[david rendon]

Hello everyone,
I'm machining a concave surface using a 7/8 2 flute carbide endmill and the problem I'm finding is that when the ballmill starts cutting with the quadrant, the surface finish starts to look not so good.
Any advice on wich tooling I should use?

[awerby]

So it's hard to say exactly what your problem might be. In general, ball-end milling cutters are the only way you can machine a concave surface without "stair-stepping". But it could be that your endmill is too big, or you're trying to take too big a bite at one time, or your machining strategy is flawed. If by "cutting with the quadrant" you're talking about the steep sides of a bowl-shaped concavity, I'd suspect the latter.

I don't know what program you're using or what strategy you've chosen, but there are several ways in which a CAM program will attempt to cut a concave surface. One is horizontal finishing, which places tool passes at a given spacing in the XY plane. This works fine for shallow areas, but as you start climbing the steep part of the slope, it will start placing the passes further and further apart vertically. Another strategy is called "waterline" cutting, which works similarly, but spaces the passes apart vertically instead of horizontally. This will work best on the high sides of a bowl, but less and less well as it comes to the shallow part, since there is increasingly less vertical distance between the passes. The solution to your problem may be to divide your concavity into steep and shallow areas, and use waterline cutting on the steep parts, and horizontal finishing on the shallow ones.

Of course there are more elaborate strategies available in some CAM packages; you might check yours to see what's available that might do the whole surface at once, or remachine certain areas for optimum surface quality.

Andrew Werby
ComputerSculpture.com — Home Page for Discount Hardware & Software

[david rendon]

thank u Andrew
I'm actually cutting on Y direction, taking small steps down Z (imagine that my concavity is projected on Z-X plane).... the finish looks good until the cutter starts reaching to the lower part of the concavity.
I'm using a 7/8 ball mill and planning to change that for a 1.0" (need to reduce the time aswell).

My next plan b is to change the cutting direction ( I'm gonna arc on Z-X plane) =)

[78nova]

I would suggest trying a 3-flute solid carbide ball end mill like from Fullerton Tool Company. Fullerton Tool Company - Solid Carbide Cutting Tools | FullertonTool.com A 2-flute ball just does not seem to work as well especially when you start to reach the lower part of a concavity and if it is not a very good center cutting tool. A 3-flute will be much more balanced and leaves a better finish. Smaller step over amounts and swarthing across or around will also benifit. What is the 2-flute you are currently using? Is it a resharpened tool or have a factory grind? Is it a Ski-carb type tool? Ski-carbs are a special type of high performance end mills that have a third (neutral or circular) land along with the primary & secondary lands & cut to center very well. A manually ground tool will most likely always under perform to a precision factory grind concerning high performance end mills.

Take note* A ball mill only works as good as the grind it has on it. A 5-axis plus tool grinder will be able to apply the best possible grind. If you used a basic manual tool grinder to establish or sharpen a ball end mill, it will not perform as well as a factory grind and most often, much worse. We also use Fullerton 2 & 3 flute end mills. When one chips or gets dull, a resharpend one will not perform at all like a new one. My best tool grinder on a monoset can get it close but they just do not perform as well as a precision ground factory grind, side cutting, it works OK, end cutting, not so good on a resharpened tool. A good cnc multi-axis tool grinder is worth it's weight in gold when it comes to trying to duplicate a factory grind.

[mfgbydesign]

I as well am having difficulty visualizing your operation. Perhaps a screen shot attached would help.
Some thoughts are, you are cutting top to bottom, and reaching the bottom using more of the tool tip where there is low surface speed. I try to start at the bottom and work my way up to use the side of the tool. Besides surface speed the grind is generally better here too.
When you're pushing the tool to the bottom of the contour it tends to wander. When you climb cut with the side of the tool the deflection is in one direction.