CNC Tooling

[sanddrag]

Originally Posted by Mr. Mike

Another CAD/CAM package to check out is BobCad. They have sales every so often. We purchased 2 seats of mill and lathe for $1,500.

I evaluated BobCAD/CAM (along with half a dozen others) and I can't say I'd recommend it based on my 2 hour demo of it. The UI and workflow seems primitive and complex compared to some other software packages. Also, once contact is initiated, be prepared to deal with their relentless sales force. You're basically on their contact list for life at that point, and you'll hear from them at least twice a month.

[James Tonthat]

Originally Posted by sanddrag

I evaluated BobCAD/CAM (along with half a dozen others) and I can't say I'd recommend it based on my 2 hour demo of it. The UI and workflow seems primitive and complex compared to some other software packages. Also, once contact is initiated, be prepared to deal with their relentless sales force. You're basically on their contact list for life at that point, and you'll hear from them at least twice a month.

We used HSMXpress last year for all our milling and worked for everything that we needed it for (pocketing, countersinks, bosses, contours, etc.). You provide your email address in exchange for their free version (HSMXpress, HSMWorks is their paid version). I think they emailed me once if I was interested in HSMWorks and haven't contacted me since. It's a pretty easy to use package with really good Solidworks integration. They were purchased by Autodesk a bit ago so they're working on an Inventor version.

One of the good parts of having a plug in program into your CAD program is when you do rev's they'll automatically rebuild into your CAM program so that all you need to do is re-post it for your G-code.


The 1/4" EM was definitely our workhorse last year and when we were newbs at it, we'd have it cut with the tip of the EM (broke a couple EM's). I later on predrilled a lot of the paths with a 1/4" drill then entered maybe 1" into the material using the top of the EM closer to the tool holder. It's all about balancing heat, your tools, your fixturing, and your machine. You'd be surprised how much you can push your tools with the HP/revs you have.

[techhelpbb]

Originally Posted by sanddrag

I evaluated BobCAD/CAM (along with half a dozen others) and I can't say I'd recommend it based on my 2 hour demo of it. The UI and workflow seems primitive and complex compared to some other software packages. Also, once contact is initiated, be prepared to deal with their relentless sales force. You're basically on their contact list for life at that point, and you'll hear from them at least twice a month.

BobCAD is extremely aggressive about sales.
A bit too aggressive at times.

I find there interface a bit old fashioned in visual style but I have found that depending on your perspective of the CAD/CAM/CNC workflow BobCAD can be great product. I own a few versions with and without dongles.

There is unfortunately a learning curve.
I had the same trouble the first time I used it.
Once I got the hang of it things went smoother.
I could never have made due with a 2 hour demo either.

Originally Posted by Mr. Mike

• When it comes to cutting aluminum, stay away from any coatings that are gray to black. They are TiAlN (Titanium Aluminum Nitride), AlTiN (Aluminum Titanium Nitride), and TiAlSiN (Titanium Aluminum Silicon Nitride). Aluminum will stick and nasty thing will happen.

Does this not depend on the speed of the spindle?

Usually you have to spin the TiAlN end mills at higher speeds to make the coating operate as intended (18k to 22k RPM).
You would not want to use a TiAlN end mill too slowly or it will be worse than an HSS end mill.

Then there's the other issue, the higher the spindle speed the higher the IPM you need to move or risk rubbing. Not a problem for good machines but a problem for light weight gantry mills.


Generally and not in reply to anyone:
I linked this in a topic in the motor section but I will link it here as well:
http://blog.cnccookbook.com/2012/03/...tting-success/
Props to scottandme for posting a reference to G-Wizard as well (last page).

The issue I have with this topic is that I suspect that the different teams have different CNC machines.
A servo driven bridge or turret mill will have different requirements than a stepper driven gantry mill.
The bridge or turret has greater rigidity.
Depending on the spindle operating range it will impact the IPM.

It is hard to pick out what machine is what.
Some of the machines might be using steppers and therefore must target lower IPM feeds.
Some of the machines might have less cooling.
Some of the machines might have higher speed spindles with no ability to go slower.
The key elements that make this work depend on the knowing the machine sore spots.

