[DareBee]

Back on topic.

The lack of spindle RPM aside, you will still cut WAY better with carbide because of the material rigidity. TRUST ME, it is a night and day difference. The rigidity is much more important than the bit of extra sharpness.

Using stub length is also the way to go.

haslagl
Niagara tool makes TiCN coated HSS. I use these a lot when I need larger diameter endmills and don't wish to pay carbide prices. The first time a tried them I was amazed at how much longer than TiN they lasted.
I am sure there are other manufacturers as well but I haven't looked.

[Oldmanandhistoy]

Back on topic.

The lack of spindle RPM aside, you will still cut WAY better with carbide because of the material rigidity.

Just so I am clear here are you saying I should use STC even with my 3000 rpm max?

Can I run STC at lower rpm than recommended without lose of performance and on a hobby type machine?

Or are you assuming the correct spindle speed will be used?

John

[dertsap]

the coated endmills are great on harder materials where the extra lube is needed , on aluminum we use uncoated carbides for the most part and any hss we use are uncoated , aluminum for the most part doesn t wear tools ,
the sharp cutting edge of hss is not always an advatage and can be a great disadvantage a large portion of the time , an unstable sharp hss tool will often dig in causing over cutting and chatter , many times a dull tool will work far better than a sharp one as it will deflect rather than over cut

[DareBee]

Just so I am clear here are you saying I should use STC even with my 3000 rpm max?

Can I run STC at lower rpm than recommended without lose of performance and on a hobby type machine?

John

Yes and Yes.

I used to use HSS for everything in my knee mills (I believe they are 2200RPM max).
We got int a few months of riny-dink tooling that we needed small cutters for. Cutters were always chattering, snapping, gouging and what not. I switched to SC cutters and almost all those things went away (except for extreme conditions). The cutters were/are more or less being used almost the same as an HSS cutter was (this is manual milling remember).
The price of cheap small dia SC (uncoated) cutters is, well, cheap (I don't use this crap in my CNC - just for the manuals). I ONLY buy carbide cutters - no matter what - in diameters 1/4" or less. This saves me money and produces better product.

These are my experiences and opinions.

[Oldmanandhistoy]

Yes and Yes.

I used to use HSS for everything in my knee mills (I believe they are 2200RPM max).
We got int a few months of riny-dink tooling that we needed small cutters for. Cutters were always chattering, snapping, gouging and what not. I switched to SC cutters and almost all those things went away (except for extreme conditions). The cutters were/are more or less being used almost the same as an HSS cutter was (this is manual milling remember).
The price of cheap small dia SC (uncoated) cutters is, well, cheap (I don't use this crap in my CNC - just for the manuals). I ONLY buy carbide cutters - no matter what - in diameters 1/4" or less. This saves me money and produces better product.

These are my experiences and opinions.

Thank you for that I will definitely be giving it a go. So in a lot of cases I will be able to run STC end mills at max RPM (3000 in my case) and just increase the feed speed as much as I can or until I get problems?

John

[dpuch]

Solid carbide works very well with aluminum at any speed, especially for the smaller diamaters due to its stiffness. Also it will hold an edge a lot longer than HSS. If you have a choice, do NOT use TiN or TiAlN coated tools for alunimum, the coatings tend to allow the aluminum to stick to the tool. Bright finish or polished finished tools are great. Use a coolant/lubricant. WD40 is a popular choice for quick cuts, but for normal cutting use air/mist, or a flood coolant. Even plain water will do wonders, but obviously is not the best choice. An air jet will be better than nothing since it removes chips and provides cooling, but no lubrication.

Speeds and feeds vary so much because of the different conditions a cut takes place under. Machine, tool and part rigidity all affect how heavy a cut (deep, wide and fast) you can make. You will have to take some recomended starting numbers and adjust them to how well they turn out on your machine. For internal corners, use the same settings you would use for a full width slot.
Cutter speed is mainly controlled by heat ans tool wear. With carbide tools in alunimum wear usually isn't much of an issue except with cast aluminum and a few less common alloys. So your limiting factor is heat, and this is mainly controlled by your coolant. If an endmill breaks and has material packed around it or melted to it, you need better coolant or to slow down the tool RPM.

Look up some referance numbers, tool manufactures usually have good starting points. Then learn how your setup will do relative to that.

Dale

[Oldmanandhistoy]

Would it be pushing it to say STC end mills are suitable for any metals or is there exceptions to this rule?

John

[Oldmanandhistoy]

Would it be pushing it to say STC end mills are suitable for any metals or is there exceptions to this rule?

