Cutting aluminum sheets

[iflyamphib@aol.com]

THREAD FROM ARCHIVE
================================================== =
Cutting aluminum sheet

From: Jim Ratte 13 Dec 1998

Interested in using ShopBot to cut flat aluminum sheet up to .25 thickness. Anyone used the machines for this yet?

Also, being a fairly new computer user for about a year, just getting comfortable with windows based software. I understand ShopBot uses DOS to actually run the program for the machine. Any way to use a windows program for this, or use an entirely different program to run the machine itself?

Thanks for your patience with a cnc newbie! Please email responses to iflyamphib@aol.com (mailto:iflyamphib@aol.com)
Jim Ratte Recreational Mobility www.recreationalmobility.com


From: Steve Fillipp 14 Dec 1998

Hi, Jim.
We've cut aluminum a few times with our 'Bot, using a standard router. I like to use three or so passes to cut all the way through 1/4" material, and have gotten acceptable results - obviously not as good as with big-time machine tools, but o.k. if you're cutting all the way through.

It's pretty hard on the cutter, mainly because of the excessive spindle speed. We use titanium nitride coated carbide 1/4" end mills, and lube the heck out of the metal. WD-40 works well, just keep things nice and wet, and pay attention. One of the guys at ShopBot told me that someone he knows uses dishwashing liquid. Sounds promising but I haven't tried it.

I don't remember specific feed rates, just start slow and work from there. You'll get a feel for it pretty quickly. Regards, Steve Fillipp


From: Brian Taylor 14 Dec 1998

ShopBot must use DOS - do NOT use any flavour of windows as this is a pseudo multi-tasking system and does not give full time control of the machine. You will see jerky motion as Windows goes off into the weeds to check for email, scanners, plug-n-play components, games, etc. DOS devotes full time to the job at hand.

We all typically use Windows for the CAD parts design then make a disk of the parts file which we run on a separate old DOS machine dedicated to just driving the ShopBot. With the low price of surplus DOS machines this is no burden.

Re Aluminium - ShopBot is a tool that will move any cutter over the sheet. Although most of us use routers and cut wood, you can cut metals, glass or stone with appropriate tools AND mist or liquid coolant. The high speed routers on most ShopBots are NOT suitable for metal - way too fast and no coolant.

Metal parts often require a higher precision than ShopBot delivers and this might also be a problem - it all depends on your application.

[phil]

Re cutting aluminum
Spindle RPM for any material cutting depends on several factors. Material, feed speed, cutter material, cutter type, # of flutes, coolant etc..
For aluminum cutting I use carbide spiral bits used in milling machines. For rpm I use a normal Porter cable router but I use a variac as the power source. A variac is an adjustable variable AC power source. It's basically a transformer that can be varied from 0 to 140% of the incoming line voltage just like a volume control on a radio. The one I use is rated at 15 amps and costs about $100. You can buy variacs from places that sell electronic test equipment or other electronic parts. A variac is the best variable ac source to use as it supplies a true sine wave to the router as oppossed to the lamp dimmer type circuits that actually modify the wave shape of the ac signal which could affect the router.
For aluminum you need slow RPM's. How slow? Hard to say. Aluminum comes in different grades and again the bit etc.. are other factors to consider. Basically you need enough RPM's to cut the material with a good quality cut without burning up the bit and allowing chip removal of the material at a rate consistent with the results you want. I have used from 500 to 3000 RPM.