For example:

Originally Posted by sanddrag

On our router at ~20,000 RPM, we've had a lot of trouble cutting aluminum with a standard 1/4" 3 flute carbide variable helix endmill we use with great results at 6,000 RPM with coolant on the mill. On the router, it just wants to load up and melt/weld chips. I'm thinking a 2-flute would give better chip evacuation.

Currently, our coolant system on the router is a student and a spray bottle of WD40.

I assume the mill in question is a turret type like a Bridgeport?

At this link...
http://www.daycounter.com/Calculator...lculator.phtml

Plug in 0.25", 300SFM, 3 flutes.
You get: about 4,500 RPM, 27.5 IPM
Makes sense that this works.

Plug in 0.25", 1,310SFM, 3 flutes
You get: about 20kRPM, about 120 IPM
This is probably not going to work.
I would be a bit suspicious of a carbide end mill rated at 1,310SFM uncoated.
Even more suspicious if your router can sustain the feed rate to keep it from rubbing.

At a spindle speed of 20kRPM I think you should consider a TiAlN end mill for the router with 2 flutes and 1/8" diameter.
That would get you:
655SFM, 20kRPM spindle speed, 80IPM feed.
If your gantry mill is outfitted with either really powerful steppers or servos it will work.

Try this:
http://www.wttool.com/index/page/cat...lls+%28USA%29/

Otherwise if you can't get the power from the steppers on your gantry:
Use a single flute as others have suggested and you'll divide that feed rate in half.
At that point if it's not enough edit your depth of cut and tool path to accommodate.

[scottandme]

Originally Posted by techhelpbb

Does this not depend on the speed of the spindle?

Usually you have to spin the TiAlN end mills at higher speeds to make the coating operate as intended (18k to 22k RPM).
You would not want to use a TiAlN end mill too slowly or it will be worse than an HSS end mill.

Anything with Al in the coating will not work to cut aluminum. Mainly for chromoly steels, stainless, titanium, nickel alloys, etc. They need high temperatures to "activate", which requires high SFPM numbers. From what I understand it actually creates a thin film of aluminum oxide when it hits that activation temperature. That's purely dependent on the size of the cutter and the material - but 18 to 22k is pretty extreme for a VMC - that's a specialized machine. Most are in the 8k to 12k range give or take. Generally with those cutters they don't use coolant (same with many carbide/ceramic insert cutters), just a heavy air blast to clear chips. The coolant can cause the insert to fracture from thermal shock.

For aluminum you either want uncoated, ZrN, or TiB2. TiCN can work well, but avoid TiN. Most major brands make geometry specifically for cutting aluminum (higher helix, polished flutes, etc, etc).

[techhelpbb]

Originally Posted by scottandme

Anything with Al in the coating will not work to cut aluminum. Mainly for chromoly steels, stainless, titanium, nickel alloys, etc. They need high temperatures to "activate", which requires high SFPM numbers. From what I understand it actually creates a thin film of aluminum oxide when it hits that activation temperature. That's purely dependent on the size of the cutter and the material - but 18 to 22k is pretty extreme for a VMC - that's a specialized machine. Most are in the 8k to 12k range give or take. Generally with those cutters they don't use coolant (same with many carbide/ceramic insert cutters), just a heavy air blast to clear chips. The coolant can cause the insert to fracture from thermal shock.

For aluminum you either want uncoated, ZrN, or TiB2. TiCN can work well, but avoid TiN. Most major brands make geometry specifically for cutting aluminum (higher helix, polished flutes, etc, etc).

So you are basing this on the VMC (Vertical Milling Center) not being able to obtain those high spindle speeds in general?

What if they are using a standard shop router(19kRPM - 25kRPM) or a RotoZip (15k-30kRPM) for a spindle on a homemade gantry?

Course the price they pay is not just for the coating it's also that they will need a high feed rate.
A high feed rate most smaller steppers would have difficulty achieving.

I agree with you if you slow down the spindle and operate more in the range of 8k-12k TiAlN is the wrong coating to use.

Without knowing what sort of machines each team is trying to use it gets a bit more involved.

[scottandme]

Originally Posted by techhelpbb

So you are basing this on the VMC (Vertical Milling Center) not being able to obtain those high spindle speeds in general?

What if they are using a standard shop router(19kRPM - 25kRPM) or a RotoZip (15k-30kRPM) for a spindle on a homemade gantry?

Course the price they pay is not just for the coating it's also that they will need a high feed rate.
A high feed rate most smaller steppers would have difficulty achieving.