John

May have pushed my luck to far thanks for all the help :cheers:

John

[altair]

Just to add my two cents to this thread, I have been making slots in 6061 T6 in the last 2 days with a 1/16 carbide end mill (stubby). The slots are 6" in length and I had to make 240 of them.
The slots are .075 x .075 and I have been able to machine the full depth in one pass. On the return stroke, the slot is widened to .075.
I run the mill at 22000 - 25000 RPM and feed at 8 IPM. I have an air blast shooting right at the back of the end mill through a .032 nozzle, and I supplement with a bit of lubricant (Alum-Tap) in a small accordion bottle with a syringe needle on the end of it. Every second or two, I point the tip of the needle in the path of the air blast, and the venturi effect draws some fluid out of the bottle. Because the needle ID is so small, only a minute amount of lube flows out. I think it took me just one ounce for the whole job.
This could be called Almost-Dry Machining I guess.
Many times, I am able to machine the aluminum dry when the end mill is a bit bigger. I think the trick is in the air blast. It has to be very strong, but at the same time very small to avoid blowing the microscopic swarf all over your work area, and in your clothing... Itchy & Scratchy. Most of the time I smear one drop of lube on the surface of the part just before the bit enters, and this is enough to make a hole 2 or 3 times the dia of the bit, in 1/4 alum.
I always use UN-coated carbide bits for Alu, HSS don't last. Carbide wears too. I changed my bit mid-job because I had to lube more frequently.

I ought to find a way to automatically inject the lube directly into my air line, but I would need a way to meter very small amounts. Maybe with a needle valve... ? Ideas are welcome.

Guy

[dpuch]

Would it be pushing it to say STC end mills are suitable for any metals or is there exceptions to this rule?

John

Pretty much. I am sure there are some exotic materials out there that may be a problem. Also as mentioned before HSS may be a better choice for some plastics. At 3/8 or 1/2" it may be more cost effitive to use HSS for hobby stuff, but the solid carbide still works better.

[eorourke]

I also would use carbide endmills for cutting aluminum. First of all, how much HP does your machine have, what is the taper of the spindle? How far is the tool hanging out? Are you slot milling or just cutting on the side of the endmill(profiling)? I would try a Benchmark endmill. This is a 3 flute em which you can run at 10,000 RPM and a .002" chipload. This is = to 60 IPM at 10,000 RPM. Depth of cut is .060"- .125" axially.

[harryn]

I am still a begginner hobbiest, and almost anyone of this forum knows more than me about machining Al. The one item I did not see in this thread that is really helpful for beginners (like me) is to use an Al alloy that is easy to work with.

An experienced machinist can make most anything work. A home machinist often does not have the personal or spousal patience to obtain this experience. For that reason, it did not take me too long to give up on 6000 series Al, regardless of its wide spread use. For me, it is a pain, as well as soft materials like copper.

My humble suggestion for home beginners is to spend the $s to get 7000 series Al and just stay with it for everything. It can be found scrap sometimes, it machines very nicely, its is hard and strong, can be anodized, etc. For someone that makes limited parts count like me, it is a real joy. On a per pound basis, the cost difference is not significant for the small user. For my hobby uses, 7050 and 7075 in a T6 temper are identical, and so far, always better than 6061 types.

[dpuch]

If you buy material, the main material used is 6061. It is plentiful and a middle of the road performer in most respects. It will machine fine as long as you do not get the tool and material too hot. Using oil like wd40 if it is being sprayed on, or plenty of flood coolant otherwise. I can run a 3/4 EM at 14000RPM 3/4 deep and 0.006" per flute as long as there is coolant ALWAYS on the tool. This is on a commercial horizontal, so no worries about chip removal though.

7075 makes great parts, but is more expensive, less common. harder and more abrasive. Defiantly use carbide with it, and still make sure you have good coolant. Also be aware that it is not an alloy that welds well if at all, I can't remember. I do not know about others in the 7000 series.

I think the biggest problem is people use unknown metals. I think most sign material, sheet for bending and lawn chair tubes (scrap material) are all very soft alloys. 5000 series I think is common. This is so they can bend them without it cracking.

Bottom line, if you have material melting and sticking to your tools you need to slow down the spindle RPM and or provide better coolant.
niagara cutter techinfo

Dale

[DareBee]

Utility grade, formable sheet, aluminum typically used for fabricating is 3000 series (3003).
It is very reasonable and fab shops always have plenty.
If you do not enjoy cutting copper you won't like machining this stuff. OK not nearly as bad as copper but it is soft and gummy. Like copper it cuts best with coolant and taking heavy chiploads.

[davereagan]

High Helix endmills mad efor cutting aluminum are night and day better than standard 30 degree helix endmills. Do you have to use 1/8" instead of 1/4" The price won't be much different and 1/4" can take so much more chipload. Try www.kbctools.com, the top of page 149. Tap Magic EP fluid is great too. Running dry will gall (melt) with much depth of cut.

