Part of me says, "of course you can, if you go slowly and use the right bits" to this question, but since I have yet to see any mention of people cutting titanium on their Taig, I have to ask.
I know there are many custom knifemakers that use a Taig in their shops for various operations. And Titanium is used quite a bit these days in high end knives, especially stuff like Timascus for knife handles....
So, has anyone cut titanium on their Taig mill? If so, how- what bits and speeds did you use? If you think it could, what kinds of bits would you think are needed?
Never cut titanium with it? Well, what was the hardest material you ever cut with it? Tungsten? G-10? Kevlar sheet?
Largest resource on the web about Taig lathes and mills
I knew it could be done. I just wanted to make sure of it- I plan on working with Titanium block a lot.
Since I am new to the tooling aspect of all this, I've seen that endmills can have 2 or more flutes. People seem to recommend 2 flutes for softer materials like aluminum, and 4 for harder materials.
That 1/32" dia HSS end mill- how many flutes did it have? Would carbide or tungsten carbide endmills work well on titanium, or ruin? What about bits with this TiAlN coating I keep seeing on many endmills? Any thoughts?
A lot depends on the alloy in question, but when machining titanium you want to make sure that you are not letting the tool dwell or rub in the cut. This will work harden the Ti, and ruin your day. Ti can also be very springy, so pay attention to setups, so that you don't have the part flopping around. It's not just finish that suffers, if the part bounces too much you will stop taking cuts, leading back to the dwelling and day ruining.
Escott- how would you recommend securing titanium plate, or round stock?
Cartertools- You're the one I'm ordering from shortly, within a week, once I figure out all I need, so I'll just ask here- since I plan on machining a lot of titanium (hopefully), do you carry any endmills you'd recommend for it?
To everyone- how many flutes should an endmill for cutting titanium have? Again, is tungsten carbide a bad thing to use with it, or good?
Also- I plan on squaring up large flats on the stuff too, so what sort of flycutter can handle/be ideal for use with titanium?
Can anyone link specific bits they have or would use on this stuff, so I can get an idea of what I should be looking for?
Thanks again for these great tips.
Round stock gets better, vise, lathe chuck, or I like a collet block chuck if the part is under 1.125" in diameter.
I would use a 4 flute, probably carbide. Thinner cutters are going to be more prone to flex, and I'd use as short a tool length as you can.
Working with titanium is not very difficult. If is CP grade titanium, then it is cake walk.
If it is Titanium alloy, then you need to have some strategy before cutting it as it will work harden very fast. For Ti alloy sheets, try wire-edm or water jet or plasma cutting before considering cutting using any other tools.
Titan Engineering, Singapore. Titanium Metal & Alloy suppliers.
I'm afraid. I read this thread: Who makes the best end mills?
I am beweildered at all the possible makers and options of endmills.
All I've gathered so far is that the harder the material, generally, the more flutes your endmill should have for good cutting results.
So far, after scrutinizing that thread, I've come up with a couple endmill lines that might work well for titanium, and in general.
#1. SGS Z-Carb series.
#2. Destiny Tools Raptor Line.
All these years, I figured if I had the machine, I could make what I wanted, because I knew what I needed to do to shape and cut to get what I wanted.
Now, I'm not so sure- I have a feeling I'll end up destroying a lot of material and endmills because I have no way of knowing which endmill I should use for what, much less where to get things at a good price, when there's so many distributors and levels of quality.
Anyone have recommendations for SPECIFIC bits from specific makers that work really well for them with Titanium? Ie: carbide or HSS, number of flutes, size, speeds, etc. Why don't we start a stickied thread where we post specific bits and materials they work exceptionally well on (limited to what users cut here on Taigs).
And finally, what simple cart & basket, online prices listed site do people here recommend for buying endmills & flycutters?
I don't mean to offend, but you really should spend some time reading things like machineries handbook, and other texts dedicated to explaining in great detail what you need to know to cut metal. Forget specific brands, it's not going to give you the results you need. Instead, understand the process, then pick the tool which helps you achieve it.
