Designing parts that are easy to machine can make a huge difference in part cost and quality.
Make sure inside corners take into account endmill radii.
Try not to design sharp, square inside corners. Allow for the radius of the endmill. If you must have a pocket with sharp square corners, there are ways to accomplish this task (broaching, EDM, etc.), but they are usually much more expensive than simple milling.
Illustration- It is very easy to design square pockets such as the example on the left above, but it is harder to machine them than you would think. An end mill will always leave rounded inside corners, as shown in the right hand version. A smaller endmill can minimize the radius, but it will still be there. Very square corners can be created through other techniques (broaching, EDM, etc.), but this gets pricey.
If you are fitting something inside a pocket, often the corners can be cut away with an endmill so that the sharp corners of the mating part will still fit without jeopardizing alignment.
Illustration- Often, pocket corners can be cut away so that a mating square part can still fit accurately in the pocket.
Watch EM length to diameter.
Endmills work best when they are very rigid. Avoid making deep pockets or inside corners with small radii. Generally, an endmill will cut easily with a length of up about 4 times its diameter (e.g., a ž" endmill cutting a pocket up to an inch deep). Endmills can be cut deeper, sometimes up to 10-15 times the diameter, but this gets progressively harder and more time consuming to do. It these cases, the mill must be "stepped down" the wall of the pocket in very small increments, or run at extremely slow rpm and feed rates. In general it is best to limit pocket depth to as small a multiple of end mill diameter as possible.
Illustration- A deep pocket with small inside corners cut with an extra long endmill is just asking for trouble. Endmills like this will chatter and break easily, and surface finish will be poor.
Illustration- One way to work around the above problem would be to build up the part from three components. This way the pocket could be easily milled from the side and all corners could be kept sharp.
Plan parts for standard EM sizes; make corners larger than EM diameter
As CNC milling has become more common, shops have tended to use standard size endmills for much of the milling work. This is because modern CNC milling machines can mill arcs and curves without regard to endmill diameter. Before CNC, on a manual mill, you would have to choose an endmill with the diameter of the inside corner you wanted to mill, or use a difficult-to-setup rotary table. Now nearly any radius can be milled with a standard size endmill. For efficient material removal shops still need endmills of different sizes, but most shops keep a good supply of only the common sizes. These are usually even fractions of an inch, e.g., 1/16", 3/32", 1/8", 3/16", 1/4", 1/2", 3/4", etc. Metric sizes in even mm increments are common as well.
When designing parts, it is good practice to design inside corners with these endmills in mind. However, when possible don't pick corner radii that are exactly the same as endmill diameters. The reason is that if you bring a .25" diameter endmill into a corner of .25" for example, the endmill has a large portion of its surface area in contact with the work during the finishing pass. This leaves the endmill prone to chatter and poor surface finish. It's better to machine a .300" diameter corner with a smaller endmill, such as a .250" diameter. If you need something close to a .25" diameter corner, choose a slightly bigger radius instead, say .27 or .30. Avoid very small differences, as a .251 corner will effectively machine the same as a .250 corner. You need to add .020 or .030" to lower the surface area contact sufficiently.
Illustration- If the corner of the pocket is has the same radius as the endmill, there is a large area of surface contact on the finishing pass (shown in red). Designing a slightly larger corner than a standard endmill size limits the surface contact and reduces potential chatter.
Don't specify too deep tapped holes
Putting threads in holes (tapping) is usually not a difficult process. But it gets progressively more difficult and expensive as the tapped holes get deeper. Keep in mind that for maximum strength, you only need a hole to be tapped to a depth of 1 to at most 3 times the diameter. Any deeper and the screw will break before the threads pull out. Think about the average commercial nut on a bolt. The thickness of the nut is usually is only 1 to 1.5 times the bolt diameter, because this is all the thickness that is needed. But despite this, we often see prints with tiny holes tapped to extreme depth.
Bear in mind too that the threaded portion of taps is not too long. A 4-40 tap, for example, only has 5/8th of an inch worth of threads on it. If a deeper threaded hole is specified, the tap shank has to be ground back. Because of the depth of the hole there is also an extreme risk of breakage. A very expensive hole to manufacture indeed!
If you need to have a long through hole to clear, for example, a threaded shaft, try to specify threads on only one side of the hole, with a drilled hole from the other end.
Illustration- Long tapped holes (A.) require custom tooling and are expensive to make. Instead, design shorter holes tapped from each side (B.). A through drilled hole, but with short threads from each end is also acceptable (C.). If you need to pass a long fastener or part through the threaded hole, consider back boring as shown in D.
Watch for High walls- EM, toolholder and spindle clearance issues
Another problem area in machining is tool, toolholder and spindle clearance, especially next to high walls or other part features. The end of a standard ER-16 collet chuck, which is often used to hold smaller endmills and drills, is about 1.125 inch in diameter. If you have a pocket next to a high wall, for example, this clearance can present a problem. Sometimes a smaller chuck, like an ER-11, can be used. But this will still have a diameter of about .75", and can only hold quite small tools up to about .25".
You need to bear in mind these tooling clearance issues when designing parts. As always, there are work-arounds, but they are expensive and time consuming.
When possible, design multiple parts or pieces that can be bolted, fit, or welded together to alleviate clearance issues.
Illustration- The photo shown is a typical machine tool spindle with an endmill holder. The accompanying illustration shows typical toldholder and spindle sizes. These numbers are approximate and will vary with the specific machine tool, taper size (#30, #40, #50), etc., but they give you an appreciation of types of clearances required for easy machining.
Limit Machining Risk Factors- Design simple parts
An important but little talked about factor in part cost is the risk involved in the work. For example, if a shop is going to engrave text on a $20,000 mold cavity supplied by the customer, they will charge many times more than if they are asked to engrave the same text on a $10 piece of steel. The reason is risk. The shop cannot afford to make a mistake on the mold, so they will spend much more time testing and proving out the procedures than on the cheap piece of steel. In addition, if they do make a mistake (and mistakes are part of the business of machining) on a costly mold, it will mean a costly insurance claim or worse. As such, the shop charges a premium.
The logic follows if a part gets too valuable. Imagine a part with hundreds of features fashioned out of a huge block of aluminum. The single part might take days to make. If the shop makes a mistake near the end of the project, the part may have to be scrapped at enormous cost. As a result, the shop will charge a premium. If the same part where made of several smaller and less complex parts bolted together, the project would cost less, even though the shop now had to produce a larger number of parts.
As a rule of thumb, it is better to design assemblies out of simple, smaller parts than to try to make a single large complex part.
Illustration- A complex part as shown might be better designed as three separate parts fastened together with shoulder bolts or screws with locating pins. Each of the individual parts then become less risky, clearance problems are avoided, and significant material is saved as well. Often the three simpler parts will be much less expensive to manufacture than a single more complex part.