Suggestions for milling Titanium

[Metals and materials]

There are many I could fine online on tips and tricks to mill titanium. But I want to hear from Mastercam's programming point of view, what extra precautions I should take while making a program for milling Titanium. 

Or like any general advice for milling 6Al-4v. This is my first-time milling Titanium, and the best part is that it is also the first time my machinist, milling Titanium in 5Axis machine. So, I wanted to make sure I am not scrapping part or tool.

Thank you for your responses in advance!!

[X_IHS]

Good work holding, proper tools (coatings, number of flutes), proper coolant concentrations.

Good article here Milling Ti

 

 

[Manofwar]

Something of note when working with S class materials. Be very careful about your first passes against raw stock. If the stock is oversized you can over engage your tool. Which will break the tool instantaneously. I generally always drew my stock .02"-.05" larger then what I measured to help with this issue. The material wants to soak heat, even blipping the coolant off for a second while it's touching material can end the tools life. If you have TSC use it!

[Matthew Hajicek - Singularity]

Use material specific cutters, use HSMAdvisor for starting parameters, and avoid full width slotting if you can.  Dynamic paths work well.  Make sure your part is well fixtured and supported, since the material is more flexible and elastic than steel.

[nickbe10]

Titanium (6Al4V) is pretty straight forward if you use good machining practices.

It is both hard AND tough.

It is (like Aluminum) a heat resistant material. That is, it does not conduct heat well.

As rigid a set up as you can manage. Both with your tools (short as possible) and fixturing / tooling.

I leave a fair amount of stock (obviously it depends on the cutter you are using), with a .5 -.75 inch solid carbide, and pretty much any insert cutter I can think of, I am leaving 0.02" stock to finish. If you are only leaving 0.01 with inserts, you are probably in trouble already.

Keep you chip load as high as you can to get the heat into the chip, more stock helps here.

Smaller parts are fine in a 40T machine, but once you get up much above 12" you will certainly wish you had a 50T.

[Manofwar]

Something else, be very careful making threads in this material. You can tap it, but it requires tapping fluid, and peck tapping most of the time. It's generally a lot safer to threadmill, if you only have a couple parts to make, I would suggest it over trying to figure out tapping. (unless you have a sacrificial piece to figure out how the tapping works.) 

[nickbe10]

12 minutes ago, Manofwar said:

Something else, be very careful making threads in this material.

 

Holes are nothing but misery generally, and Titanium is no exception here.

MolyD mixed with Copperease is one of the best tapping fluids I have used for Ti.

In the hard metal shops I have worked in, generally anything more than 3/8" diameter and I am looking at a threadmill option.

Also true for the nasty stainless steels.

 

[cruzila]

^^^^^^

I've had fair success with Emuge reverse spiral cut taps. Form taps do work but you need good tapping fluid. Drill to the max allowable size per the drawing or drill charts

[Colin Gilchrist]

Use Dynamic Milling. Make your stepover 2-4% of the tool diameter, maximum 5%. You want to minimize the heat getting into the tool and stock, and maximize the heat getting into the chip. Taking a small stepover minimizes the cutting edge contact time as the tooth is shearing off a chip. To maximize material removal, you'll want to use a flute at least 2:1, depth to diameter.

Unless you have very massive amounts of material to remove, I like using 1/2" diameter endmills because of the value. 

https://www.helicaltool.com/products/tool-details-84511

I use FSWizard, and love this app/software. If you don't have a copy, it is worth getting the "pro" version, with the lifetime license. Money very well spent.

I plugged in the following parameters for the tool I recommended above:

• Grade 5 Titanium, 6al-4v (310-350HB)
• Solid Endmill
• Carbide
• ALTiN coating
• IN units
• 0.5 Tip Dia
• 6 flutes
• 1.35" stickout
• 0.03 Corner Radius
• Flute Length 1.25"
• 38 degree helix angle (I guessed, this wasn't listed)
• 90 degree lead angle
• 0.5 shank diameter

Engagement:

• Depth of cut 1"
• Width of cut 0.02"
• Width of cut percentage 4%
• No to slotting
• Yes to Chip Thinning
• No to HSM

Overrides set to 100% for speed and feed.