I agree with you if you slow down the spindle and operate more in the range of 8k-12k TiAlN is the wrong coating to use.

Without knowing what sort of machines each team is trying to use it gets a bit more involved.

There are plenty of different coatings available if you look through a major supplier catalog. All different geometries and designs for different materials, as well as several different coatings. For aluminum - regardless of machine, TiAlN is a bad choice. The aluminum will have an affinity for the Al in the coating and will gum up. For aluminum geometry you generally want a high helix angle to help chip evacuation, a large gullet to allow plenty of space for the chips to eject, and a sharp cutting edge. Coatings that work well in aluminum are ZrN, TiB2, and TiCN. Uncoated works perfectly fine as well. Generally they make the surface harder and smoother to prevent the chips from welding to the surface of the tool. With aluminum coolant is normally used to help eject chips, add some lubricity, and keep chips from welding to the surface of the tool.

For a router in particular - the best option is using a carbide single flute tool. Carbide can run high SFPM numbers in aluminum, so that way if your router is 8-10K minimum speed you won't be burning up the tool. Single flute does two things well. Firstly, it gives a ton of room for the chips to evacuate so that they don't pack up in the gullets of the end mill and cause the tool to load up with aluminum, stop cutting, and snap. The second is derived directly from the speed and feed formulae. Say each tooth needs to be taking 0.002" per revolution so that it doesn't start "rubbing" as opposed to cutting. If you have one flute, that means you're only moving 0.002" per revolution of the tool. If you have a 4 flute tool, each tooth needs to take a 0.002" bite, so you have to move 0.008" per revolution of the tool to maintain proper chip load. On a router that can be the difference between a manageable feed rate, and something that the machine cannot achieve.

For example - you have a router that can vary from 10K to 20K RPM and you're using a 1/4" end mill to slot.

I would use a single flute uncoated carbide end mill. Depending on the specific tool, SPFM in 6061 can be anywhere from 800 to 2000 SFPM. You can run slower, but running fast will wear the tool prematurely. A 1/4" tool running 800 SFPM is 12,200 RPM. Perfect, right in the range for our router spindle. Now finding the feed rate is just (spindle speed * # of flutes * chip load). Say we're being conservative and taking 0.002"/tooth. That means our feed rate is only 24 inches/min. Any machine on the planet can do that without worrying about acceleration in curves, angle changes, etc. If we want to go faster, we can bump up to 20k on the spindle (~1300 SPFM, likely fine for carbide), and the feed rate jumps up to 40 inches/minute. Perfectly achievable numbers, the tool isn't going to burn up or rub, and we have a ton of room for chips to jump out (only one flute!).

If you like 1/8" end mills, then you can run 24 IPM at 12,200 RPM (0.002"/tooth and only 400 SFPM), or 40 IPM at 20k RPM (0.002"/tooth and 650 SPFM).

Using a two flute cutter doubles those feed rates while keeping the spindle speed the same. Three flute triples, and so on. But now you have increasingly little room for the chips to evacuate, especially with a smaller 1/8" end mill. Your previously reasonable 25-40 IPM feed is now up to 100-160 IPM on a 4 flute tool, and you'll need to be taking a shallower cut if you run out of HP in your spindle.

As for the first part - TiAlN is perfect if the situation is correct. Here's Niagara's chart: http://www.niagaracutter.com/techinf...d_solcarb.html

Say we're cutting 300-series stainless (over 32 rockwell C). We would probably want to be using an air blast to clear chips, and let the coating do the work. We need to coating to heat up to work properly, so here we don't want to be under the recommended SFPM numbers.

So say a 3/8" 4 flute end mill - chart reads 100-150 SFPM and 0.001"/tooth. TiAlN coating adds 60-100% increase in SFPM. So we're somewhere between 160 and 300 SPFM. Let's use the high end - that gives us all of 3,000 RPM and 12 inches/minute. That's why most big VMC's don't really need insane spindle speeds unless they're running aluminum, copper, brass, etc. Even with the coatings, most jobs in steel, stainless, titanium, etc aren't going to going that fast. After that you'll have to start reading about HSM and radial chip thinning, etc, but that's way beyond the scope of this.

[techhelpbb]

Well I am confused then.

