seen one of those pitches before at IMTS. From my understanding I think there was a valid point. If I seen the same pitch I think they were saying that buying a cheap tool is more expensive than you think. Reason being is sometimes your machine $/hour rate ends up costing you more overall dollars for a part if you are running very conservative.

 

If your cutter is $100 and your hourly rate is $100, and you have 3 hours tool life to cut one part it costs you $400.

If your cutter is $300 and your hourly rate is $100, and you have 1 hour tool life to cut the entire part, it still costs $400 for the part,

but in the same time you got three parts done versus one.

 

I agree that hogging cutters are still a great way to remove material, but times change, high performance cutters pay back their own price, and then some. The same goes with new NC programming toolpaths such as dynamic mill. There is a learning curve and maybe additional costs, but the more you use them the more they pay back.

 

Also, if you ran a 20mm tool at 400-500 sfpm and 0.006" radial depth of cut in titanium, but only achieve 60 seconds of tool life...??? Where you using coolant???? Parameters such as this are everyday for dynamic mill in Ti64 with 60-90 minutes of life even at 0.040" radial depth.

[mkd]

jbhunter,

very astute reply!

good on you to acknowledge the possible benefits and ease of old school HSS. with the right machine and part geometry, this method can and will WILDLY out perform many fancy-smancy-ity-bity step-over high speed techniques on CU. IN. per minute basis. i have yet to apply post V9 tool paths to Ti, but would love to even with large step over (30-40%) with HSS.

of course small stepovers open up a wider array of lighter / faster machines.

 

anyone's experience has limits. i have not done the exact cited example in 6AL4v. i did it with Ti-62222 (F-22 part) with a .04" stepover. uuuuh ya, with High pressure external coolant. tool life was seconds not minutes. would love to know how to improve.

i have not personally seen Ti 6al4v run acceptably over 200 sfm. believe me i tried. too many variables to know where i was going wrong.

i did a pretty neat 6al4v improvement project back in 2005. took a 12hr cycle time part and brought it down to 3-4 hours with a change to a near-net waterjet profile and small stepover methods using Robb jack's tight flute endmills. there was such a tool-life-sweet-spot in keeping it below 200 sfm! Allot more work changing cutters above that.

I'm from Missouri. Show me. If that sounds like a challenge...well..

 

ref:

http://www.cs.odu.edu/~mln/ltrs-pdfs/NASA-97-themec-wdb.pdf

[mkd]

1000% confident I can do over 3cuin/minute with hours of tool life on a $100 tool.

1.25 dia, .50 stepover. 2 in deep and 3 in per minute.= 3 cuin/min

or

1.25 dia, 1.0 stepover, 2 in deep and 3 in per minute.= 6 cuin/min

 

compared to HSM:

.787 (20mm) 1.18 deep 2400rpm(500sfm) .04 stepover 72ipm (.003") =3.42 cuin/m

i dont think you would get more than 20 minutes out of this tool. in my exper. much much less.

i've done 80 ipm with this setup for hours and hours but nowhere near 500 sfm. i think anyone who says 500 sfm is smoking crack.

[Guest CNC Apps Guy 1]

I use the Iscar HSM Spreadsheet for calculating speeds and feeds. It has NEVER let me down. Inconel, Ti, SS, etc...

 

Case;

Matl' - 17-4 @ 38Rc

Tool - 2.9" Face Mill @ 75% Stepover and .050 DOC 530 SFM @ .0047 IPT

Toolpath - Facing/Contour

Tool Life - 1 part per corner (using Octo Inserts)

Cycle Time - 20min 38sec.

 

Tool .5" Bull E/M @ 10% Stepover and 1.25 DOC 490 SFM @ .0171 IPT (with chip thinning)

Toolpath - 2D HSM - Dynamic Area

Tool Life - Entire run + (left after 12 parts because I got bored and tool still looked new)

Cycle Time - 9min 13sec.

 

Doubled the cubes/halfed the cycle time, better than 12x tool life, easier on the machine, etc...

 

Just sayin'

[mkd]

last time i checked 17-4 was not in the Ti family.

 

so to get to a 1.25" depth with a facemill it would take 25 z steps of .05"???

the guy who programmed that needs to be slapped.

 

i wonder what the cycle time would have been with a 1.25 corncobb, full depth and 40% stepover, 6 minutes?

[Guest CNC Apps Guy 1]

i wonder what the cycle time would have been with a 1.25 corncobb, full depth and 40% stepover, 6 minutes? Burned up tool!

 

Fissed for accuracy.

[Guest CNC Apps Guy 1]

I just went with a semi-random tool they already had in the magazine. Nothing special. Starting from scratch I would have probably been able to get it down to the 5-7 minute range without too much effort.

 

Besides, this was a 40 taper machine... Old School Low and Slow doesn't get it done in a lot of today's machines. You need a completely different approach. SUre everybody wants to see a 6" cutter buried 4" deep in steel and hear that rumble, but many of today's machines are not made to remove material in that manner.

[robk]

I don't mean to pick arguments with you James, but you are dead wrong about the Ø1.25 corncob burning up in your above statement. As a matter of fact our older horizontal Mori-Seiki machines (45 & 50 taper) will cut all day long (6 hrs. per cutter) with Ø1.0" Hanita corncob rougher @ about 30sfm in Ti (40% stepover with full DOC). Ø1.25 would not be a problem. This is on programs that have proven themselves over and over again. Old school low and slow gets it done in this case. You can't beat that for material removal. The machines are running unattended for hours...