[fpworks]

Back to his original problem...just wanted to point out a couple of things that caught my eye:

Check the runout of the tool! (don't accept more than 0.0003" on a 1/8" tool) Runout increases the loading on one side of your tool. Since you said no aluminum was melted around the tip of your tool, my money is that your problem is here. This is a big deal with smaller tools, especially with more aggressive cutting parameters.

Run either a two or three flute tool. Throw away the concept of "chip load" for determining your feedrate in aluminum, and think feed per revolution. Chip evacuation is the big deal in aluminum. You can feed a 2 flute tool harder than a 3 flute tool. Relatively speaking, a 4 flute endmill is nearly worthless in aluminum.

Do everything right, and you should be running at 0.004 IPR (Inches Per Revolution) at 0.1" depth and full diameter cut with an 0.125 endmill.

[ewest]

I'm using HSS tin coated. Also, what do you mean by too much backlash? How much is too much?

Wade

TiN coating SUCKS in aluminum. Don't use it. It sticks. Also, crank your spindle speed up as much as possible, and keep a squirt bottle of WD40 or synthetic cooling. I use this stuff called "Premiere 600" mixed with water, and it works great too. With it, I prefer to use High Speed Steel tooling. It seems that the HSS starts with a sharper edge than carbide (but of course it wears)

and check runout, as mentioned before.

You have a dial indicator, right? If not, get one, and if you can't afford a good one, at least get a piece of Chinese crap. Unless you've checked, you might have a completely shot spindle or bad tool holder, or garbage and chips packed up in to the taper on the spindle. I was shocked when I tested our CNC here at the shop. There was about .001 of runout in the spindle taper, and the tool holders, which are supposedly a good brand, had about .005 or more of runout!!! Jesus! Anyway, the bearings in the spindle are shot, new ones are on order, and I just don't know about these tool holders. The moral of the story: Maybe it's not you. Check the machine for problems.

How's your fixturing? Are you using double stick tape or a good clamping?

Also, are you using a 2" long mill when you could actually use one that's 1/4 inch long?

[wwendorf]

TiN coating SUCKS in aluminum. Don't use it. It sticks. Also, crank your spindle speed up as much as possible, and keep a squirt bottle of WD40 or synthetic cooling. I use this stuff called "Premiere 600" mixed with water, and it works great too. With it, I prefer to use High Speed Steel tooling. It seems that the HSS starts with a sharper edge than carbide (but of course it wears)

and check runout, as mentioned before.

You have a dial indicator, right? If not, get one, and if you can't afford a good one, at least get a piece of Chinese crap. Unless you've checked, you might have a completely shot spindle or bad tool holder, or garbage and chips packed up in to the taper on the spindle. I was shocked when I tested our CNC here at the shop. There was about .001 of runout in the spindle taper, and the tool holders, which are supposedly a good brand, had about .005 or more of runout!!! Jesus! Anyway, the bearings in the spindle are shot, new ones are on order, and I just don't know about these tool holders. The moral of the story: Maybe it's not you. Check the machine for problems.

How's your fixturing? Are you using double stick tape or a good clamping?

Also, are you using a 2" long mill when you could actually use one that's 1/4 inch long?

Well, I guess i'll revive this thread a bit. I finally got a FogBuster 2 nozzle coolant system and it seems to be making my life much easier. I recently did some cuts with a 9/16 endmill, making 1/10" deep cuts in aluminum at 6ipm. I was able to crank it up to 9ipm, but I felt a little more comfortable at 6ipm. I was also spinning at 3400 RPMs. Boy, did the chips fly!

I still have to get back to using an 1/8" endmill. I'm going to use a rule that i hear from a friend o mine, cut only as deep as 1/3 the diameter of your endmill. So far, it's been working for me. I'm going to purchase some HSS TIN and nonTIN coated endmills and figure out which one give me better results. So far i've been pretty happy with the TIN coated stuff.

I'm currently waiting on an order I placed for a shower pole that will wind up holding a heavy clear vinyl shower curtain in my shop. The chips flying everywhere are getting totally out of hand and totally into my woodworking tools. I wish I had room for an enclosure, but that is out for now. The vinyl curtain should keep the chips in the vicinity of my mill to make cleanup a bit easier at least.

Thanks for everyones tips and information.

I really appreciate all the posts and the information is invaluable to me.

When I get some time to play with a 1/8" endmill again, I'll post here and let you know what I find. Oh, btw, I did purchase some carbide endmills, so we'll see how those work.

Thanks,
Wade