 

This gives a recommendation of 1337 RPM, a Feedrate of 68.86 IPM (68 IPM). This requires 2.14 horsepower, and results in 1.38 cubic inches per minute of metal removal.

 

 

 

[Matthew Hajicek - Singularity]

For threads in Ti, I find form taps work well, where applicable.

[Aaron Eberhard]

I did a project using a Kennametal RSM cutter for roughing.  It was a .75" I believe with 13(?) Flutes?  It was insane.  And it lasted forever.  I'll grab the model number, speeds and feeds next time I'm near a computer for you.  It was awesome.

[jpatry]

On 10/27/2023 at 12:43 PM, Manofwar said:

Something else, be very careful making threads in this material. You can tap it, but it requires tapping fluid, and peck tapping most of the time. It's generally a lot safer to threadmill, if you only have a couple parts to make, I would suggest it over trying to figure out tapping. (unless you have a sacrificial piece to figure out how the tapping works.) 

What about form tapping?

[MrFish]

22 hours ago, jpatry said:

What about form tapping?

Thats a big NO, threadmill is the safest.

Dynamic toolpaths with max 8% step over, make sure you are always taking a a cut, i.e. don't run air passes

[jpatry]

2 hours ago, MrFish said:

Thats a big NO

Is it because the material is quite springy and does not like to deform permanently in such an operation, or is it due to how titanium likes to adhere to other materials under such conditions?

[MrFish]

9 minutes ago, jpatry said:

Is it because the material is quite springy and does not like to deform permanently in such an operation, or is it due to how titanium likes to adhere to other materials under such conditions?

This explains it well 

Titanium is also a challenge. “In addition to its high tensile strength and low ductility, titanium has very low thermal conductivity, meaning that it doesn’t absorb heat very well,” Gennuso said. During a tapping operation, heat enters the workpiece, tap and chips, he explained. Because forming doesn’t create chips, the heat must go into the tap or the material. When form tapping titanium, a lot of that heat penetrates the tool and causes premature failure.

[jpatry]

6 hours ago, MrFish said:

This explains it well 

Titanium is also a challenge. “In addition to its high tensile strength and low ductility, titanium has very low thermal conductivity, meaning that it doesn’t absorb heat very well,” Gennuso said. During a tapping operation, heat enters the workpiece, tap and chips, he explained. Because forming doesn’t create chips, the heat must go into the tap or the material. When form tapping titanium, a lot of that heat penetrates the tool and causes premature failure.

This is great to know.

The company I work for has yet to bid on any titanium jobs, but they love to imagine themselves more capable than they are, and make promises that are often of dubious deliverability.

And so, it's not a matter of if, but rather of when, thus I'd rather be armed with as much information as possible.

[cruzila]

On 10/28/2023 at 4:10 PM, Aaron Eberhard said:

I did a project using a Kennametal RSM cutter for roughing.  It was a .75" I believe with 13(?) Flutes?  It was insane.  And it lasted forever.  I'll grab the model number, speeds and feeds next time I'm near a computer for you.  It was awesome.

I forget where I saw it (Boeing? aerospace? IMCO?) but there were tests to see if the number of flutes could be maximized for roughing TI. It came down to runout and the limits of the physical universe. To get each tooth to engage well and give long life 13 is about the max for an endmill. Material removal rates boils down to number of teeth.

 

[Metals and materials]

Does the Variable Helix Angle matter here? I saw some tooling online they have Titanium as applicable material but have helix defined as variable. Curious, if that helps with cutting Titanium or is it one more selling tactics?

[Matthew Hajicek - Singularity]

A few months ago I had to make 100 parts with six 000-120 threads in each, Ti6Al4V-ELI.  I started out threadmilling, but it was taking several minutes per part, and I had to keep gauging, adjusting the offset, and rerunning to keep the threads in tolerance.  Each threadmill was only good for about two dozen parts.  Same job came up again, and this time I got form taps; one and done for each hole, about a second per hole.  The one tap lasted the whole job, and every hole was perfect.