Cause I not 7 days ago used a TiAlN 1/8" end mill, 2 flute on aluminum.
With coolant and it was hardly a new end mill for that purpose.
I am not the only one either.

So I guess the question I have is at what operating temperature is this coating appropriate?
Since the question here appears to come down to whether or not it can reach that temperature.


Answering my own concern:
I have a long commute so I decided to call around to Duramill and Niagara.
Spoke with the technical folks not sales.

The reason the coating operating temperature is not specified is apparently because they consider the TiAlN coating inert.
It shouldn't want to bind chemically to aluminum any more than Titanium (no affinity according to Niagra).
The coating provides hardness and durability till the yield temperature well over 1,000 degrees Celsius.
This differs from aluminum titanium nitride which is high in aluminum and therefore is an active coating.

The issue they clarified is that aluminum will of course melt well into the safe operating temperatures of these bits.
So you don't have to hit a certain temperature to make them work.
However just because the bit will withstand these temperatures does not mean the aluminum you are working won't melt and wet the bit.
Obviously once the aluminum melts and wets the bit welding will soon follow.

The reason my machines are not experiencing that issue is because I do not cut aluminum without coolant.
Therefore I am cooling everything.
I do not consider the cooling to be really heavy duty so the bit does get hot.
However the aluminum being worked is basically a heatsink and the coolant cools that.
The gantry mills I have used TiAlN with are pretty rigid. I have seen much worse.
Also I am aware that aluminum tends to melt so I take measures to keep moving.

This is why there is no minimum desirable operating temperature specified.
This is also why it works for me.
I told both companies that I've used these with aluminum and no huge red alarms went off.


However I still agree a slower spindle is desirable for this purpose.
It would eliminate the need for the tool that could be a bit more expensive.
Additionally it would reduce the risk that a slow cut would weld.

[scottandme]

Originally Posted by techhelpbb

This is why there is no minimum desirable operating temperature specified.
This is also why it works for me.
I told both companies that I've used these with aluminum and no huge red alarms went off.

I'm surprised that they said that - I've heard plenty of people having issues when they tried to run TiAlN in Aluminum and had issues with build up edge forming, surface smearing ruining the finish etc. Could have been your cut parameters being moderate enough that it wasn't noticable, or the cut was generating minimal heat (quite likely with a small 1/8" end mill). I guess best case you're paying a decent amount of $$ over uncoated without an appreciable benefit compared to other coatings.

Either way - the proof is in the products that they sell. Duramill and Niagara don't put that coating on their aluminum-specific end mills. They both sell either uncoated or TiCN coating on those tools. They're both a bit behind the curve on aluminum coatings it seems, since ZrN and TiB2 are being used in many other mfg's high end aluminum products. We've used the Niagara aluminum specific end mills with TiCN since McMaster sells them and it's convenient (AN3xx series). They work well, but I can't speak to if they're appreciable better than uncoated - we don't push our machines that hard and they're not being run 24/7 to notice any difference in longevity.

I have never seen anyone sell an aluminum specific end mill with TiAlN on it - uncoated, TiCN, ZrN, TiB2, and DLC are the only ones I can remember seeing. I've also never seen aluminum as a recommended material for TiAlN or AlTiN.

Originally Posted by techhelpbb

However I still agree a slower spindle is desirable for this purpose.
It would eliminate the need for the tool that could be a bit more expensive.
Additionally it would reduce the risk that a slow cut would weld.

It doesn't really matter - you want to run carbide with smaller cutters. For one, the price difference is usually minimal compared to HSS. Carbide is significantly more rigid that HSS, which is especially helpful for small diameter cutters. And even uncoated carbide has almost no speed limit in aluminum. Cuts weld if the SFPM is too high, chip load is too low, or the chips aren't being ejected from the cut. So to fix the first you use carbide, to fix the second you use a single flute cutter so you can maintain proper chip load at lower feeds, and that also fixes #3 by giving room for chips to eject.

If it's on a mill and not a router, then you still want to use carbide if only for the rigidity benefits.

[techhelpbb]

Originally Posted by scottandme

I guess best case you're paying a decent amount of $$ over uncoated without an appreciable benefit compared to other coatings.

Not so sure about the $$ I paid < $10 for those 2 flute end mills including shipping and handing quite some time ago. In a production operation with various tool paths I can't say I consider that expensive.

