[mutski]

Hi all

I'm sorry, I'm sure you answer this question a lot but the search tool just finds soooo much not really relating to my question.

I'm new to CNC routing. I've just got a small 600x400 desktop router. We want to be able to make cutouts in up to 3mm aluminium to mount various switches, buttons, LCD displays etc. I'm really not too sure what kind of bit to use though. I thought carbide was the way to go, so I got some Dremel 9904 bits (tungsten carbide). They seem to work, but the flutes fill up very quickly which means they dont cut very well and I have to stop the machine and clean them out (which is hard).

I'm running the feedrate at 500mm/min, 0.2mm/pass which seems to be what people are suggesting reading the forums here.

What kind of bits should I be looking for?

Cheers - Matt

[-Chris-]

Hi not sure abouy the bit your useing by your discreption but it sounds like your not useing any coolant. it doesent take long before aluminum starts smearing and loading a tool without something to lube things up, spray a little wd or trans fluid on cutter and sheet while cutting. they do make mist systems to keep the cutter cool and lubricated kool mist is one

[mutski]

I have been spraying a lubricant which is similar to WD-40 that claims to be good for cutting. This morning I got a dedicated cutting liquid from Sutton. Maybe I'm not using enough. I'll try using a bit more as it cuts.

Cheers for replying - Matt

[mutski]

I just tried a 8mm diameter hole in 2.5mm thick aluminium with HEAPS of cutting fluid. Didn't seem to make any difference to the amount of aly that's now stuck in the flutes. The Dremel 9904 has about 8 flutes in a 2.4mm bit. I think the flutes are too small for this application.

Matt

[keebler303]

1) Dremel bits are of poor quality to start with. I wouldn't recommend them.
2) It sounds like you are using a burr, not an endmill. It will never work.
3) Buy a good quality 2 or 3 flute carbide endmill and you will never look back.

Possible sources include enco, mcmaster carr, msc, etc.

Good Luck
Matt

[hpowell]

You have too many flutes. As well as floog or mist coolant, aluminum needs as much room as possible to evacuate. I suggest no more than three flutes.
Harry

[hpowell]

That should be "flood or mist"

[mutski]

Thanks for the help everyone. Now that I know what to look for it makes it easier going through catalogues.

I'm going to order some of these:

Solid Carbide End Mills 2 Flute

Is that what I'm after?

Cheer - Matt

[hpowell]

Yep. Get high-helix, sometimes called "Streaker".

[WidgetWorks_Unlimited]

The proper tool depends a lot on your spindle capabilities.

If you're using a wood router that runs at 20,000 RPM then switching to standard end mills meant for metal cutting won't help - most metal cutting is done at much lower RPM.

For the wood routers you'll need a single flute "O-flute" cutter. The flute is polished to reduce chip buildup and the rake and helix angle are specifically designed for aluminum chip evacuation. Buy a tool with the shortest depth of cut that will handle the thickness of your material.

Onsrud makes an .125" cutter .250 DOC for about $30 ea - you can cut aluminum at 20,000 RPM without any coolant.

Also, you need the right alloy of aluminum to cut without flood coolant - 6061 is the most common and works great.

Finally, you need to move the cutter fast enough to make chips. Going too slow will cause major problems.

[CNCMAN172]

As other have said you really need to understand a few aspects of your machine to successfully cut aluminum.

Spindle Speed is critical
Depth of Cut also varies greatly depending on your spindle power
Cutters need to be very sharp and I recommend 2 Flute cutters, however some 3 Flute cutters are design for aluminum.

When your cutters are gumming up this can be caused by several factors. The wrong cutter, too many flutes on the cutter, lack of cutting fluid, depth of cut too deep, feedrate too fast, etc.

There are some very nice Onsrud single flute cutters that can cut that tin aluminum 3mm in a single pass depending on your spindle power like a previous poster mentioned.

I have been very successful using 1/8" carbide 2 flute endmills on my little home built mill. I have to turn my Bosch router down to about 12,000 rpm and set my depth of cut to .025" and my feedrate to 8 ipm. I also recommend a small amount of WD40 and start off with a feedrate of 4 ipm and then start increasing and listening to your machine.

The type of alumium is just as important as all these other elements. Some aluminum just machines terrible. you can go online and review the various types of aluminum and they describe the best types for machining. As another user posted 6061 is very popular and machines very nicely.

Hope this helps. Good Luck
CNCMAN172

[macdarren]

not an expert by any stretch of the word but 500mm/min seems fast to me unless this is a higher end cnc with the proper tooling and cooling.

[VWSatOz]

Look for SPECIAL cutters for aluminium, they need to have highly poished flutes, mirror finish if available, and very open flute design, not much longer though in the weak flutes area than the thickness of metal you are cutting in order to keep as rigid as possible. Sometimes they weld up with alum when plunging into the job, try RAMPING into the cut ie a Z move should have a combined sideways small move in order to allow the swarf IN and the coolant IN and FLOOD coolant or spray mist so the cutting is always WET and libricated. Ally can grades esp. the soft low strength ones can sometimes be soft gummu stuff that starts this welding problem real easy, so sheet may be quite a problem yet some higher grade blocks can be mcd dry.
I used bigger diam HSS cutters and would always have to modify the flute and end back-off to create heaps of spaceand clearance up the flutes on their TIP/ends so the end could plunge in without welding up, yet the main cutter not weakened.
If you can buy those cutters DESIGNED for ally this is easier. Diamond polishing the rubbing surface of carbide cutters also works well if no lube, but this v difficult with your tiny 3m jobbies. Single flute also works, as then you have huge trough for swarf to ride up and can use same feedrate mm/min still or even more than the multiflute! You need to experiment with all those lubes the others mentioned. It is the feed per tooth that you must calculate, say .01mm per tooth for starters and work up from there with each trial, revs can be very high if you have the lube there always, and claculate the CUBIC mm per minute your spindle and power can cope with, then if you have 1/2 the depth of cut you can double the feedrate to keep the same mm3 per minute, same cutter load, same heat, same swarf, same deflection etc & you can really churn out jobs! I HAVE DONE THIS !!! but hose tiny cutters are the hardest to live with if you aint got the high revs! then you MUST feed slow!

[golfnut]

Hi Matt,
Machining aluminium as has been said posses it's problems. The biggest of which is evacuating the flutes of swarfe, You need to use aluminium geometry slot drills or end mills. These have much wider flutes than conventional end mills slot drills. You can cut aluminium without flood coolant but a air blast or vacuum to clear the swarf is advisable.
Spindle speed needs to be high. e.g a 6mm diameter solid carbide 2 flute slot drill can be run at the following speeds and feeds;

RPM = 15,000 to 20,000 rpm

table feed = (depending on spindle power available and surface finish required) 600 mm/min (23.4"/min) to 4000 mm/min (1575"/min). The table feeds equate to 0.02mm/tooth and 0.1mm/tooth.
Depth of cut depends on the application. If full cutter diameter engaged then max depth should 3mm, if profile milling anything from full flute length for say 0.2 mm width of cut, reducing as the width increases.

I hope this helps.

[schbrownie]

Hi Matt,

you may have to do more than just change your bits. Regardless of what type of bit you get, you should be able to find out some information about that bit and how it likes to work. Just about any (requtable) manufacturer will list information like, recommended RPM, feed rate and depth of cut. Use this information to alter your program for the best results.

[JACS1954]

Try a single flute carbide e/m for aluminum . 1/4 dia. stubbie (Then plunge and circle
dia. to size.
They work great (Tin coat if cutting dry)
Jac