Printable View
Im trying ti machine a cup die out of 1018 steel, normally this would be done on a lathe but i would like to try to do it on a mill. its pretty much just a pocket thats round at the base, 5in. in dia 6 in. deep. I figure machining this part would be simular to mold making. What type of tools are generally used for simple molds? I know master cam has a lollipop endmill but ive not yat been able to find one, are ball endmills my only choice?
Drill a hole as large as possible in the center of cavity, rough out rest of the material with a carbide inserted shell mill, then finish with the ball endmill. Use the largest BEM to finish sides then use the correct size to pick out the material left for your bottom radius.
A ram EDM would provide a better wall finish.
I'm sure there is some draft. I've accomplished this several times. I did a standard Z-axis rough. Then finished with a Tapered Endmill (Draft angle cutter). The core I also did the same way. You'll have a much better finish and the CNC time is fairly quick. No fancy programing. Less polishing.
Quote:
Originally Posted by hydrospin01
That's pretty deep for a standard ball endmill unless you're going to buy a big one.
Are you sure you don't want to stay on the lathe? It will be faster, and the tooling will be cheaper.
How I would normally machine a deep pocket with a radius at the bottom corner, is with a Bull-nose endmill. You can use the radius to get a nice smooth finish and you can use a much larger diameter endmill which typically will have longer length, and is much stiffer.
There are several ways to program it for a CNC, to cut the taper, but in a manual mill you would likely need to use a tapered endmill to put draft on the cavity wall.
Jim
I agree a bull nosed taper end mill would work fine. If you can't find what you need. Just get a standard tapered end mill and have the local cutter grind shop do the radius for you. I do them my self on my cutter grinder but I'm sure it could be done for around $25 or so. The custom tool would easily pay for itself in the time you'd save. I'd probably get or make a straight bullnose to do the ruffing and finishing of the bottom.
When I have to cut detail like this, I usually program a straight cutter to step down the wall and around the radius, leaving stock to clean up later. Then I will come back in with the bullnose cutter to do just the last 0.005-0.010". This way I don't wear out my expensive cutter roughing out steel.
Jim
I'm looking at a similar type of project, my taper is on the O.D. and it's about 52" in dia. I was wondering if chucking up a carbide bur in my mill would work for the basic roughing?? I have access to a 8" long set of bur's which would reach just dandy [max needed depth is ~6" or so] but I'm not sure if this would work...Crazy idea?
Curious..
Jerry
Burrs are not good for roughing, they can't handle the chip load for taking heavy cuts. They might do fine for finishing.
Jim, if I was to limit to 1/32 step over w/ a full DOC [~1/2"] and about 15-18krpm, that would suffice as a 'light/finish" cut? Does using coolant help when using a burr? I haven't really found a better way to do this part, I'm a bit scared that using an end mill that long will cause issues w/ chatter and the in-ability of my mill to handle cutting loads which are too heavy.[it's really just a heavy router, not a mill...] We'll have to see..
Jerry
I know this is a CNC forum, but you could cut the "cavity" with a flycutter and rotary table on a convetional mill. You can cut concave as well as convex shapes this way. Mount the work on a rotary table, axis being through the center of your cavity. The fly cutter needs to be set to a specific diameter. The head of the mill needs to be rotated on an angle. It has been a long time since I have done a set up like this. I will need to do some checking into my old notes as to the exact calculations for the cutter setting and head rotation. Check back later after I have researced this. I will post later.
I would use a large bull (not ball) nosed end mill. SGS carries a varitey of sizes. A bull nose is a flat bottomed end mill with a .02 or .03 or .06 or .120 dia. in the corner. So a 1.00 dia end mill with a .06R. in the sharp corner. this makes it so you don't have to take a small end mill a mile deep. I also have an edm at my shop. I use a lot of bull nosed end mills.