I almost didn't click this thread because I'm not aware of a best endmill for slotting. There isn't even a best technique, because a rigid machine with high pressure coolant can use different strategies than a lighter machine tool and a squirt bottle. That said, to answer the question, I feel a three flute cutter is the best endmill for slotting, and a cutter with variable pitch and variable helix will help prevent the chatter and gouging that is a common problem in the process. However, most any cutter will work fine for just slotting a guard, it is the technique that matters most.
For me, a lot of the cutters I use utilize an odd number of flutes, which reduces problems on the surface 90 deg from the cut, however most general purpose endmills are two or four flute, so I'll stick to them.
If you insist upon plunging, you will get better results with a two flute. If you're having problems re cutting chips due to a very deep slot, you will want a two flute. Also, a two flute will gouge less in a less than rigid setup. That said, I do like the improved productivity of a four flute, even when slotting.
A relatively foolproof technique for cutting a 1/4" slot in high carbon steel with a less-than-industrial-machine-tool:
Drill 3/16" holes on both ends of the cut. Unless you have a very rigid setup, plunging is really hard on endmills because the wobble is basically uncontrolled motion, which wipes out your cutting edges, particularly with carbide.
Don't use more tool stick out than necessary. Deflection in the cut is going to be a problem. 3/4" stick out max.
Using a 3/16" four flute carbide cutter turning 1800 RPM plunge 1/16" into your predrilled hole and feed to the other hole at a rate of about 6 inch per minute (IPM). So a 1 1/2" slot will be crossed in 15 seconds. Blow the chips out. Plunge another 1/16" and feed back to the other side. Repeat until you're at full slot depth, it should only take a couple minutes. If you're doing this with carbide (which is ideal for slotting because it is stiff) you can turn it up this high and feed this fast, but you're going to want to wear good eye protection to keep hot chips out of your eyes. Use regular (or constant) air blasts to keep the chips out of the slot and the cutter will last a long time. Re cutting chips is what damages carbide in this application, not heat or lack of lubricant.
The next step is to feed over in one direction to cut one side of the slot, leaving a little stock behind for finishing. Feed over in the air and plunge down at 6 IPM to a depth of about 1/4". Climb milling is best in a slot because it reduces chip re cutting. Climb milling on a manual machine without ballscrews can cause uncontrolled feeding as the backlash is taken up by the cutting forces, but usually not with a light cut and a cutter this small. Just be on the look out for it. Do this on both sides until you're at full depth and full width.
If you want to take a finish pass with a 1/4", use a 2 flute or the wobble at the end of the cut (where it starts to plow) will cause a gouge on the left hand side of the cut.
Speeds and feeds and depth of cut in a CNC using a quality 3/16 cutter in high carbon steel would all be about double, so the job would take about 1/4th the time. The one relative constant would be chip load per tooth. You need to be between .0003 and .0015 for a cutter this size in this material. If you fall below that range the cutter won't cut properly, it will rub, which will dull the cutter and work harden the work piece. If you go above that range you'll overload the cutting edge (and possibly run out of relief), even on a really shallow cut.
So, your feed rate window is tied to your RPM. Your RPM (actually your SFM) is tied to your cutter type (size, material, coating) and the material being cut. Your depth of cut is tied to your cutter diameter and material cut,the cutting angle (slotting is 180 deg), machine and setup rigidity. And to some extent the volumetric displacement of your balls...
Cutters are almost always under nominal, so unless you have a lot of runout, a 1/4" cutter used on your finish pass will likely leave a .248" slot. Something to be aware of.
