HobbyKing.com New Products Flash Sale
Reply
Thread Tools
Old Nov 19, 2012, 10:39 PM
Registered User
United States, CA, Santa Monica
Joined Jul 2011
493 Posts
Help!
Cannot cut aluminum for my life

Hey all, I've had really good tips on this forum from some really experienced machinists. Hopefully, you gurus can help me out again! I've been trying to cut 1/8 in aluminum sheets for quadcopter arms with a 1/8 in 2 flute end mill on my Zenbot CNC. However, The bits just keep on breaking. I'm taking cuts at 0.04'' depth, feeds at 20 ipm, and rpm at around 20k. This produced a nice cut at first but after about 2 minutes of polishing, broke. So I used the G-wizard calculator thinking I would get a good idea where to start- the numbers came out to be about 16k rpm at 30 ipm. I tried that and the end mill had a really bad chatter before any cuts were even made and just snapped. My router maxes out at 24k RPM, so I've ordered some 3 flute end mills. What would you guys suggests for feeds/rpm/depth of cut on a Zenbot machine?

Thanks
Lpbug is offline Find More Posts by Lpbug
Reply With Quote
Sign up now
to remove ads between posts
Old Nov 19, 2012, 10:43 PM
Registered User
United States, CA, Santa Monica
Joined Jul 2011
493 Posts
Forgot to mention the type of Aluminum, which is 6061-T6.
Lpbug is offline Find More Posts by Lpbug
Reply With Quote
Old Nov 19, 2012, 11:16 PM
Registered User
Ward Hagaman's Avatar
San Diego
Joined Mar 2003
2,293 Posts
Are you using anything to cool/lubricate your cutter? You can look at the broken cutter and see if chips might be welded to it. Can you use some WD-40 and a spray bottle?
Ward Hagaman is offline Find More Posts by Ward Hagaman
Reply With Quote
Old Nov 19, 2012, 11:47 PM
Registered User
United States, CA, Santa Monica
Joined Jul 2011
493 Posts
Quote:
Originally Posted by Ward Hagaman View Post
Are you using anything to cool/lubricate your cutter? You can look at the broken cutter and see if chips might be welded to it. Can you use some WD-40 and a spray bottle?
I am trying to get a hold on some tap magic as I read WD-40 is flammable, no chips were welded to the broken cutter. I bought myself a pump just to have chip clearing/cooling, but as of now I don't have any lubrication. I've seen many people cutting 6061 dry so was assuming I would be able to as well, but I guess it's trickier than it looks!
Lpbug is offline Find More Posts by Lpbug
Reply With Quote
Old Nov 20, 2012, 04:48 AM
Registered User
Denver, CO
Joined Dec 2005
6,259 Posts
Depth depends on how rigid the setup is.
This is how I figure it. I lookup the SFM, and chipload for 6061 t6. It varies by end mill design, so best if from the endmills manufacture. If not a few general specs can be found. I see 400 to 800 SFM for carbide endmills is common, 800 to 2000 for some more rigid cutters. A 2 flute is not that rigid, same goes for the router. So I would go towards the low end of 600 SFM. The chipload is 0.001 inch, for the 0.125 inch mill. For other sizes in 6061-T6 I look up in a chart, or use this formula, 0.008 to .01 inch x the tool diameter.
Now the math.
Chipload = 0.008 x .125 = .001

RPM = (SFM x 3.82) / tool diameter
So RPM = (600 x 3.82) / .125
So RPM = 18336

Now the feed rate
RPM x chipload x number of flutes = feedrate
So 18336 x 0.001 x 2 = 36.7 ipm
This is a general formula that does not take into account many other factors, but is fairly good for most things. The formulas can be turned around to work backwards, incase the router rpm needs to be at something different due to things, like lacking torque at lower rpm.
I always have better results with lubrication. WD-40 is very good. I normally use lubrications made for millling, in my homemade fog buster mister.
Roto Rob is online now Find More Posts by Roto Rob
Last edited by Roto Rob; Nov 20, 2012 at 02:46 PM.
Reply With Quote
Old Nov 20, 2012, 09:40 AM
Dieselized User
gkamysz's Avatar
Chicagoland
Joined Feb 2000
7,301 Posts
Rob, that feed would be much too slow and drag the cutting edge melting the aluminum.

Feed rate = Feed per tooth x #teeth x RPM.

.001" per tooth, x 2 teeth x 20,000RPM = 40 IPM. If you can't feed this fast the cutting edge rubs more than it cuts creating heat and this causes the aluminum to melt to the cutter.

With aluminum, machinability depends very much on how hard it actually is. And this can vary. I would still expect it to cut at 20IPM.

If your machine is not sturdy enough to run these feeds and speeds you either need to reduce the depth of cut or reduce RPM (maintaining feed per tooth), or both. 1mm deep is too much I think. A two flute will cut aluminum better than a 3 flute especially if you can't feed faster. More teeth requires greater feedrate. More flutes reduces the ability of the cutter to clear chips and makes things worse.

I had a piece of aluminum that I killed 4 or 5 1/8" endmills on before I just gave up. Same feeds as always, and even my normal endmills wouldn't work. Well within the range recommended for the cutter, but I think the aluminum was soft.

