Practical everyday DFM guidelines: They truly save time and money Part 1: Geometries

This Blog has spent a lot time talking about the philosophy of Design for Manufacturability (DFM). There are several good books on the subject of DFM and the reader can find in Amazon.com. Just type DFM in the search gadget.  We will nonetheless look at some of the very basic Guidelines to DFM, more specifically at Mechanical / Structural and System design guidelines that I picked up in Design For Manufacturability from David M. Anderson as well as other site on the internet. The Guidelines are separated in 6 groups:

· Geometries (Gn)

· Standard Parts (SPn)

· Material (Mn)

· Assemblies (An)

· Tooling (Tn)

· Geometric Dimensioning and Tolerancing (GD&T)

Geometries

G1: Webbed Machined Parts

Make the inside corner radii of webbed, machined parts such as bulkheads, frames, beams, spars, formers and ribs, normal to the working plane. Avoid closed angle geometries that will require a ramp which add complication and cost to the part; refer to Figure 1.

Figure 1: Webbed Machined Part

G2: Driven Corner Radius

The side of an end mill creates the inside vertical corner radius. To assure tangential smoothness of the inside corner radius with the wall, the  corner radius should be designed with a radius slightly larger than the cutter radius. This is called; driven radius. By designing the corner radius oversize (consult the machinist), thus preventing the end mill smashing into the corner radius, causing undercuts, whiplashes or rope twist finishes. It enables the cutter to drive around the radius, instead of forming it with a size for size and mill cutter radius; refer to Figure 2.

Figure 2: Driven Corner Radius

G3: Fillets versus Chamfer

A Chamfer is typically less expensive than a Fillet. Unless necessary, stick to chamfering which can be done by hand, instead of programming the tool path of a special end mill. Refer to Figure 3. However, on primary structures, the fillet is preferred because of the fatigue cracks that can appear on the shaper change of geometry of a chamfer. Always consult the Stress Function.. 

Figure 3: Chamfer types

G4: Fillets and Corner Radius

Avoid excessive tool changes. Use one minimum radius size for all inside corners of a pocket. Use the same radius size for all corner, and same radius size for all fillets.

G5: Drilled Holes Size

Specify standard drill bit sizes. Unusual hole sizes bring up the cost of manufacturing through purchasing, inventory costs and generate tool proliferation. Always consult the machine shop.

G6: Through Holes

Through holes are preferred over blind holes. This has to do with the fact that a blind hole does not provide good chip exit and cooling.

G7: Reaming

Reaming after drilling is more easily conducted on a through hole.  However, Reaming add cost to the part. Reaming operations are usually required for pin installation or to prevent fatigue cracking in holes.

G8: Drilled surfaces

The entrance and exit surfaces of a drilled hole should be normal to the hole axis. Refer to Figure 4. Holes in the angled surfaces will require a spot-face normal to drill axis to prevent slippage.

 Figure 4: Angled drill Surface

G9: Number of holes and direction

Minimize the number of drilled hole sizes so that tool changes are minimized. Minimize also the number of directions on the part that holes must be drilled from so that setup time is minimized.

 

Figure 5: Surrounding geometry



G11: Tapped holes

Tapped holes cost more to produce than normal drilled holes.

G12: Access to Tools

Always consider the size of the tool required to assemble a component. For wrenches, consider the swing. Refer to figure 6.

Figure 6: Tool Clearances

 

G10: Surrounding geometry to hole

If there is protruding geometry surrounding a drilled hole, there may be risks of touching the geometry either by the drill bit or the drill chuck. Refer to Figure 5.

G11: Tapped holes

Tapped holes cost more to produce than normal drilled holes.

G12: Access to Tools

Always consider the size of the tool required to assemble a component. For wrenches, consider the swing. Refer to figure 6.

 G13: Hole depth

Deep, narrow holes with length to diameter ratios larger than three should be avoided. A drill bit will start to drift sideways at a depth .75 X Drill diameter, i.e.: a .25 Dia. drill with start wandering at .187” deep. The deeper the hole, the more chances you risk of breakage. One way to avoid a deep, narrow hole is to use a stepped entrance.

G14: Boring versus Drilling

Boring is more expensive than drilling, so drilling should be used if possible.

G15: Milling

Minimize the number of set ups required. Milling should be grouped into sets of parallel planes.

G16: Milling depth

Design milled pockets so that the end mill required is limited to 3:1 in length to diameter ratio. Longer end mills are prone to chatter. If long end mills cannot be avoided, clearances needs to be designed into the part. Refer to figure 7.

Figure 7: Milling Pockets

G17: Three-edge corner

When designing a three-edge inside corner, one of the inside edges must have a driven radius (refer to Guideline G2). Relief hole must be incorporated in the design. The hole must be drilled first since drills cannot withstand significant side loading. Refer to Figure 8.

Figure 8: Three Edges Corner

G18: Surface Flatness

For machined surfaces with a high degree of flatness, bosses should be used. The bosses are easier to control, clearly define the areas needing to be flatness controlled, and ensures stable assembly. Large flat surfaces for assembly are more difficult to control and unless highly accurate, therefore very expensive, will be a hyper-static assembly.