COOLING is a must on aluminum milling! I use a spray bottle filled with a 5 to 1 mixture of water and liquid soap. I first flood the sheet of aluminum with the spray and then keep a spray at the point of contact with the material and bit during cutting. I have cut 1/2" thick aluminum this way. It takes a long time and not really worth to do on a production basis but OK for a few odd parts. I usally use a depth of about .050 per pass for big bits and deeper for smaller bits. But you should never cut deeper than the 1 or 1.5 times the diameter of the bit to avoid breaking or flexing of the bit. Trial and error will soon lead you to the most desirable combination for your situation.
A habit I started to get into is to establish a cheat sheet of material, bit ype, depth of cut, rpm used, feed speed. Once I have a job running pretty good I record the information on the sheet. I also keep a record of what combinations didn't work well. This way you can zero in on best combination of setting the nest you run the same or similar job.
To avoid a mess on your table from the coolant spray, I first tape a sheet of plastic film over the whole table (over my sheet of aluminum too.)
I then use a knife to cut an opening over the area where the aluminum will be cut. Using masking tape and 1" wide strips of plastic or laminate I build a dam around the area that will be cut to contain the coolant and chips etc.. When I'm done cutting, i soak up most of the liquid with rags and then roll up the sheet of plastic film and discard it easily.

The other problem is that the shopbot frame (struts) are really not strong enough to cut aluminum as you will get a lot of vibration and the y axis will flex upward somewhat and the bit will want to ride the aluminum rather than cutting it. But with a SLOW feed speed, proper bit, coolant, and the correct RPM as determined by trial and error you can cut aluminum on the shopbot. If you have a lot of cutting to do you will find very frustrating but for a few small pieces it is worthwhile.

[phil]

Re cutting aluminum

Found a good reference site on web that has an excellent detailed instruction on cutting aluminum and other non ferrous metals.

Go to the following site:

http://www.axyz.com/

scroll down to an area called general and there you can click on "cutting non-ferrous metals."

Good luck and happy botting!

[carol]

I went back and read the past messages concerning milling aluminum on the Shopbot. Then I tried cutting aluminum. Oh, boy!
I want to cut a 12" long 1/4" wide slot through 3/16" #6061 aluminum. I have tried using a 2 flute up-spiral end mill 1/4" in diameter. Machine is the 96" rack & pinion model. Router is 3 HP set to 10,000 RPM. Feed rate was at 1.00. Ramp at .65. Plunge was down to .015 a pass. Problem is breaking bits when about to make the through pass. Another problem is the aluminum slag adheres (read 'welds') itself to the carbide bit. 24 passes to get through. Builds too much heat. Also, I have been running the slot along the Y axis. Is the X axis stronger? And I thought the Shopbot guys said I could do this without misting.

Now that I've told you all the wrong things I have done. Tell me what I should do.

Thanks.

[bruce_clark]

Carol:

Here is just a couple of thoughts (that doesn't
make them right).

First, I personally think that the SB is not rigid
enough for solid carbide cutters (even my mill is
not rigid enough for carbide!).

Now, your feeds and speeds look dead on from a
textbook standpoint. My questions is this: Does
the AL vibrate a lot while cutting? Does the
machine vibrate a lot? Either may be flexing so
much that the cutter is getting an uneven chip
load and that may be contributing to your cutter
breakage.

Another posibility is that the cutting is not
clearing the chips very well. Are most of the
chips cleared out of the slot between passes? I
have found that on a mill the biggest cause of
breakage of cutters, for me, was recutting chips.

If you want to stay away from oil/water coolant,
have you considered using an air gun or something
similar to help keep the AL cool and clear the
chips out of the slot?

Lastly, what type of cutter are you using? Brand,
cut, lead ect. If you can slow your router down a
little more, you might be better served by using a
high speed steel cutter. They are more forgiving
than carbide (and they are cheaper) with variable
chips loads and they usually leave a better finish
than carbide. The downside is you will probably
HAVE to use some kind of coolant.

Bruce Clark
bwclark@centurytel.net (mailto:bwclark@centurytel.net)

[joa]

I just cut out a nice aircraft panel... here's my advice... slow the router down as far as you can get it and slow your feed down to about .1 or less. Do the slot in two passes. Use a thick (but not too thick) mixture of dish soap and water in a spray bottle. You want it just thick enough to not run all over but not so thick that it globs up and holds the chips.

