Design Parts to save you money!
Trying to make your parts for the least cost? Todays article looks at reducing the cost of machined parts through careful management of internal pocket radii.
Forward this to your favorite mechanical engineer or design professional!
In the picture above we can see a deep pocket part with a internal radius of 0.296 inch. The depth of this pocket is 1.7inch. A typical rule of thumb on pocketing is that you (ideally) do not wish to go deeper than 3D, that means that for a 0.5 in diameter cutter you don't want to have a pocket deeper than 1.5 inches, so this pushes that envelope just a little.
Looking closer you can see a 0.296 inch radius, why is that nice?
If the part designer had elected to use 0.250 inch radius that would make this part hard to cut, that's because as the tool approaches this corner its path would engage a full 270 degrees on the cutter diameter, that represents a "torque spike" on the tool. The torque spike at best makes for a "chatter" pattern in the corner, and at worst can shatter your tool. If the corner was radius 0.25 in then you would have to run feed optimization (that slows the tool down for the corners) or the whole profile would be just run slower than need be. If the corners were tighter than 0.25 in radius then the shop would be forced to use an even smaller cutter, exceeding the 3D ratio and that would slow things down even more.
A tighter radius than 0.25in would add 60+ seconds to the part run time. While that may not seem like much; at typical shop rates that is about $2 extra per part.
So the moral of this tip is: "Always look at using the largest possible radius for internal pockets, and push back on your pcb designers to round off those square board corners, its a trivial thing for them and saves $$ per part. Always pick a radius that is about 20% larger than a nominal cutter size, ie 0.3in instead of 0.25in"
Call us for more information or for a no obligation DFM part review.
Sign up for more tips!
The video below is the simulation of the part cutting process, you can see the finished article on our website homepage in the galleries.
In this specific instance we pre-drilled the whole pocket with a 10mm carbide parabolic flute drill bit (100 ipm feed), roughed it with a 0.75in rougher on a ramping perimeter profile (50 ipm feed), followed by a ramping cut with a 0.5in 3 flute finisher (100 ipm feed), overall cycle time was 1m30s for that set of operations. That's about 4 cubic inches of material removed per minute which is very aggressive.