• I want to thank all the members that have upgraded your accounts. I truly appreciate your support of the site monetarily. Supporting the site keeps this site up and running as a lot of work daily goes on behind the scenes. Click to Support Signs101 ...

help requested in routing .040 aluminum license plate blanks

iSign

iSign

New Member
well, this is just a last minute effort to bang out a few license plate blanks with radius corners. I already got client approval to hack up some 6x24 riders into 6x12 sign blanks with square corners.....
-
-
-
-
-
-
-
-
-
oh... I just found this half written post that I forgot about, hiding under my enroute window...

anyway, by now I've finished the job... partly on the assistance of GB2 who I called first, and also Dale, of Big Squeegee fame... so, I ended up cutting up these standard .040 white sign blanks using a single flute up spiral. I tried a double flute down spiral I loaded just for the occasion, and the first one broke the second it hit the table, which i think was partly due to my bad guess to slow the rpm's, combined with not enough hold-down tape to assist my vacuum...

so, in the end, 90 ipm feeds, and 22,000 rpms on the spindle seemed to give me good results with the single flute up spiral. I didn't want to deal with the auto mister since i was just cutting 5 license plate blanks, and i had cut .040 a year ago without fluid...

well, I was going to ask for advice, so even though the job is done, I did have a little de-burring to do & wondered if better results are available, so anyone want to chime in with other considerations?
 
S

SqueeGee

New Member
Routing aluminum was my least favorite thing to route for all the reasons you mentioned. Holding it in place was always a hassle and I hated setting the mister up. It would make a mess of the shop and I would always forget to reverse the cut direction leaving a gnarly edge.

Somethings that I did to help was:

I sold my router and have gone back to outsourcing this work.

Doug, you know I kid. I hope you're doing well. Happy routing!
 
iSign

iSign

New Member
hey, Dale mentioned reversing the router too!!! just like reversing a circular saw to cut metal.. but I didn't want to try that, having never heard of that before...

did you do it with router keypad controls, or software?
 
iSign

iSign

New Member
oh ok... conventional, or climb... I know where that is... ok, gonna try that.. maybe I should tape a sheet of 1/8" PVC to my MDF spoil board & then try out the mister.. I think the aluminum will be bonding better with tape to PVC, plus the oily cutting fluid will mostly stay on the PVC, instead of saturating the MDF...
 
Typestries

Typestries

New Member
Best way, sharp onsrud or belin 2 flute upcut, very wet, 30 ipm feed, slow plunge so the tip of the bit does not gum up right away, 18k rpm. It's not fun but it works. Adding bridges on alum helps. Did I mention I too like routing alum the least-esp painted. 5052 routs like a charm, 3003 not so much.
 
CES020

CES020

New Member
You should try Tri-Cool MD7 Synthetic coolant. Works wonders on aluminum. Not cheap, but it's designed to be used in a micro drip system. However, a spray mist system with it dialed all the way down will work and not burn too much up. Costs about $100 a gallon, but it'll stop all that gumming up and rolling a burr large enough to skin a deer hide with.

Climb or conventional doesn't matter too much if the cutter is buried all the way around. It might make a slight difference, but I've not seen any noticeable difference in my experience. If the flutes are not surrounded by material (like a slot), then climb and conventional can make huge differences. They do 2 completely different things with the chip that causes that.

If you have some problems, give that MD7 a shot. You can saturate a spoilboard with it and it won't harm it. Doesn't make it swell up like water based coolants. It's really really nice stuff. They also have MD1 that's a vegetable oil. I've heard good things about that, but I have not used that one.

It takes so little, you won't have to fog up your shop to use it.
 
Malkin

Malkin

New Member
I have no router experience or advice, but for only 5 cuts I would have just scored them with a knife and snapped them against the edge of a table.
 
SignManiac

SignManiac

New Member
What little bit of aluminum I choose to cut, is done with a vortex tube hooked up to air compressor. Does a good job of keeping the bit cool. My table came with the misting system but it's never once been used in ten years.
 
J

John L

New Member
I have seen answers to this question all across the board. I have come to realize it is entirely specific to your particular setup; hold down method, spindle/router HP, router frame size and flex, size of the parts you are cutting, etc etc etc. It doesnt seem that these things should make much of a difference but I am now 100% certain they do in a big way.

If you already got fairly acceptable results once, I would make a big note of the details of that setup and tape it up near the computer you use for your toolpathing. You can then use that as a baseline for experimenting with your equipment in looking for that magic recipe that leaves no burrs, doesn't struggle or plow through, decreased cutter wear, etc. etc.

I personally got the most awesome cut with... Onsrud 1/4" single edge UPCUT SPIRAL SUPER 0 FLUTE, PN: 65-025 (1/4" version of the bit).