Hope this helps:)

[flyboy]

I know this is an old posting so it's for archive purposes more than anything. I've been cutting aluminum and have found the following settings to work for me. 1/8'' aluminum - not sure hardness... .05" depth of cut each pass, feed rate of .02 IPS . Also I have a speed control from harbor freght and have it turned down all the way. really slow I know but corresponds to the speed I use with my Maxnc mill which doesn't have coolant either. I will try faster speeds next but that's just what is working and not melting back in or causing chatter for me. It takes a while but I'm not a commercial user so it's ok for my airplane instrument panel and small parts

[davidallen]

cheap cooler
for a low cost 'mister', check out:
http://mistymate.com/mmp16.html
it uses a hand pump to pressurize a water container and has a very fine misting nozzle that can be located near the router bit. you might be able to use a soap solution to help with flow on the metal. I wouldn't recommend anything volatile since a flammable mist near an arcing router might cause problems.

I've use one in front of a fan to cool the shop on low humidity days. a full bottle will last about 90 min. with intermittent pumping.

[noah@noahsart.co.nz]

Hello all. I just got an enquiry for 15mm thick aluminium letters. Should I just tell them to get lasered? Anyone cut anything that thick and the Bot lived to tell the tale?

[didde@lowcountry.com]

A 500 watt yag laser might cut it,but a someone with a plasma shopbot, might be able to cut it too. I havea new 30 watt co2 laser and its hard to cut anything over 1/8" and thats wood.

[gerald_d]

See this recent aluminium job. (http://www.talkshopbot.com/forum/messages/2/1617.html?1054887945)

[fitz943]

We cut .5" aluminum all the time. We use a Belin .25" bit @.75" per sec. I think I run the router 16,000rpm or whatever the middle setting is on the porter cable. The depth of cut is .125" and we do a clean pass @.02". With mist, it does great. I cut between 12-18 hours on one bit last week.

[noah@noahsart.co.nz]

Thanks for your suggestions.
1. I do not have a mister
2. Tom that makes 50 passes for a half inch if my non-metric maths are correct. So approx. 70 passes for 15mm. That makes about a day standing there with a garden spray and earmuffs, babysitting the thing. I will pass on this one until I have more gear and experience, and one day get a plasma or laser.
Gerald I saw that job and was very impressed.

[gerald_d]

Simon, I'll try and translate Tom's post to southern hemisphere units and language
:

.. cut 12mm aluminum all the time. We use a Belin 6mm bit 18mm per sec. I think I run the router 16,000rpm or whatever the middle setting is on the porter cable. The depth of cut is 3mm and we do a clean pass (a trim off the edge at full depth) at 0.5mm (ie. a smaller tool offset)

It looks like only 5 passes in total.

[noah@noahsart.co.nz]

Gerald, Thats Lekker! But too late, I have let the job go. Fortunately there is currently plenty other work about to keep me occupied. However, cutting 3mm of aluminium in one pass is a lot for my setup - I am currently using a Benchtop with a hand-held deWalt 1.4KW router jubilee-clipped on. In 3 weeks my PRT96 will arrive, complete with PC router. I have a really heavy steel table built already, waiting for the shopbot. No longer will I have to get those 2440 by 1220(!) sheets cut into strange sizes before commencing work.

[fitz943]

Gerald, Thanks for the translation. I deal with a few Brits here in Virginia and we confuse each other all the time when we talk about sizes. You were right about the 5 passes. Thanks again.

[dsain66@aol.com]

I know this isn't quite related to the SB, but using Belin bits with an MultiCam MG routing table running at 18000 rpm we successfully cut in 1/8" passes at about 50 inches per minute. Using a mister that puts a very fine spray of vegetable oil down where the cutter meets the material. The Belin bits seem to be superior, but a bit costly...

[gerald_d]

Hi DSain

What diameter bit would that be? (It is all related, and we like hearing from the guys who run real CNC machines
)

[Vic Router (Unregistered Guest)]

I cut alum on my AXYZ machine with similar settings and feeds and speeds. Please note
that best results are obtained when "climb cutting" non ferous ie brass , alum and copper.
That is cutting in a counter clock wise direction.

[Vic Router (Unregistered Guest)]

Gerald , you can use 1/8"Belin up to 1/4"