Greg
gkamysz is offline Find More Posts by gkamysz
Reply With Quote
Old Nov 20, 2012, 09:50 AM
Registered User
raed5's Avatar
Orlando "Buzzards" FL
Joined May 2002
1,191 Posts
"6061T6" is very hard, and corrodes easily, 2024T3 would be a better choice!
T6, T3...etc indicates heat treat factor, "O" has no heat treat, very soft and can be bent by hand.
Raed
raed5 is offline Find More Posts by raed5
Reply With Quote
Old Nov 20, 2012, 09:56 AM
Dieselized User
gkamysz's Avatar
Chicagoland
Joined Feb 2000
7,301 Posts
7075-T6 is much harder than 6061-T6 and I'd much prefer to machine it. 2024-T3 is harder than 6061-T6 so it cuts better as well.

Greg
gkamysz is offline Find More Posts by gkamysz
Reply With Quote
Old Nov 20, 2012, 02:30 PM
Registered User
Denver, CO
Joined Dec 2005
6,259 Posts
Quote:
Originally Posted by gkamysz View Post
Rob, that feed would be much too slow and drag the cutting edge melting the aluminum.
-----
Thanks, must have been to late at night to do math right. I'll go back and fix it.
Roto Rob is online now Find More Posts by Roto Rob
Last edited by Roto Rob; Nov 20, 2012 at 02:47 PM.
Reply With Quote
Old Nov 20, 2012, 07:08 PM
Registered User
United States, CA, Santa Monica
Joined Jul 2011
493 Posts
Yeah, I used a feeds calculator and it seems like I won't be able to machine at any of the recommended speeds- I tried 16k and 30 ipm and my 1/8 in bit broke. I appreciate all the help- my CNC is made out of HDPE, so it's not very rigid. I think I'll try 12 ipm and 20k rpm at a depth of 0.04'' since that's what another person with a similar machine did.
Lpbug is offline Find More Posts by Lpbug
Reply With Quote
Old Nov 20, 2012, 07:48 PM
Registered User
Ward Hagaman's Avatar
San Diego
Joined Mar 2003
2,293 Posts
I'll bet that you are getting vibration. I would use as short an end mill as you can find ("stub end mill") and put it as deep into the collet as possible, and run the router as slow as you can (10K?). I wouldn't worry about feeding fast at first...shoot-- slow it way down in my opinion, and squirt WD40 every 10 seconds or so and see if you can get through the job. I don't think that a HDPE machine will be that great for aluminum. Have you tried G10? McMaster sells it at a good price.
Ward Hagaman is offline Find More Posts by Ward Hagaman
Reply With Quote
Old Nov 21, 2012, 03:47 AM
Registered User
Denver, CO
Joined Dec 2005
6,259 Posts
Do you have any info on the type of end mill. Like is it carbide, Hss, or even the manufacture.
Roto Rob is online now Find More Posts by Roto Rob
Reply With Quote
Old Nov 21, 2012, 09:55 AM
Dieselized User
gkamysz's Avatar
Chicagoland
Joined Feb 2000
7,301 Posts
The easiest thing to do is reduce depth of cut. Depth of cut you can adjust without impact to anything but total cutting time for the part. I cut a lot of parts at 0.5mm DOC before I made new spindle. because we aren't using stout machines you need to experiment with the machine to find it's capabilities. The tool specs are great when everything else is up to standard. Many things are coming into play. Tool run out could be a problem. If only one edge is cutting the load is much more than expected and the tool breaks. Tool runout is critical when using high RPM and fast feeds.

Greg
gkamysz is offline Find More Posts by gkamysz
Reply With Quote
Old Nov 21, 2012, 12:11 PM
Registered User
dpot's Avatar
France, Auvergne, Lapalisse
Joined Dec 2005
915 Posts
i find if i rub a paraffin candle on the alu plat you can see how hot it is getting and it helps the cuter to.
if you plung in and out the cuter dus not like it it is beter to cut in wit X Y and z mouvment and dwell betwen cuts use a drill to drill all the start points of the cut after that is is all down to speed and feed.
dpot is online now Find More Posts by dpot
Reply With Quote
Old Nov 21, 2012, 06:22 PM
Registered User
United States, CA, Santa Monica
Joined Jul 2011
493 Posts
@Rob I was using 2 flute 1/8 in carbide square end with TiCN coating.

@Ward I've cut G10 and Delrin with good success and nice finish. However, I really want aluminum arms for my quad (looks and rigidity), so I'll keep trying

@gkay I'll try 0.02'' or approximately 0.5 mm if the 3 flutes don't work too well with 0.04, but man will it be boring standing by the machine for 2 hrs squirting WD-40 haha
Lpbug is offline Find More Posts by Lpbug
Reply With Quote
Reply


Thread Tools

Similar Threads
Category Thread Thread Starter Forum Replies Last Post
Help! Cannot keep my Tricopters YAW Servo centered & stable. AcroFPV Multirotor Talk 14 Apr 20, 2014 01:45 PM
Question laser cut aluminum mgivens The Builders Workshop 11 Oct 03, 2012 09:18 PM
Discussion APM2.0 AUTO RETURN HOME SUCCESS! But cannot get position hold. OPEN MY PIDs. votreami Multirotor Talk 2 Jun 08, 2012 06:04 AM
Discussion Cannot solder aluminum tab to nickel ones ?? khaled_abobakr Batteries and Chargers 10 Apr 12, 2010 12:11 PM