My feeds and speeds for .040, .090, .125 alum with these bits are:
1/4" bit 12,200 RPM's, @ 1 IPS, Z @ .40 IPS
1/8" bit 18,100 RPM's, @ .40 IPS, Z @ .40 IPS

I use vac hold down, sometimes a few perimeter clamps just to be sure, and cut it dry.

I cut up to .090 with a single pass. Thicker material, no more than .090 per pass.

Look at the chips. You want them to look like little smiley face smiles. In my case, the little smiles would go about 40% the way around the circumference of the bit I am cutting with (either 1/8 or 1/4").

best of luck.
 
G

GB2

Old Member
Checking Gerber's website, they suggest for cutting .125" aluminum with a .25" bit, using a feed rate of 30 IPM, a plunge rate of 10 IPM and a speed rate of 18,000 RPM:

http://www.gspinc.com/downloads/PDF/fastfacts/5049.pdf


Checking Onsurd's website, they offer a calculation method to determine the proper feed and speed rate based on the specific bit:

http://www.onsrud.com/xdoc/ChipAluminum
http://www.onsrud.com/files/pdf/Chipload_Aluminum.pdf


I also have a mister and have hardly ever used it, and it does make a huge mess. Unless you are cutting thick aluminum and/or cutting a volume often, I can't see using the mister for a one time or minimal use, especially for .040 aluminum. You can always supplement the mister with air sprayed on the bit from your compressor as the job proceeds or even a squirt of water from a manual squirt bottle if you feel it's needed. The idea is to find the optimal feed and speed rate that shaves off chips of aluminum while building the minimal amount of heat in the process. I think the Onsurd chipload chart is a good resource as that is the approach their calculations attempt to achieve.
 
skyhigh

skyhigh

New Member
I personally got the most awesome cut with... Onsrud 1/4" single edge UPCUT SPIRAL SUPER 0 FLUTE, PN: 65-025 (1/4" version of the bit).
Click to expand...

I just cut my first "aluminum" anything the other day. That was alumalite, so not really a great feat (.012 thick alum x 2 sides + the plastic) I used the same bit your talking about John.....and it left one heck of a mess.....not with the metal, but with the plastic. The utility knife cleaned it up pretty quick.

John, you didn't mention if you do conventional or climb?


Doug, 5 license plates? I wouldn't do that solely on principal......LOL. (I know....it was practice)
 
G

GB2

Old Member
Belin, another premier router bit manufacturer, has some guidance in the last pages of their catalog also...good luck trying to figure it out though:

http://belintools.com/Catalog.pdf


Also, Hartlauer, one of the best suppliers of router bits has some very simple tips that make good sense if you're having trouble trying to figure out the best feed and speed rates. Also, in the middle of their catalog there is a chipload chart that is very helpful:

http://www.hartlauer-bits.com/hints.html
http://www.hartlauer-bits.com/HartlauerBitsList.pdf
 
Techman

Techman

New Member
no need to use a mister for aluminum.
All it does is flood the shop with aerosol mist.
USe a squirt gun or an old oil squirt gun and fire away about every 7 inches.
Aluminum likes wet flooded. not mist.
 
J

John L

New Member
Skyhigh, I always climb cut aluminum here. AND always ramp into the material, do not plunge straight in or you will cause greatly accelerated bit wear.

I only rarely cut any factory laminated composite material any more but any of those 65 series bits should work well for both the aliminum and the plastic layers of the material.

In the past, to get decent edge quality in Alumipanel and Dibond (hope thats similar to your Alumilite), I have run seperate cut files for the alum and the plastic. The first pass will ramp in and is just deep enough to go through the alum. I blow off the sheet real well to help prevent the bit grabbing a shard and rasping up the plastic core. I then run a plastic toolpath with the same bit - but it has now been toolpathed with my plastic speeds and feeds (but also climb cut).

Another reason to ramp in, especially with the laminated panels, is that a plunge cut with these 65 series bits will push a little circle of metal into the plastic and sometimes that sharp little circle will spin around with the bit and really cause havoc with the plastic edge quality as it cuts along.

Also watch that these laminated panels dont get too hot at the edge because they can delaminate between aluminum and plastic. Just watch the chips that are coming off. The sheet and the bit should not be getting hot if it is cutting properly.

Some of this stuff really is an expensive experiment until you get it running the way you want. I have a cup full of broken carbide to remind me to test. Once I get a setup working, I sometimes then take a small piece of the actual material, write what I did on it, and hang it by the toolpathing 'puter.

Hope thats of some help to you anyway.
 
You must log in or register to reply here.
Top