Machsupport Forum

Mach Discussion => General Mach Discussion => Topic started by: Katoh on April 21, 2010, 11:15:21 AM

Title: Aluminium Cutting
Post by: Katoh on April 21, 2010, 11:15:21 AM
Good Evening to All
Its been quite a while since my last post, just goes to show when you build a good Mach machine nothing really goes wrong, True to a point, since last time I posted anywhere, I have added a 4th axis to the big router, and actually worked out how to use it, still trying to learn how to alter a 3d file but that is a different matter entirely.
Ok enough rambling from me, My next project is to make a 23' Aluminium boat, the panels I am hoping to cut using my CNC router, I can already hear shrieks out there, apparently it can be done. The thickest material will be 6mm and the rest will be 4 and 3.
The machine has a 5HP Fimec motor speed range from 7 to 14.700 rpm and cuts max speed 3000mm/min comfortable, can go a lot faster but scary at high speeds! I don't want to use mist lube on the cutter I have made up a concentrated compressed air fitting to blow onto the cutter, but I don't want oil going all round the joint.
I will probably use either a 3mm or 6mm cutter cut down, smaller the better.
Now the Crunch, What I would like to know What is be best cutter to use? speed/feed rate? rpm? and cut depth?
Has anyone got experience?
Cheers Katoh
Title: Re: Aluminium Cutting
Post by: Hood on April 21, 2010, 11:27:12 AM
I cut lots of 5083 and wouldnt dream of doing it without flood, you may be lucky and get away with air only but.... well  I have never had much luck. Then again I only have 4000rpm spindle on the mill so maybe getting the spindle speed and the feed cranked up will help. Get a cutter specifically designed for Alu and you may stand more of a chance.
Why do you not want oil on he cut?

Hood
Title: Re: Aluminium Cutting
Post by: Katoh on April 21, 2010, 11:39:10 AM
Hi Hood
You probably don't remember my Machine but its a great big flat bed router, know with a 4 axis down one end, the work sits on a timber base and its all contained with timber surrounds. Ok I chop up a plate with mist, mist floats around soaks into the timber, next time I use the router to shape a $1000 stick of walnut for someone oil starts leaching into the job from the base and destroys the job, I see this get upset, grab a gun and shoot the router. This is a very dramatic recreation of what could happen, but I really prefer not to go down that path if you know what I mean.
Katoh
Title: Re: Aluminium Cutting
Post by: Hood on April 21, 2010, 04:16:30 PM
Ha ha OK I see now why you dont want oil and coolant there ;D
Suppose you are just going to have to try and see how you get on but as said I would definitely go with a cutter specifically designed for Alu, they are usually sharper and have a high helix and can be fed fast if you have the spindle speed, and you do :)
Hood
Title: Re: Aluminium Cutting
Post by: ger21 on April 21, 2010, 04:40:33 PM
You can get router bits for cutting aluminum dry from www.onsrud.com. They won't be cheap, though.
Title: Re: Aluminium Cutting
Post by: Katoh on April 21, 2010, 07:37:18 PM
Thanks Hood and Gerry
I will look at the onsrud site maybe also cmt might have something, but it would be nice to talk to someone how actual does it with the same sort of machine, little tips and tricks are at times invaluable.
Katoh
Title: Re: Aluminium Cutting
Post by: ger21 on April 21, 2010, 09:01:39 PM
RPM and feedrate will be critical. Onsrud should be able to steer you in the right direction.
Title: Re: Aluminium Cutting
Post by: HimyKabibble on April 21, 2010, 09:27:20 PM
Good Evening to All
Its been quite a while since my last post, just goes to show when you build a good Mach machine nothing really goes wrong, True to a point, since last time I posted anywhere, I have added a 4th axis to the big router, and actually worked out how to use it, still trying to learn how to alter a 3d file but that is a different matter entirely.
Ok enough rambling from me, My next project is to make a 23' Aluminium boat, the panels I am hoping to cut using my CNC router, I can already hear shrieks out there, apparently it can be done. The thickest material will be 6mm and the rest will be 4 and 3.
The machine has a 5HP Fimec motor speed range from 7 to 14.700 rpm and cuts max speed 3000mm/min comfortable, can go a lot faster but scary at high speeds! I don't want to use mist lube on the cutter I have made up a concentrated compressed air fitting to blow onto the cutter, but I don't want oil going all round the joint.
I will probably use either a 3mm or 6mm cutter cut down, smaller the better.
Now the Crunch, What I would like to know What is be best cutter to use? speed/feed rate? rpm? and cut depth?
Has anyone got experience?
Cheers Katoh