I called both because I was curious if one would say the opposite of the other. I've never experienced the issue you have.

I did expressely mention that other people were telling me they were having issues with TiAlN in aluminum and they both stated it depends on a lot of factors like the feed rate, the coolant, the rigidity. So your mileage may well differ from mine.

I have never seen anyone sell an aluminum specific end mill with TiAlN on it - uncoated, TiCN, ZrN, TiB2, and DLC are the only ones I can remember seeing. I've also never seen aluminum as a recommended material for TiAlN or AlTiN.

I can't say that any of the TiAlN coated end mills I've used expressely stated that they were designed for aluminum. I don't necessarily use a rule of thumb for setting up for aluminum either. However I can't really say that router typically used for wood or a RotoZip was really designed for this purpose either. I don't use TiAlN coated end mills unless the RPM of the spindle is for some reason high and I can't adjust it down.

It doesn't really matter - you want to run carbide with smaller cutters. For one, the price difference is usually minimal compared to HSS. Carbide is significantly more rigid that HSS, which is especially helpful for small diameter cutters. And even uncoated carbide has almost no speed limit in aluminum. Cuts weld if the SFPM is too high, chip load is too low, or the chips aren't being ejected from the cut. So to fix the first you use carbide, to fix the second you use a single flute cutter so you can maintain proper chip load at lower feeds, and that also fixes #3 by giving room for chips to eject.

If it's on a mill and not a router, then you still want to use carbide if only for the rigidity benefits.

Most of all these bits with TiAlN coating are carbide inside anyway so I agree this is one of those little things.
The core advice is still the same.

Originally Posted by Cory

If you tried to run one of those end mills under aluminum specific parameters (1000+ SFM, .003"+ chip load) you will load it up and break it-guaranteed. This is as much because of the geometry being wrong as it is because of the coating, as the only tools that are ever coated with those are meant for ferrous materials.

Well if you try the calculator on the page I linked before:
1,000SFM with an 1/8" mill gets you a spindle RPM of around 30,500 RPM.
With a tooth load of 0.003 and 2 flutes you get: about 183 IPM feed rate.

I have a lot of people I've worked with that only dream about 183 IPM feed rates their systems could not achieve that.
They would be missing steps.

If you increase the diameter to 1/4" you'll get down to about 15k RPM and 91 IPM or so that's more practical for large steppers and closed loop servos.

Originally Posted by Cory

I'm not sure why they told you that you don't want to run the tool at elevated temperatures. I forget where it is exactly, but somewhere between 700-800C the coating dramatically increases in hardness. As previously mentioned this is why people don't cut ferrous metals with coolant when using those coatings.

There are many studies on TiAlN here is one that specifically mentions 800 degrees Celsius.
http://www.geocities.ws/sarangrh/report/seminar.pdf

TiAlN is the most recently developed coating with a hardness of 3300 HV and is
temperature resistant up to 800°C i.e. Excellent Stability at High Temperature and
Smooth Tool Surface, Balanced Wear Resistance and Fracture Resistance, allowing the
use of ultra high-speed machining operations. This multi-purpose coating is also suitable
for working cast-iron, High Speed Turning of Stainless Steel and Al alloys and reduces
friction and adhesion of plastics materials to the moulds. New applications are found
every day with this very efficient, high productivity tool.

Further we can ask a company that does coating what they recommend:
http://www.pvd-coatings.co.uk/coatin...tialn-coating/

TiAlN coating – Applications
The properties of the TiAlN coating make it suitable for high temperature cutting operations with minimum use of lubricant or dry machining. TiAlN is used successfully to machine titanium, aluminium and nickel alloys, stainless steels, alloy steels, Co-Cr-Mo and cast irons. TiAlN is also used to protect dies and moulds that are required to operate at high temperatures such as those in medium and hot forging and extrusion industries.

Though I never try to machine aluminum without coolant.
It does not specifically say you'd want to machine aluminum dry.

Originally Posted by scottandme

Either way - the proof is in the products that they sell. Duramill and Niagara don't put that coating on their aluminum-specific end mills.

