what type of end mill to use?

I have to mill a profile out of 1/8" sheet brass, exact composition
unknown. It isn't very hard, though. This will be entirely edge
milling i.e. milling with the side of the end mill. I very rarely
mill brass and I'm unfamiliar with its machining properties. For
side milling of brass sheet stock should I just use any 4-flute
end mill, or is some special topology highly desirable?
Thanks!
Grant Erwin
Reply to
Grant Erwin
Loading thread data ...
Just use a sharp one. You do know about brass being 'hungry'? If you have no size restriction, like for inside corner radii, use somehting fom .187 to .312 diameter. I like standard 3 flute for something like this, but a 2 or 4 will be fine. Standard helix, and a light spray of water soluble coolant, though most will say run it dry. The spray will blow chips away, helps with visuals.
mj
Reply to
michael
I have always heard that brass likes to be drilled with a drill bit with no rake on the leading edge. If the bit has rake, the bit wants to screw itself into the brass. I have always ground the leading edge off my drill bits (the leading rake angle is parallel to the length of the drill) when drilling brass, with remarkably better results than the factory points.
Sooo...With this in mind, I would grind the leading edge of the milling cutter to a zero rake, i.e. parallel to a line through the center of rotation. This should keep the cutter from grabbing and trying to feed itself into the work, resulting in a more accurate cut. I have never milled a piece of brass this thin, and would be interested in what you discover in the process.
Brownnsharp
Reply to
brownnsharp
Brass mills easily, just use a real sharp cutter.
Your problem here will be clamping. 1/8 stock will want to pull up and chatter. I'd suggest you make a brass sandwich. Sacrificial material above and below, clamp it all to the table.
Karl
Reply to
Karl Townsend
I also make a sacrificial sandwich for this type of work, out of plywood. With planning, screws can be used to hold the sheet in place in certain areas of your pattern. If the shape is irregular, and doesn't have to be oh so precise, I draw the design onto the plywood and mill away at the "sandwich". I have a 4" wide bar stock that has been milled to a "T" shape of end profile, tapped through vith various sized holes, that I clamp into the mill vise for this type of flat work. Bolts, or a toolmakers clamp or two will allow you to turn the work as necessary to whittle away at it. It's one of the handiest milling accessories that I use.
RJ
Reply to
Backlash
I'm making a special-purpose workholding jig just to do this profile milling on the rotary table. There are two holes in the part and I'm planning to use them to hold the part down with. Unfortunately I'm going to have to use #10 SHCS to do the holding, but it's only 1/8" brass and I'll take it easy on the milling. I have to make several of these parts and this seems to be the only way. The work will be supported on steel bushings below (just smaller than the profile) and clamping washers above (also just smaller than the profile) so it's already sort of a sandwich idea.
It's my first attempt at making a jewelry-type item, we'll see how it goes.
Grant
Reply to
Grant Erwin
Greetings Grant, I machine a lot of brass. Sheet, round, hex, and square bar etc.. Your sheet may be half hard brass or it may be soft. Half hard machines best. The soft brass will be gummy. And making a conventional cut will show this rapidly as the chips tend to stick to the cutter and get pressed back onto the work. Use either a two or four flute cutter. If your set up allows climb cutting is best. Use a non sulfurised cutting oil. The sulfur stains the brass. Water soluble oils without chlorine work great. Use 300 to 350 sfpm with HSS tools. The brass can be routed easily. So, if the contour tolerance allows you might want to consider making a template and routing it. Drilling half hard brass with a regular drill risks having the material pull the drill into it. Especially if you are enlarging a hole or drilling after center drilling. Stoning a drill like one made for drilling plastic helps to avoid this. Brass cuts so easily you will love it. If you have a choice when buying the brass get the half hard. If you will be milling pockets, even one that's quite shallow (.010) the half hard sheet will warp. Just milling a contour on the oustide will not cause this major warping though. If you use a 1/2" dia. cutter you can stack the sheets up 8 at a time and cut them all at once. Clamping well of course. If you can, make your setup so it is possible to add clamps and remove others so the part can be milled all around in one clamping. The half hard brass will make sharp chips that are like needles so watch out. Cheers, Eric R Snow, E T Precision Machine
Reply to
Eric R Snow
All of the information you have received is good, but the less helix with either the drill or the endmill, the better.... Soft brass is very gummy and will tend to chip weld... a very light cutting oil may be in order if this is the case. Chip welding will destroy any surface finish you were hoping to get.
Reply to
Gene Kearns
It has been suggested that limonene is a good cutting fluid for all non-ferrous metals. I have not yet had occasion to try it on brass but it sure works well on aluminum.
Ted
Reply to
Ted Edwards
I do edge mill sheet brass.
If thick enough to not bend you can use spiral flute mills.
If there is a chance that it will bend use straight flute mills or in an emergency use a reamer as a mill.
Watch for buildup of chips that clog the flutes.
Hugh
Reply to
Hugh Prescott

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.