I don't see any reason you shouldn't be able to do what you suggest.  I'd probably use a carbide endmill rather than a router bit.  I do my aluminum roughing using a 1/2" carbide 3-flute endmill, 0.125" DOC (~3mm), 6000 RPM, 75 IPM.  It'll do that all day long with just a strong blast of air to keep the chips clear.  In general, with aluminum, if your feed is too slow, you'll find the tool heats up, and chips weld to the tool.  The natural reaction when you see a hot tool, and chip welding, is to slow down, but that's exactly the wrong thing to do.  You want to maintain the heaviest chipload you can get away with (which is a function of your machines stiffness and spindle power), as a thick chip will carry heat away from the tool.  If the machine stiffness prevents running the desired chipload, reduce RPM, reduce feedrate accordingly, and try again.

Regards,
Ray L.

Regards,
Ray L.
Title: Re: Aluminium Cutting
Post by: elpablito on April 21, 2010, 09:35:49 PM
Using onsrud or amana carbide single O flute 1/4" diameter you can cut at 15000 rpm and 0.003 to 0.006 per tooth (45 to 90IPM) full diameter (eventhough i never cutted more than 3mm aluminum in a single pass)
I use a cool air gun and lub myst.
Title: Re: Aluminium Cutting
Post by: Katoh on April 22, 2010, 01:07:24 AM
Gentlemen
Thank you ever so much for the advice, I will buy a couple on the O flute bits in sizes from 3-6 mm and at least know iI have a starting point, run the router at around 75ipm and speed around 13-14k rpm used air jet on the cutter and play around with a scrap piece of 6mm plate till I tweak it just right. Then start cutting out this boat, Cant Wait!
Thanks Again
 Katoh
Title: Re: Aluminium Cutting
Post by: simpson36 on April 23, 2010, 12:19:41 PM
You can get router bits for cutting aluminum dry from www.onsrud.com. They won't be cheap, though.

I'll second this. These bits can run at 'ludicrous speed' and the geometry won't try to pick up the sheet like a typical spiral end mill will. I'm pretty sure they come in down cut as well, which would help keep the sheet from singing you a tune.

I have had some success using a stick form of 'grinders paste' and a new one that I like is made by Boeing (yes, the jet company). In practice often I will trace out the path with a pen in the mill first, then go back and smear the stick lube on the cut line sort of like it was a crayon. Your compressed air stream will keep the tool cooled down (very important) but won't pick up the waxy stick lube. The lube does a very good job keeping the cutter surface 'slick' so it won't collect aluminum, and does not saturate everything around it like liquid coolant.
Title: Re: Aluminium Cutting
Post by: Katoh on April 23, 2010, 08:34:21 PM
Hi Simpson36
That lube sounds like real good stuff, do you have a proper name for it or a link to were you buy it from. Just out of interest sake what size cutters are you using and how much depth per cut are you takeing per pass?
I tried to cut some alloy a while ago with a 2 flute 6mm bit apparently made for alloy cutting, I run the router at 7krpm 1500mm/min add with a  cut depth of 1mm/pass on 10mm plate, The first and second pass were fine until the cutter pulled itself out of collect and cut 10mm in one pass, funny thing the motor didn't loose a rev the cnc started loosing steps in X and Y , Probably from the tool load but didn't stall in movement or break the cutter. So I decided back then that cut down cutters are the only way to go!
From those with experience how noisy is it? or how noisy is it meant to be? When I tried it back then it was a like high pitch squealing and screeching. I don't think that's right.
Cheers
Katoh
Title: Re: Aluminium Cutting
Post by: elpablito on April 23, 2010, 08:44:56 PM
In my experience it is quite noisy because the aluminum sheet vibrates close to the bit. Anyway you can get an acceptable finish in one pass, or if you want to make it better you can leave 0.2mm for a finish pass
Title: Re: Aluminium Cutting
Post by: Katoh on April 23, 2010, 08:53:59 PM
I don't really need a great finish because all the cuts are going to be welded up against another part or hidden.
To cut a 6mm plate in one pass, I thought would be to excessive for the cutter and machine. On timber I use the rule of thumb 1/2 x cutter dia = max cut depth. I thought alloy would be even less.
Katoh
Title: Re: Aluminium Cutting
Post by: elpablito on April 23, 2010, 09:04:56 PM
This tools are supposed to cut one diameter whithout problems but with aluminum i wouldnt try, specially if is not good quality.
Onsrud has some nice chipload tables online and at the back of their catalog. If i remember well, they give the values for 1xD and then they say that for 2xD decrease 25% feed and 3xD decrease 50%, but it is not clear for me wether thay reffer to full slotting.
Always try to keep the recommended chipload and SFM. If you dont feel confortable feeding too fast, lower feed but also lower rpm to mantain chip load and SFM. Otherwise you will generate too much heat.