Niagara Cutter 86002 Carbide Square Nose End Mill, Inch, TiAlN Finish, Roughing and Finishing Cut, 30 Degree Helix, 3 Flutes, 1.5" Overall Length, 0.125" Cutting Diameter, 0.125" Shank Diameter

Niagara Cutter A245 Carbide End Mill for Aluminum, TiAlN Coated, 2 Flutes, Square End, 4-1/8" Cutting Length, 1" Cutting Diameter

http://www.drillmex.com/img/PDF/NIAGARA/A245.pdf

[scottandme]

Originally Posted by techhelpbb

I did expressely mention that other people were telling me they were having issues with TiAlN in aluminum and they both stated it depends on a lot of factors like the feed rate, the coolant, the rigidity. So your mileage may well differ from mine.

"It might work" isn't the same as saying it's a recommended coating. If you call and ask "What tool coating is preferable for machining of aluminum?", they will not respond by saying TiAlN. That's why they don't sell it as a coating on their aluminum specific geometry tools, just uncoated or TiCN. Other companies run coatings designed for Aluminum - ZrN, TiB2, DLC, etc. Niagara and Duramill don't offer those for whatever reason, but SGS, OSG, Havey Tool, Melin, Maritool, Destiny, Lakeshore Carbide, etc, etc all do.

Originally Posted by techhelpbb

Well if you try the calculator on the page I linked before:
1,000SFM with an 1/8" mill gets you a spindle RPM of around 30,500 RPM.
With a tooth load of 0.003 and 2 flutes you get: about 183 IPM feed rate.

I have a lot of people I've worked with that only dream about 183 IPM feed rates their systems could not achieve that.
They would be missing steps.

If you increase the diameter to 1/4" you'll get down to about 15k RPM and 91 IPM or so that's more practical for large steppers and closed loop servos.

Again, conflating routers and mills here. For routers - use the Onsrud single flute carbide cutters. They solve all of the issues with having high minimum RPM and limited feed rates and acceleration profiles. 1/8" end mill - 20,000 RPM @ 40 IPM. 1/4" end mill - 20,000 RPM @ 60 IPM. Doable on any junky stepper machine.

If the feed is too extreme for the router, just drop the spindle speed. If you're cutting aluminum on a router you should really skip the silly hand routers and buy a model with a VFD controlled spindle anyway. Good uncoated carbide is perfectly happy at 1,000 SFPM and up.

For mills - you're going to be spindle speed limited in aluminum on most cutter sizes, but they're able to maintain higher feeds without issue. Even the Haas TM machines are rated for 400 IPM, and that's still plenty considering the machine size/HP.

Your feeds will be much slower just based on the max RPM for the machine. 1/4" 3 flute end mill - 6000 RPM, 54 IPM @ 0.003"/tooth. 1/2" 3 flute end mill - 6000 RPM, 90 IPM @ 0.005"/tooth. You will probably get higher MRR at lower RPM just because the HP falls off on the Haas machines at higher RPM's anyway.

Originally Posted by techhelpbb

Further we can ask a company that does coating what they recommend:
http://www.pvd-coatings.co.uk/coatin...tialn-coating/

Not exactly the most reputable site. Find any cutting tool company that recommends TiAlN for aluminum. Find any cutting tool company that sells aluminum specific geometry, and see what coating they put on the tool. It's not TiAlN.

[techhelpbb]

Originally Posted by scottandme

That's why they don't sell it as a coating on their aluminum specific geometry tools, just uncoated or TiCN. Other companies run coatings designed for Aluminum - ZrN, TiB2, DLC, etc. Niagara and Duramill don't offer those for whatever reason, but SGS, OSG, Havey Tool, Melin, Maritool, Destiny, Lakeshore Carbide, etc, etc all do.

In fairness I just added the links for that exact product offering from Niagara to my post above. So you probably didn't see that when you posted this.

Not exactly the most reputable site. Find any cutting tool company that recommends TiAlN for aluminum. Find any cutting tool company that sells aluminum specific geometry, and see what coating they put on the tool. It's not TiAlN.

Again look up at the end of my last post. Niagara sells those bits with TiAlN coating specifically for aluminum. So let's not so hastily assume that the coating company I linked is also self-promoting.

Here:

Niagara Cutter 86002 Carbide Square Nose End Mill, Inch, TiAlN Finish, Roughing and Finishing Cut, 30 Degree Helix, 3 Flutes, 1.5" Overall Length, 0.125" Cutting Diameter, 0.125" Shank Diameter

The end mill above led me to the end mill below...