If you have a very small number of parts to do, threadmilling is probably easier and safer, especially on large threads.  Form tapping is WAY faster, provided you have the right material-specific tap and enough torque.  #10 threads are the upper limit for form tapping in Ti on my little baby 20 taper CM-1's.

[MrFish]

2 hours ago, Matthew Hajicek - Singularity said:

A few months ago I had to make 100 parts with six 000-120 threads in each, Ti6Al4V-ELI.  I started out threadmilling, but it was taking several minutes per part, and I had to keep gauging, adjusting the offset, and rerunning to keep the threads in tolerance.  Each threadmill was only good for about two dozen parts.  Same job came up again, and this time I got form taps; one and done for each hole, about a second per hole.  The one tap lasted the whole job, and every hole was perfect.

If you have a very small number of parts to do, threadmilling is probably easier and safer, especially on large threads.  Form tapping is WAY faster, provided you have the right material-specific tap and enough torque.  #10 threads are the upper limit for form tapping in Ti on my little baby 20 taper CM-1's.

Well there you go then, my learning for the day. I would have never have even attempted to form tap Titanium with my understanding of the material properties and difficulties it can produce. Out of interest what tap were you using ?

4 hours ago, cruzila said:

I forget where I saw it (Boeing? aerospace? IMCO?) but there were tests to see if the number of flutes could be maximized for roughing TI. It came down to runout and the limits of the physical universe. To get each tooth to engage well and give long life 13 is about the max for an endmill. Material removal rates boils down to number of teeth.

 

From my experience this is very much machine and setup specific. You'll need both a rigid machine and setup for that.Try running a 13 tooth endmill in Ti6al4V on a HAAS !!!

[cruzila]

12 minutes ago, MrFish said:

Well there you go then, my learning for the day. I would have never have even attempted to form tap Titanium with my understanding of the material properties and difficulties it can produce. Out of interest what tap were you using ?

From my experience this is very much machine and setup specific. You'll need both a rigid machine and setup for that.Try running a 13 tooth endmill in Ti6al4V on a HAAS !!!

Roll taps will smoke in TI but doable. 

As with literally EVERYTHING in this industry, VERY MUCH specific...... bwahahahaha

[Aaron Eberhard]

On 10/28/2023 at 7:10 PM, Aaron Eberhard said:

I did a project using a Kennametal RSM cutter for roughing.  It was a .75" I believe with 13(?) Flutes?  It was insane.  And it lasted forever.  I'll grab the model number, speeds and feeds next time I'm near a computer for you.  It was awesome.

Here ya go:

I used https://www.kennametalnovo.com/app/en/search/kennametal/productdetail/6167540/full a .75" 13FL R.015 EM w/ 1.5DOC, put into a SST Shrink holder.

We were on a Makino DA300 with an HSK-63A that we were specifically told to not exceed 30%(If I recall correctly?) spindle load due to the bearings.

A full (1.5") DOC,, we ended up at 1.5% stepover, .0048 FPT @475 SFM (174IPM @ 2419).

It was fun.

 

[Matthew Hajicek - Singularity]

7 hours ago, MrFish said:

Out of interest what tap were you using ?

Balax:

https://ecomm.productivity.com/itemdetail/BALA 00102-01T

 

[Metals and materials]

Sooo, I have to tap with M8x1.25 STI for helicoil inserts. I asked one of the dealer closer to my location and he suggested to use EXo-Form Tap from OSG.

OSG 1636000708                             We have Ridgid high performance thread cutting fluid. 

I have DMU from DMG Mori 5 axis machine. Should I try? or leave aside form taps at all and start looking only and only thread cutter options

[Matthew Hajicek - Singularity]

On 10/31/2023 at 8:44 AM, Metals and materials said:

Sooo, I have to tap with M8x1.25 STI for helicoil inserts. I asked one of the dealer closer to my location and he suggested to use EXo-Form Tap from OSG.

OSG 1636000708                             We have Ridgid high performance thread cutting fluid. 

I have DMU from DMG Mori 5 axis machine. Should I try? or leave aside form taps at all and start looking only and only thread cutter options

Go for it.  Just make sure the drilled diameter is what the tap manufacturer recommends.