Aluminum .080 Cutting advice needed

[Hobodog2]

What bit should I use to cut .080 soft aluminum and what are your recommended feed and speed?

Thanks,

Pete

[Brady Watson]

Hold-down is critical. You should be using vacuum. Screws are not recommended.

You want to get a upcutting single spiral-O made for cutting metal. You cannot go faster than 1.5 IPS with a single flute tool.

ALWAYS do a ramped plunge on the Z axis. Run 1.2,0.7 @ 15,000 RPM.

See how it cuts & adjust accordingly.

-B

[Hobodog2]

Brady

Thanks for the input. I do have good vacuum, but I was going to use a downcut to avoid any uplift of material and also try to have a clean cut surface, but I will try an upcutting bit per your recommendation.

Any recommended brand/model bit?

Pete

[Brady Watson]

Onsrud makes a good single spiral-O. Get the shortest cutting length to get thru the material. Harvey Tool is also great to deal with & probably a bit cheaper.

You don't want a downcut because a smears the AL down into your bleeder, and causes burrs & the material to lift slightly - which defeats the purpose. You may want to search for Vaccum Film Technique on this board to get some ideas. Also, WidgetWorks makes a pressure foot which may be of interest.

-B

[MogulTx]

I use speeds about the same as Brady is recommending. I use an Onsrud Bit of the "63" series-( you pick the diameter and cutting length). If you run into any issues with malling and melting ( I don't think you will at 1.2IPS. I usually run at 1.3 myself, so it sould be a good speed.)


Before you start, if you spray the bit with a silicone spray, it will help to not have the aluminum latch onto the bit.

I usually set my depth per pass at .032 if I am going very deep - so it has an easy go of the cutting. This gives me a smooth edge and then I use a spiral ramp down, as well. I have cut 1/4" and had no issues.

When working with the soft aluminums (you're gonna hate this) I would use a WD40 spritzed on the bit every now and then. It will get into your spoil board so don't use it wildly.

I run a PRS Standard 4 x 8 with PC router... sometimes the size and configuration may matter so I throw that in for reference.

I have cut 103" long templates (Screwed to spoilboard on diagonal- so don't discount the use of screws to ensure the material does not move on you) in 1/8"- 5000 series aluminum several times with no problems.

Wear your eye protection!

Monty

[shoeshine]

If you can stand the mess, I use CRC brand thread cutting lubricant. It is sticky foam made for horizontal boring so it stays in place, and comes in a standard rattle can with the red straw so it is easy to get where you need it. You do need to wash down your pieces after with a degreaser though (dish soap works too)

I find it helps immensely with both quality of cut and bit life.

Chris

[Hobodog2]

Thanks to all for your inputs.

I need to get some more bits and try some of the techniques suggested (I broke an 1/8" Onsrud 63- series).

I think I need to go with a 1/4" size rather than 1/8" if I can find some.

Thanks, Pete

[tlempicke]

Thanks to all for your inputs.

I need to get some more bits and try some of the techniques suggested (I broke an 1/8" Onsrud 63- series).

I think I need to go with a 1/4" size rather than 1/8" if I can find some.

Thanks, Pete

Believe it or not Amazon has the bits you want. Prices OK and they have free shipping if you buy fifty bucks worth.

[SomeSailor]

I cut a lot of .080 and have been having great luck with Amana Tool bits. I cut dry in one pass at .65 IPS and lay down a sheet of poster board under the aluminum and set my depth at about .005" deeper than the material. I use screws to hold down 2' X 4' sheets and use tabs to hold cutouts in place where needed.

The bit I use most is the #51402 (Solid Carbide Spiral 'O' Flute, Aluminum Cutting 1/4 Dia x 5/8 Cut Height x 1/4 Inch Shank Up-Cut)

[meatbal80]

I have found much of the information mentioned above very helpful. I am also trying my hand at aluminum for the first time. I have an onsrud bit i have tried, what i am wondering is if i get a build up on the bit is it then garbage? Can i remove the aluminum with something other than a blade?

[Brady Watson]

Joel,
You will get some buildup, but it will mainly just color the bit like aluminum paint. You should not have a welded glob on the end of the tool. If you do, stop plunging straight down into the cut - instead, ramp into the cut. You must ALWAYS ramp into the cut when cutting AL. You cannot drill AL and get away with it like you can with wood. Use a spiral ramped plunge instead.

Also - don't be skeered :eek: AL 'sounds wrong' compared to other materials due to the harmonics involved. Don't fret. You want to make sure that you are making chips - not dust. The chips carry the heat away & this is critical. You can determine your chipload by measuring the thickness of the chips rooster-tailing out the back of the router with a digital mic. Make sure you are running 'in the range'. There are plenty of CL calcs online, as well as in SB3 itself.

Wear your safety glasses!!! Even when the cutting is done & you are just removing parts! Static buildup can cause a polarity switch and shoot chips into your eye.

-B