Niagara Cutter A245 Carbide End Mill for Aluminum, TiAlN Coated, 2 Flutes, Square End, 4-1/8" Cutting Length, 1" Cutting Diameter

Which gave me a reference to search for this...

http://www.drillmex.com/img/PDF/NIAGARA/A245.pdf

Here's the 1/8" TiAlN end mill for sale as factory stock:
http://www.kaufmanco.com/itemdetail/NIA%2061489

Parting that series at the same distributer:

61351 = Uncoated = $13.98
http://www.kaufmanco.com/itemdetail/NIA%2061351

61443 = TiCN = $24.21
http://www.kaufmanco.com/itemdetail/NIA%2061443-030

61480 = TiAlN = $15.63
http://www.kaufmanco.com/itemdetail/NIA%2061489

[scottandme]

The first EM listed isn't for aluminum. No idea about the second one. Looks like you found an outdated catalog page from a French tool supplier. Note how TiCN is the one highlighted as "recommended".

Here's the real A245 catalog page from Niagara's website in case anyone else is interested (uncoated or TiCN only). We've used the A345 (3 flute) with great success, they're good quality end mills.

http://www.niagaracutter.com/solidca...um_ss/a245.pdf

It's pretty clear you have your mind made up and don't want to listed to what Cory and I are saying. For anyone else following this boondoggle - here's what I would recommend.

Using a router? Buy Onsrud's singe flute cutters (63-600 series) - McMaster under "Router Bits for Aluminum" (ex PN 3317A21, 3317A25).

Using a mill? Check out Maritool (Uncoated, ZrN, DLC) or Lakeshore Carbide (ZrN). McMaster sells the TiCN Niagara tools (High-Performance Carbide End Mills for Aluminum).

http://www.maritool.com/Cutting-Tool...201/index.html

http://www.lakeshorecarbide.com/vari...raluminum.aspx

[techhelpbb]

Originally Posted by scottandme

It's pretty clear you have your mind made up and don't want to listed to what Cory and I are saying. For anyone else following this boondoggle - here's what I would recommend.

Considering that you are basically telling me I am not doing what I am actually doing? Yeap.
Even your own link points to the same part numbers.
Even if you want to say they don't make these any more you wrote they did not make them at all.

Using a router? Buy Onsrud's singe flute cutters (63-600 series) - McMaster under "Router Bits for Aluminum" (ex PN 3317A21, 3317A25).

Using a mill? Check out Maritool (Uncoated, ZrN, DLC) or Lakeshore Carbide (ZrN). McMaster sells the TiCN Niagara tools (High-Performance Carbide End Mills for Aluminum).

http://www.maritool.com/Cutting-Tool...201/index.html

http://www.lakeshorecarbide.com/vari...raluminum.aspx

Never said TiAlN was the only option. Go back and look. Don't much like people assuming I did when there's no evidence to support the claim. None the less I will once again agree with you with the right machines these are perfect tools.

I *only* use TiAlN mills with specific circumstances and *never* suggested otherwise.

I am very disappointed in the way you are reacting to this.
However it is utterly irrelevant to the fact that it does work.

Before it was implied that people were surpised that Niagara would suggest the applicability of TiAlN even though they don't sell it well that can't be a fact.
If you simply look through the Niagara price list the TiAlN end mill part numbers are still very much in there.
Both the PDF and the ASCII price list dated January 7th, 2013.
Old or not they obviously have experience with this coating on aluminum.

Now if I were in Niagara's shoes and I was selling a product that a whole bunch of people made a directed effort to dismiss I would probably shelve it as a matter of business as well. Regardless of the product quality or track record if enough customers simply decide it is not for them the volume of sales would plummet (like what would happen if a bunch of people kept going after people over it...sort of like what people often do to BobCAD and MasterCAM). It sure seems like this is a little too much peer pressure for a simple matter like this. So I guess I know why Niagara outright said to me it's just not worth worrying if they disagree. I haven't even bought these products from Niagara so I guess this is an issue they've had pushed on them before.

Besides on their actual page:
http://www.niagaracutter.com/news/fall99/

Maritool also has this:
http://www.maritool.com/Cutting-Tool...duct_info.html

So on this I agree to respectfully disagree.
Frankly I just get paid too much to sit around worrying about whether TiAlN is acceptable to anyone.

http://www.emastercam.com/board/inde...howtopic=33219
http://blog.cnccookbook.com/2012/03/...tting-success/ (list item #3)
http://www.practicalmachinist.com/vb...-tialn-121066/ (note the top post and who)
This little game of cat and mouse has after all been played out over and over.