Metal wants to be cut within a range of speeds. The outer edge of the tool should move at a given speed for a particular alloy of work, tool material and within machine tool limitations. This determines how fast you spin the tool. The formula Pi*Tool Diameter*RPM will give you the surface speed (remember to keep units straight, to get surface FEET per minute, which most tables are in, remember to divide inch measurements by 12). There are tables which show recommended speeds given material type.
Now that you have a speed figured, you need to figure out how fast to push the tool through the work. Manufacturers (reputable ones) give a number called the chipload, which can be thought of as a "feed per tooth". It's how much of a bite you take off with each tooth of the tool. Given the RPM, and a feed rate, you can calc your chipload.
If you plug in a couple numbers, you'll see that in order to keep the chipload correct, you wind up feeding a 2 flute endmill exactly 1/2 as fast as the 4 flute. This is why you see 4 flutes (and more) used on harder materials. Harder materials generally require lower speed of tool, which already lowers the feed rate. Use only two flutes, and it lowers even more, making jobs take forever.
None of that takes machine rigidity or work holding into consideration, which can mean an adjustment of the above numbers to suit available conditions, or a reduction in cut depth. There are CAM programs that will do a lot of the grunt work for you, calcing speed and feed for a given set of materials, I work with both MasterCAM and GibbsCAM at work, and both have pre-made tables, but these still require review and adjustment by the guy making the cuts. There's no substitute for experience in some respects.
Don't let that get you down though, it's all a journey. I've ruined tons of tool bits and tons of workpieces. Anyone who's spent any time in this field has. But if you take something from each one, it's certainly not a loss. With every one I figure out something I shouldn't have done, and learn something for next time.
As for vendors I've NEVER had a bad time with McMaster Carr. They will charge a bit more than some others, but they have what you need, likely in stock, and every tool I've ever got from them has been quality. Their web site is second to none, and if you can get your hands on a catalog (they generally only send them to a business) it's got great info in it. MSC is also good, as is Enco, but there are crappy tools at both of those if you don't know what you are looking for.
Escott, thank you very much for not belittling me, and being so helpful. If more people treated newbies like you, we'd be a lot better off!
I am a college grad, and my alma matter has an amazing engineering library open to public use, with more books than I could throw a stick at. I don't think anyone except current engineering students can check anything out, however. Still, I could spend a day every once in a while to read tomes on materials cutting to accquaint me.
I actually started as an engineering student, but became a linguist. Organic chemistry destroyed me, but I was amazing at calculus. In any case, I know that everything I've been reading today shows me I can understand this stuff at a deeper level, and I want to try. I also know that I will probably try starting without the knowledge anyway, because books are only so helpful. And I want to make things BADLY. I learn best by doing, anyway, so I'll probably pick some bit I think will work, and go at it.
Can you recommend any specific one book that best accquaints someone with cutting tool choice/metal removal methods? If there is a beginner's book for machinists or something, that still remains current with the advent of carbide & PCD tooling, I'd like to find and read it.
In the meantime, what bit specifically would you recommend for titanium, especially considering its nasty work hardening habit? I'm talking standard 6Al-4V.
6-4 is alloy Ti, and is one of the ones which work hardens. I've worked a reasonable amount with that particular alloy, and it isn't that fun. It's not something me or anyone else can say "here, this bit will work" It doesn't work that way, and short of someone running that alloy on the same machine, with similar cut depth, feed rate and spindle speed can give you. Most of the 6-4 I've cut is on a Haas TM1 which is substantially bigger than a TAIG. I used a selection of HSS and carbide to get my work done.
If you are unfamiliar with things like how to calculate feed rate and spindle speeds, and adjust these based on your machine, don't start out cutting 6-4. All it's going to do is upset you, and you'll get frustrated. Start with something softer, like Aluminum or even machinist wax, then work your way up. Nobody starts making the most difficult parts from the most difficult material.
I'll repeat this again, since you seem to have ignored it, if you are trying to cut blanks out of sheet Ti, there are better ways to get the work done, contact job shops in your area to see about abrasive waterjet, plasma, wire edm, or laser cutting. Waterjet, plasma and laser cutting are very fast, waterjet is most likely going to be the least expensive of these. If it was me I would get the blanks cut with one of these methods (a little easier for me since I work at a place with a couple of lasers) and then do finish work with my mill. Choose the correct process, especially if you are trying to make money at this.