DFM for Beginners: 7 Mistakes in CAD Models That Increase Production Costs

DFM (Design for Manufacturing) is a discipline that determines whether a part will be manufactured in three days at a reasonable price or end up in an endless email loop of inquiries, ECO changes, and surcharges. We see the following seven mistakes most often in the pricing process—each one drives up the price, extends the lead time, or both. For each one, we provide a specific rule and guidelines for adjusting the design while it’s still in CAD.

The vast majority of additional costs do not arise during production, but during the design phase—at the moment when the designer draws a feature that can only be manufactured more expensively, more slowly, or not at all. Good DFM means cutting costs out of the geometry before you send it for pricing. The following chapters walk through the seven most costly decisions in CNC and sheet metal fabrication and show how to avoid them.

Tolerance is the most powerful pricing lever in the entire drawing. The transition from a standard machining tolerance (ISO 2768-m, typically ±0.1–0.2 mm depending on the dimension) to ±0.01 mm does not simply mean “a little more precise” — it means a different machine, different tools, slower feed rates, in-process measurements, and often inspection on a CMM. This will affect the unit price by tens of percent. A common mistake is a general note stating “all dimensions ±0.05” across the entire drawing, even though only five dimensions are critical.

Apply functional tolerances: use tight tolerances only where parts fit together or seal, and use the general tolerances specified in the standard for the rest. Specify the fit for a bearing or pin using a fit system (e.g., H7/g6), not ±0.005 on each part separately. And distinguish between dimensional tolerance and geometric tolerance (flatness, concentricity)—the latter tends to be more expensive and is often what actually ensures proper function.

A milling cutter is a cylinder—therefore, a perfectly sharp inner corner does not exist. If you set the radius to 0 in the corner of a pocket in CAD, the machining process will round it anyway to the tool’s radius; or (if you insist on a sharp corner), they’ll have to resort to EDM or wire cutting, which multiplies both the cost and the lead time. Depth is also critical: the deeper the pocket, the larger (and more expensive) the tool must be to prevent it from breaking.

• Inner corner radius ≥ (tool radius) — in practice, design the radius to be at least 1/3 of the pocket depth so that the corner can be milled with a suitable tool
• Pocket depth up to ~4× the tool diameter; deeper = slender tool, lower feed rates, risk of vibration
• At the bottom of the pocket, allow for a small radius at the face of the end mill—a “sharp” edge at the bottom is also costly
• If you need a truly sharp inside corner, add a dog-bone or T-bone cut instead of requesting EDM

A thin wall vibrates and “warps” during machining—resulting in a poor surface finish, missed tolerances, and the need for fine finishing passes. For metals, do not go below ~0.8 mm (aluminum) or ~0.5 mm (steel) without consulting an expert; large, thin surfaces also tend to warp once internal stress is released. With sheet metal, the logic is the opposite, but just as unforgiving: sheet metal that is too thin for a large enclosure will sag and be difficult to handle.

The solution is a design one, not a manufacturing one: add a rib, a ribbed section, or a flange to give the surface rigidity, rather than simply increasing the thickness. For sheet metal covers, a perimeter flange and a few embossed lines are often enough to turn a “sheet” into a rigid part.

For holes, several independent constraints must be considered. Diameters under ~1 mm and deep holes (depth-to-diameter ratio over ~5:1) require special tools and core drilling with flushing—a slow and expensive process. A hole too close to the edge will “tear” or deform during machining; keep the distance between the hole center and the edge at least 1.5 times the diameter. As for threads: prefer through threads to blind threads; for blind threads, keep in mind that the thread will never reach the bottom of the hole (leave a run-out of 1.5–2 pitches).

• Use standard drill/tap sizes (M3, M4, M5…) — a non-standard hole requires a non-standard tool
• Depth-to-diameter ratio up to ~5:1 at no extra charge; for deeper holes, use a through-hole or machine from both sides
• Distance from the center of the hole to the edge ≥ 1.5× the diameter
• Blind thread: thread depth ≤ 2–3× the diameter; a deeper thread serves no functional purpose and only increases the cost

The most common mistake with sheet metal is assuming a “sharp” bend. A press brake creates an inner radius roughly equal to the sheet metal’s thickness (or even smaller for soft materials); if you draw an R0 in the model, production will still use the technologically feasible radius, and the dimensions will shift. The second pitfall involves holes and cutouts near a bend—if they lie within the deformation zone, the bend will pull them in and deform them.

• Inner bending radius ≈ sheet thickness (t); smaller radii are possible only by agreement and with suitable material
• Distance from the edge of the hole to the bend ≥ 2.5–3× t + radius (otherwise the hole will stretch into an oval)
• The minimum length of the bend arm is ≈ 4× t so that the press can grip it at all
• Take springback into account—the exact angle is a matter of setup, not CAD

The most expensive detail in a CAD model is the one you added without knowing why. DFM is the discipline of asking about every element: “I’m paying for you, so what do you do?”

Materials are often specified out of habit rather than for functional reasons. Using 1.4404 stainless steel where 6082 aluminum would suffice results in poorer machinability, longer machining times, and more expensive tools—and offers no benefit for a part that will never be exposed to a corrosive environment. Similarly, for surface finishes: “ground to Ra 0.8 over the entire part” is expensive and unnecessary when only one contact surface is functional. Specify surface roughness and finish selectively and state the purpose (sealing, appearance, corrosion resistance) so that the manufacturer can propose a less expensive equivalent.

A model without drawings is the most common cause of bid delays. A 3D model contains the geometry, but it does not specify which surfaces are functional, where the measurement reference is, what the critical tolerance is, or how the part is inspected. Without this information, the manufacturer either has to guess (and play it safe by setting a higher price) or ask for clarification—and the quote is delayed. Include a 2D drawing with the coordinate system, critical dimensions, and necessary GD&T; leave non-critical dimensions with general tolerances.

• Define 3 bases (A/B/C) — they will define the coaxiality, perpendicularity, and position of the holes
• Highlight the critical dimensions; cover the rest with a note on general tolerance (ISO 2768)
• Specify the material, condition (e.g., T6), surface finish, and edge requirements (deburring, chamfering)
• Check the units and scale—incorrectly set mm/in or scale settings are a common cause of scrap

Summary: DFM isn’t about designing worse, but about designing more thoughtfully. Before you send your model for a quote, go through these seven points as a checklist—for each element, ask yourself whether its cost is justified by its function. You’ll save on iterations, shorten the turnaround time, and the quote you receive will be lower and free of uncertainties.