[Cory]

Originally Posted by techhelpbb

Well I am confused then.

Cause I not 7 days ago used a TiAlN 1/8" end mill, 2 flute on aluminum.
With coolant and it was hardly a new end mill for that purpose.
I am not the only one either.

So I guess the question I have is at what operating temperature is this coating appropriate?
Since the question here appears to come down to whether or not it can reach that temperature.


Answering my own concern:
I have a long commute so I decided to call around to Duramill and Niagra.
Spoke with the technical folks not sales.

The reason the coating operating temperature is not specified is apparently because they consider the TiAlN coating inert.
It shouldn't want to bind chemically to aluminum any more than Titanium (no affinity according to Niagra).
The coating provides hardness and durability till the yield temperature well over 1,000 degrees Celsius.
This differs from aluminum titanium nitride which is high in aluminum and therefore is an active coating.

The issue they clarified is that aluminum will of course melt well into the safe operating temperatures of these bits.
So you don't have to hit a certain temperature to make them work.
However just because the bit will withstand these temperatures does not mean the aluminum you are working won't melt and wet the bit.
Obviously once the aluminum melts and wets the bit welding will soon follow.

The reason my machines are not experiencing that issue is because I do not cut aluminum without coolant.
Therefore I am cooling everything.
I do not consider the cooling to be really heavy duty so the bit does get hot.
However the aluminum being worked is basically a heatsink and the coolant cools that.
The gantry mills I have used TiAlN with are pretty rigid. I have seen much worse.
Also I am aware that aluminum tends to melt so I take measures to keep moving.

This is why there is no minimum desirable operating temperature specified.
This is also why it works for me.
I told both companies that I've used these with aluminum and no huge red alarms went off.


However I still agree a slower spindle is desirable for this purpose.
It would eliminate the need for the tool that could be a bit more expensive.
Additionally it would reduce the risk that a slow cut would weld.

If you have a choice you would never use TiN, TiAlN, or AlTiN in Aluminum. If it was all you had, you could use it without immediately destroying your end mill. All the things Scott said are true though, regarding surface finish and BUE. You can definitely notice the latter occurring.

If you tried to run one of those end mills under aluminum specific parameters (1000+ SFM, .003"+ chip load) you will load it up and break it-guaranteed. This is as much because of the geometry being wrong as it is because of the coating, as the only tools that are ever coated with those are meant for ferrous materials.

I'm not sure why they told you that you don't want to run the tool at elevated temperatures. I forget where it is exactly, but somewhere between 700-800C the coating dramatically increases in hardness. As previously mentioned this is why people don't cut ferrous metals with coolant when using those coatings.

[Cory]

Originally Posted by techhelpbb

At this link...
http://www.daycounter.com/Calculator...lculator.phtml

Plug in 0.25", 300SFM, 3 flutes.
You get: about 4,500 RPM, 27.5 IPM
Makes sense that this works.

Plug in 0.25", 1,310SFM, 3 flutes
You get: about 20kRPM, about 120 IPM
This is probably not going to work.
I would be a bit suspicious of a carbide end mill rated at 1,310SFM uncoated.
Even more suspicious if your router can sustain the feed rate to keep it from rubbing.

At a spindle speed of 20kRPM I think you should consider a TiAlN end mill for the router with 2 flutes and 1/8" diameter.
That would get you:
655SFM, 20kRPM spindle speed, 80IPM feed.
If your gantry mill is outfitted with either really powerful steppers or servos it will work.

1300 SFM is perfectly reasonable for uncoated carbide. Most vendors will recommend 700-2000 SFM for a carbide end mill with aluminum specific geometry.

TiAlN, AlTiN, and TiN are always bad for aluminum. They have an affinity for aluminum which leads to galling, causing your end mill to load up and break.

While you are correct that TiAlN and AlTiN are designed to perform best at elevated temperature, you could never even get them to that elevated temperature in aluminum as you would have to run without coolant and you would be guaranteed to melt your chips and pack the flutes long before getting up to temp, completely disregarding the fact that these coatings are not advisable in aluminum due to their physical properties.