Machining Titanium

[pejaer]

This is also a newbie questions, but quick help (!) overrides

I need to "face mill" a circular pocket in a small titanium part. Really, it doesn't need to be pretty, I just need to cut into/remove a surface/wall on an exiting part which has a cavity on the inside and expose the inside...

Anyway, the surface/wall is (best I can tell) about .070" thick. I started with a .078 4-flute carbide end mill and setup a pocketing wizard with the parameters attached in the jpeg...the end mill snapped in about 1 second. Of course, I forgot to use coolant, but I am thinking that it probably would have broke anyway since it was so quick...on the bright side, I did make one or two slivers....so I am encouraged.

Can someone look over the wizard (please work with this, I don't have a lot of time to explore other software for this quick job) and give me some pointers?

Much appreciated.
Paul

[txcncman]

You want maximum SFM to be about 150. Do you know how to calculate RPM from SFM? Chip load should be about 0.002" to 0.0035" per tooth. Do you know how to calculate feed rate after you have calculated RPM?

[tbaker2500]

I don't have G-Wizard in front of me, but I highly recommend it to stop breaking bits if you are unsure of your feed rates. A tiny bit like that needs to be spinning at much faster than 800rpm. 70thou is probably too deep a cut also. I don't know Titanium, but in aluminum I'd run a .0625" bit at 50thou deep, 4500rpm at 3.5ipm, 2.5ipm plunge.

[tbaker2500]

You want maximum SFM to be about 150. Do you know how to calculate RPM from SFM? Chip load should be about 0.002" to 0.0035" per tooth. Do you know how to calculate feed rate after you have calculated RPM?

My gut tells me that chip loading would break a 0.078" bit? But I don't know titanium.

[Sp-4renegade]

you might try " titanuim machining data" on bing, they had some good tips

[TXFred]

As others have said, your feeds and speeds are FUBAR.

You're feeding at 3 IPM, but plunging at 5 IPM. Plunge feedrate should normally not exceed half of the feedrate. And your spindle speed is way too low. It's no wonder you killed the cutter.

First of all, make sure that you have a center cutting end mill. If you don't have that, then it's going to break on the plunge no matter what your feeds and speeds are.

Here's a screenshot from G-Wizard. I plugged in the numbers you gave to get these results. In short, change your spindle speed, change your feed and plunge feedrates, switch to climb milling, reduce your stepover, and run flood coolant. If the end mill is not center cutting, drill an entry hole.

I cannot promise that these numbers are good, but they should be a good starting point.

Good luck!

Frederic

[pejaer]

Frederic,

Thanks for the info. You are right, I botched the plunge rate....I had in my mind it was the approach speed and not plunge....rookie mistake.

I am looking at your G-wizard, and it looks to me that the RPM is a data input and not something the software is telling me to set...I am curious if you can explain to me if this is true....I get the point from you and the others that (apparently) I need to max out the spindle at 5100 which is the opposite of what I was thinking....but is G-wizard suggesting this or is this an input?

2nd question: I would appreciate it if you crunch the same with a .1875 2-flute HSS cutter...in hindsight, there is no reason not to go with the larger cutter (rookie mistake 2 or 3)...

Thanks.

[pejaer]

Hello txcnc,

I put the numbers in to the Mach calculator, and it seems pretty fast (if I did it right). The RPMs puts me over the 5100, and the feedrate seems quick...is this a time where one should intuitively jump to a larger cutter if possible? See attached.

[txcncman]

Hello txcnc,

I put the numbers in to the Mach calculator, and it seems pretty fast (if I did it right). The RPMs puts me over the 5100, and the feedrate seems quick...is this a time where one should intuitively jump to a larger cutter if possible? See attached.

I always use the largest cutter possible, up to the point that side tool pressure will overcome wall thicknesses, work holding or cause chatter issues. Depending on the actual pocket size to be cut, with 0.070 walls, I would venture a 1/4" tool could be used with no problems. If smaller inside radii are needed, rough with the 1/4" and finish with something smaller.

5100 RPM on a 5/64" tool with coolant should not be too fast. As I said, 150 SFM is the maximum for this material with a carbide tool, which would be 7346 RPM. At 5100 RPM, that is 104 SFM. At 5100 RPM, and 0.002" chip load on a 4 flute tool, your feed would be 40.8 IPM. The 40.8 feed is what I would use at 50% axle depth of cut and 40% radial depth of cut. For 50% axle depth of cut, and 100% radial depth of cut, I would use 20.2 IPM as my starting feed. I never plunge any tool more than 10 IPM. In this case I would plunge at 4 IPM or less on the 0.078" tool.

[tbaker2500]

Paul-
I highly recommend downloading the 30-day trial of G-Wizard and playing with test numbers. The big thing you should pay attention to, when using small cutters (and I even mean 1/4" as small) is tool deflection. Switch to "Advanced" mode, and look at the tool deflection number. If it is in orange, there is a strong possibility you will break the tool. If not right away, then soon. This double-check has saved me many tools. And as always, use the biggest tool you can. And the shortest tool, also. Stickout from holder makes a big difference on tool flex.

Keep experimenting, and have fun!

[Steve Seebold]

You want maximum SFM to be about 150. Do you know how to calculate RPM from SFM? Chip load should be about 0.002" to 0.0035" per tooth. Do you know how to calculate feed rate after you have calculated RPM?

That's way too fast for titanium. You should be running your spindle at 20 to 25 surface feet per minute, 2.8 IPM feed. That's .0007 per flute at 1,000 RPM and don't plunge into your part. Ramp or helix in. If you plunge, you'll break a cutter every time.

Titanium works exactly the same as aluminum but at 15% of the feed and speed.

Calculate your feed rate RPM times the amount par flute times the number of flutes.

Good luck.

Clean your machine and save your chips. They're worth a couple of bucks per pound.

[txcncman]

That's way too fast for titanium. You should be running your spindle at 20 to 25 surface feet per minute, 2.8 IPM feed. That's .0007 per flute at 1,000 RPM and don't plunge into your part. Ramp or helix in. If you plunge, you'll break a cutter every time.

Titanium works exactly the same as aluminum but at 15% of the feed and speed.

Calculate your feed rate RPM times the amount par flute times the number of flutes.

Good luck.

Clean your machine and save your chips. They're worth a couple of bucks per pound.

According to the above information, since I run aluminum at 850 SFM, titanium should be run at 127.5 SFM. And since my chip load on aluminum would be about 0.008", titanium chip load would be about 0.0012". Hey, maybe my numbers were not that far off to begin with.