Title: Re: Aluminium Cutting
Post by: Katoh on April 23, 2010, 09:29:11 PM
Thanks for that, that's basically what I was thinking, I was thinking to use a 6mm cutter and do it 3 pass on 6mm plate, or I don't know if I'm pushing my luck too much now, is to use a 1/8" cutter in do it in 4 passes that's about 1.5mm per pass, I really need to sit down with some scrap and try a few different things.
Title: Re: Aluminium Cutting
Post by: ger21 on April 24, 2010, 07:55:27 AM
Quote
From those with experience how noisy is it? or how noisy is it meant to be? When I tried it back then it was a like high pitch squealing and screeching.

A larger tool will probably be quieter. When cutting hardwood , a 1/4" bit will literally scream, where a 3/8" bit will be nearly silent.

Quote
On timber I use the rule of thumb 1/2 x cutter dia = max cut depth


If you're machine is up to it, you should be able to cut 1-1.5x dia. Yesterday I was cutting walnut 3/4" deep with a 3/8" cutter, at 400ipm. With harder wood, like maple, I decreased the depth to 3/8".


I found a post on another forum from someone who cuts 1/8" 6061-t6 aluminum all the time. Uses an Onsrud 63-622. Cutting dry. .03125"/pass (.8mm), 85ipm and 19000rpm.
Title: Re: Aluminium Cutting
Post by: simpson36 on April 24, 2010, 08:37:53 AM
You are always going to be better off cutting all the way thru the material in one pass if you can, even if you need to use a slightly larger cutter. Likely marine grades of aluminum are called for here and those cut fairly clean. If I remeber correctly, the machine in question has enough power to make the 6mm cut.

The biggest issue in cutting aluminum in multiple dry passes is keeping the slot clear of chips, and heat generated at the bottom of the slot. Re-cutting chips also makes heat and lots of vibration, and the cutter rubbing on the sides of the slot make a lot of heat that cannot be carried away in the chip. A thru cut automatically clears the chips, runs cooler and smoother. In my experience, the clogging of multi flute cutters always starts at the bottom of a slot where the heat is highest. That's one reason a single point 'router' type bit is best to use as it only has a single contact point with the bottom of the slot. You can modify a normal cutter to resemble this profile by grinding the end to a concave shape, but better to spend the bucks and buy the excellent cutters produced specifically for this type of operation.

I'll just throw in a Simpson tip-of-the-week here for those who have 'tried everything' and still cannot get a multi pass cut to work for them. If you are having a bad time with a particular material, you can try offsetting each successive pass by say .003" to the climb milling side of the cut. The result is faily dramatic. There is a rather complicated explanation for this that I won't go into here, but I toss it out there as an option for those who are inclined to experiment. 

