Drilling was something I have thought about for a long time but the sherline chuck that I have is rather small. I could buy a larger chuck and a larger bit to go with it, but I think I would rather buy a roughing endmill to do the job. The hole that I need to pocket is not all the way through the work piece and is rounded at the bottom like a dome.
One of the first tips I learned when I got this mill is to rough cut the work piece as close to the final dimension so milling is minimal. for example, cutting a length of aluminum with a chop saw to say 2.05 to 2.1" and then milling to the exact size of 2" same with my large hole, drill it out then mill it to size which is something I might consider in the future but for the experience, I want to first try pocketing it with a roughing endmill and then finish with a ball mill.
I'm not sure I understand what you mean when you say tight bolt hole. My guess is that you are drilling a tight bolt hole pattern, where the holes are over lapping leaving a uncut "core" at the center. Great idea, but in my case it would only end up as an island.
--- In SherlineCNC@yahoogroups.com, "imserv1" <imserv@...> wrote:
> See below
> --- In SherlineCNC@yahoogroups.com, Ron Ginger <ronginger@> wrote:
> > > About your specific problem, Drilling is way more efficient at removing gross volumes of metal than milling. Drill out that center part of your pocket and get the part up high enough that the mill chip falls away below the cut. Some routines use a drill to "swiss cheese" a pocket ( or even a 3D surface)and then mill them. If your hole goes all the way through your material( ie not really a pocket), you can drill a tight bolt circle just inside the finish diameter, mill away the web between the drilled holes and the big plug in the center will break free, avoiding all the time required to turn it into swarf.
> > >
> > > Fred Smith - IMService
> > > http://www.imsrv.com
> > >
> > Fred, I have considered doing this on a couple projects, but I have
> > worried that all the holes create interrupted cuts as the mill passes by
> > the holes. Does this have much effect? I would think it could set up
> > some awful vibrations.
> Just remember that you can cut this material without the drilling. The drilling only makes it easier. Set your feed rate as if it were not drilled, to start. If you are cutting across webs between holes, you will get the benefit of a lighter average chip load and this will permit you to ultimately increase your average feed rate.
> One of the techniques developed for high speed machining of hard materials with dry cutting conditions is a circular approach to the work material. Called trochoidal milling, it creates a similar tool loading pattern as milling through a pocket of pre-drilled material. The variable step over distance gives the tool a chance to cool and purge built up chip as it proceeds through the cut.
> This example was not done on a Sherline, but..., the first assembled controller we sold was mounted is a heavy steel enclosure, 8 x 10 x 4 high. The boxes were powder coated. The lid had a 120 mm fan installation. That required that we cut a hole approx 4" dia in a 1/16 thick steel part ( plus some other cutouts for switches, mounting, etc). I tried several techniques to knock that hole from the material. The best method I found was to use a quality #3, cobalt, Centerdrill to drill a tight bolt circle, leaving about .02 between hole diameters. Then to rough cut and finish with a 1/8 4 fl carbide em. It worked very well and the total machining time was 40-50% less and tool life was over 50 pcs, vs 5-6 without the drilling.
> We used this technique for the other rectangular holes too, not just the fan cutout. We used VectorCad-Cam to program the hole patterns at evenly spaced distances along the contours.
> Fred Smith - IMService