The Panel Pro uses a rotary cutting tool called an end mill. In this white paper we will explain the different types of end mills and their uses.
Nomenclature:
size. The nominal cutting diameter.
Shank. This is the part that is gripped by the collet of the router. The Panel Pro routers employ an industry standard ER11 collet that can accommodate up to 1/4” shanks. Typical shank sizes are 1/8, 3/16, and ¼ inch.
Metric sized ER11 collets are available at various industrial supply firms. The shank and the cutting diameters may be different.
Length of cut (LOC). The length of the end mill that is intended for cutting.
Overall length (OAL). The distance from end to end.
Flutes. The cutting edges.
Center cutting. The term used to indicate an end mill is able to plunge straight down without an existing hole.
Single ended means there is only one end intended for cutting. Double ended means both ends are capable of cutting with the shank in between these two areas.
End mill material. While high speed steel end mills are available in larger sizes, they are too flexible in the smaller sizes like 1/8”. The most common material is either pure carbide or in some cases 90% carbide, 10% cobalt which makes them a bit less brittle.
Typical material cut with the Panel Pro is aluminum of various grades and plastics.
The Panel Pro routers are variable in rpm from about 10000rpm to 240000rpm. Using a commercially available feed and speed calculator, assuming a 1/8” end mill and 1/8” thick 2024T3 aluminum cut full depth, it recommends a feed rate of 33.6 inches per minute. This is based on 24000 rpm and yields a surface speed of 785 feet per minute. This is the speed that the cutting edge is moving through the material.
The calculations also produce a chip load of about .0007 Inches per flute.
When a bit breaks, the first inclination is to reduce the feed rate. This is rarely a good idea because it does not allow the sharp edge of the flute to dig in and actually cut.
The 33.6 inches per minute also assumes a perfectly rigid tool and work piece. As you know we clamp aluminum sheet onto 1” square bars. The Panel Pro itself is constructed out of aluminum extrusions. This can not be considered a rigid set up. In addition it appears the speed and feed calculators do not take into account the length of cut.
The longer the length of cut, the weaker the cutter will be. It will flex and ultimately break from fatigue.
Before we got smarter, we were using a single ended 1/8” end mill that used a 1/2” length of cut. We found the life to be very short. They were breaking at about the end of the flutes where the flutes end and the shank starts.
We were able to find a high strength end mill that would extend the life, but we would still recommend figuring on an end mill per panel.
Then we discovered the double ended end mill. This end mill has 2 flutes, a 3/16 shank and a 1/4” length of cut.
With this end mill, about the only thing that will break it is if it runs into something with the router not turning. If the router is turning, it cut through just about anything including clamps.
The fact that it has a 3/16 shank and only 1/4” LOC, makes the end mill immeasurably stiffer. You can see the cut difference in the chips. They are a nice cup shaped chip whereas with the 1/2” loc the chips come off as sharp little shards.
We still back down a bit from the recommended 33.6 ipm feed rate however and find that 20ish seems to work about right from experience. AvCAM move settings includes a feed rate calculator intended for 2024T3 that gives a reasonable ball park.
Number of flutes:
I have had people suggest using a 4 flute end mill because it would be stronger. They do not work. The area to extract the cut material is too small and the flutes will pack with swarf (cut aluminum chips). We have had a custom end mill made for us that incorporates the 3/16 shank, 1/8” double ended end mill but with just one flute.
This end mill works way better on plastics and soft aluminum than the 2 flute end mill. I have used it to good success on 2024 as well. We have this end mill available on our web site. There are commercially available single flute end mills available, however they typically have 1/2” length of cut and unless your just cutting plastic, you are back to the excessively flexible scenario again. Reducing the number of flutes increases the chip load and the G wizard machinists calculator suggests 16.8 IPM for this end mill, again with rpm at 24000, 1/8” depth of cut.
I mentioned earlier that reducing feed rate on 2024T3 is a bad idea, however, reducing feed rate may be applicable on softer materials where there is a tendency to clog the flutes.
Cutting more brittle plastics like acrylic work fine with a 2 flute end mill. Anything softer such as the polyethylene s (hdpe etc) or lexan should be done with a single flute end mill. Soft materials like 5052 aluminum or copper should be cut with a single flute end mill. If at all possible, make holes that are larger than the end mill so that the end mill does not plunge straight down. If you plunge straight down in polyethylene or lexan, a long stringy chip will wrap around the end mill and you will have to stop frequently to clean it off or it will build up and mar the surface of your material.
Coatings do not seem to make a lot of difference for cutting 2024T3.
get panel Pro end mills here. If you cant follow hyperlinks, paste or type this into your browser http://BullerEnt.com/product-category/panel-pro/panel-pro-parts/
Bottom line. Get the shortest length of cut and the fattest shank and the fewest flutes. Push it hard like 16 – 25 inches per minute