Title: Re: Aluminium Cutting
Post by: Katoh on April 24, 2010, 10:28:01 AM
Gentlemen
 I'm starting to get a bit confused now. I cant see my cnc cutting a 6mm sheet of marine Alloy 5086 with a 6mm cutter in pass, I can only see a lot of stress on the machine, a huge tool load, and a good possibility of loosing steps. and or damage to the cutter, spindle or even the CNC mechanics. My very good friend with his Huge Bridgeport CNC mill will only take passes to 1/2 the dia of the cutter, and he does this for a living.
Gerry even you wrote about the other thread the guy who cuts 1/8 sheet in nearly 1mm passes, and Yes I can see the advantage of offsetting each pass, but It just sounds like a lot of material to be removed in one pass.
I don't really know, or maybe I'm just a bit of a SOOK when it comes to my machinery but I don't like when I here them struggling, and when it happens you can hear them, I'm sure no good can come from it.
I know my Machine and with a 3/8" cutter at 120"/min  with 5mm passes its very happy in melamine and most timbers, I once had the problem were my final finishing pass ended up before my cutting passes and it cut 3/4"  MDF in one pass, the result was not pretty, it did not loose steps but hold downs failed due to the tool load and 2 ton of cnc bolted to a concrete slab started to shake and vibrated, pretty scary stuff.
The day when the cutter pulled out and it was cutting 10mm thick plate with a 6mm cutter in one pass, was definitely bad enough, now that's only 1.7 times cutter dia. I cant see this as being a good thing.
Katoh
Title: Re: Aluminium Cutting
Post by: ger21 on April 24, 2010, 12:47:59 PM
With a 5HP spindle, you definitely have enough spindle power to make those cuts in a single pass. Sounds like the issue you have is machine rigidity, and possibly lack of stepper power.

I've been running $100K+ routers for the last 10 years, so I have a little experience. Sometimes cutting deeper and faster will make much less noise than shallower and slower. Also, how well the part is held down has a large influence on noise generated. I used to use a router with vacuum pods. When cutting near the pods, the sound volume could be as much as 5 times lower than when cutting in unsupported areas. At my new job, with a 5x12 vacuum table with two 40HP pumps, cut's are much quieter. I can cut 3/4" MDF in a single pass, with a 3/8" bit, at 700ipm. If the bit is sharp, it won't make hardly any noise at all.

Get a good 3/8" compression cutter and you should have no trouble cutting 3/4" melamine in a single pass at 500ipm, if your machine is up to it. Your spindle certainly should be.
Title: Re: Aluminium Cutting
Post by: simpson36 on April 25, 2010, 05:52:05 AM
Katoh;

The solution to your dilemma is found in this old Vaudeville yarn;

Patient:  "Doc, it hurts when I do this!"

    Doc:  "Then don't do that!"


Title: Re: Aluminium Cutting
Post by: Katoh on April 25, 2010, 09:44:23 AM
Gerry sorry I did not  mean to offend if I did, you have clearly much more experience than I and access to much better machinery than what I have, more than likely a better range of cutters as well. I just know the capability with my machines and how far I can push them until it all turns pear shaped.
This is why we ask the question in the first place.
simpson36 your dead right, I wont be doing that because it does hurt, but at least all of you have given me a starting point and some really good ideas to get this alloy cut. By the way you still have not told us what the name of that cutting paste is and were to get it from?
Katoh
Title: Re: Aluminium Cutting
Post by: ger21 on April 25, 2010, 11:17:51 AM
No offense taken. Just pointing out what your spindle should be capable of. But the rest of the machine has to be up to the task as well. Good luck. :)
Title: Re: Aluminium Cutting
Post by: Katoh on June 12, 2010, 10:01:57 PM
Fellow CNC,ers
To those that have followed this thread or read the thread asking the same questions as I have, I have had time to do the following tests and have come up with what works on my machine.
Yes a single flute carbide cutter is the only way to go, just a little compressed air blowing onto the cutter is fine and will clear the chips. Now here is the crunch time, all depending on the rigidity of your machine will determine what size cutters you can use without to much trouble, my machine is quite rigid but its cutting surface is 300mm lower than cutter at full Z when the cutter is this low it does have some movement which cause problem's.
Ok I found for my machine a 1/8" single flute carbide cutter run at 12500RPM cutting 500mm/min at 1mm/per pass will give you an exception edge with no chatter and is extremely quite. This was tested on some 10mm plate and the results were very pleasing indeed. Larger cutters do not work so well in my machine due to the increase in tool load.
If your machine has a smaller z than mine and can keep the cutter up on the gantry were it can have  more support less flex in components you will probably have better luck than me with larger dia. cutters.
Again thanks to all
Cheers
katoh
Title: Re: Aluminium Cutting
Post by: BluePinnacle on June 15, 2010, 11:03:58 AM
I was thinking in terms of a high helix, solid carbide milling cutter. They leave a lovely finish on aluminium.