12. Can it be Built?
Designing geometry is half the battle. If a CNC mill can't reach the features, or a 3D printer needs too much support material, the design has failed in practice. Design for Manufacturing (DFM) is the discipline of shaping your CAD geometry around the capabilities and limitations of the process that will produce it. Ignoring DFM leads to parts that are expensive, slow to produce, or simply impossible to make. A bracket that looks perfect on screen might require five-axis machining when a simple redesign could be cut on a three-axis mill. A 3D-printed enclosure might collapse mid-print because its overhangs were never checked. DFM thinking saves cost, shortens lead times, improves yield, and produces stronger, more reliable parts. The earlier you consider manufacturing constraints in the design process, the fewer expensive redesign cycles you will face.
3D Printing (FDM)
Fused Deposition Modeling builds parts layer by layer from thermoplastic filament. Because each layer must be deposited on something beneath it, geometry that hangs in mid-air creates problems. Designing for FDM means understanding how layers, supports, and thermal behavior interact.
- Layer Orientation for Strength: Parts are weakest between layers (the Z-axis). Orient your print so that primary loads run parallel to layers, not perpendicular. A bracket loaded in tension should be printed on its side so layers stack along the force path.
- Overhang Rules (45-Degree Max): Any surface that angles more than 45 degrees from vertical requires support material. Chamfer overhanging edges to 45 degrees to make them self-supporting and avoid messy support removal.
- Support Material: Supports consume extra filament, extend print time, and leave rough surfaces where they attach. Design parts to minimize or eliminate the need for supports by using chamfers, splitting the model, or reorienting the build.
- Minimum Wall Thickness (1.2mm): Walls thinner than about 1.2mm (three perimeter passes with a 0.4mm nozzle) are fragile and may not print reliably. For structural parts, aim for 1.6mm or more.
- Infill Strategies: Infill percentage and pattern (grid, gyroid, triangles) trade print time against strength. For robotics, 25-40% gyroid infill offers a strong balance. Fully solid parts are rarely necessary and waste filament.
- Bridging: Horizontal spans between two supported points can bridge short distances (typically up to 50mm) without supports. Keep bridges short and use cooling fans at full speed to prevent sag.
- Build Plate Adhesion: Large flat surfaces warp as they cool. Use brims (extra perimeters around the base) for adhesion, and avoid placing large flat areas directly on the build plate when possible. Chamfered or rounded first layers reduce peel forces.
CNC Machining
CNC milling removes material from a solid block using rotating cutting tools. The geometry of the tool itself imposes hard constraints on what shapes are possible. Understanding these constraints prevents designs that look great in CAD but are impossible or prohibitively expensive to machine.
- Tool Radius Constraints: A spinning end mill is round, so it cannot produce perfectly sharp internal corners. Every internal corner will have a radius equal to or larger than the tool radius. Design fillets into internal corners from the start.
- Dogbone Fillets: When a mating part requires a sharp internal corner (e.g., a rectangular pocket for a square peg), add "dogbone" or "T-bone" relief cuts at the corners. These small circular cutouts allow the square part to seat fully into the pocket.
- Minimum Pocket Depth: Deep, narrow pockets are difficult to machine because long tools deflect and chatter. Keep the depth-to-width ratio below 4:1 for standard tooling. Deeper pockets require specialty long-reach end mills and slower feed rates.
- Fixturing and Workholding: The part must be clamped securely during machining. Design flat reference surfaces and consider how the part will be held in a vise or fixture. Avoid designs that require flipping the part many times, as each setup adds cost and introduces alignment error.
- 3-Axis vs 5-Axis Capabilities: A 3-axis mill can only approach the workpiece from the top. Undercuts, angled holes, and complex contours on the sides require either multiple setups or a 5-axis machine (which tilts and rotates the tool). Designing for 3-axis saves significant cost.
Laser Cutting
Laser cutting uses a focused beam to cut 2D profiles from flat sheet material (acrylic, plywood, steel, aluminum). It produces extremely precise parts quickly and cheaply, making it a staple of robotics prototyping.
- Kerf Compensation: The laser beam vaporizes a thin strip of material (the kerf, typically 0.1-0.3mm depending on material and laser). If you need a precise slot width, offset your cut lines by half the kerf. Most laser software can apply kerf compensation automatically, but your CAD dimensions should account for it.
- Minimum Feature Size: Very small holes, narrow slots, and thin tabs may not survive the cutting process. As a rule, the minimum feature size should be at least equal to the material thickness. A 3mm-thick sheet should not have features smaller than 3mm.
- Tab Placement for Sheet Parts: When cutting parts from a sheet, small tabs (micro-joints) hold the parts in place so they don't shift or fall through the bed. Place tabs on straight edges away from critical dimensions. Sand or file tabs smooth after removal.
- Nesting Optimization: Arrange multiple parts on a single sheet to minimize wasted material. Orient parts to share cut lines where possible (common-line cutting). Good nesting can reduce material costs by 20-30%.
Sheet Metal
Sheet metal fabrication bends flat metal into 3D shapes using press brakes. Chassis panels, electronics enclosures, and structural brackets are commonly made from sheet metal. Designing for sheet metal requires understanding how material stretches and compresses during bending.
- Bend Radius Rules: Every bend has a minimum inside radius determined by material type and thickness. For mild steel, the minimum bend radius is typically equal to the material thickness. Bending tighter causes cracking on the outside surface.
- K-Factor: When sheet metal bends, the inner surface compresses and the outer surface stretches. The neutral axis (where material neither stretches nor compresses) shifts inward. The K-factor (typically 0.3-0.5) describes this shift and is essential for calculating accurate flat patterns.
- Flat Pattern Development: The flat pattern is the 2D shape that, when bent, produces the final 3D part. CAD tools calculate the flat pattern using bend allowance formulas that incorporate the K-factor, bend angle, and material thickness. Always verify flat patterns before sending to fabrication.
- Relief Cuts: When two bends meet at a corner, the material tears unless you add a relief cut (a small notch or slot) at the intersection. Relief cuts should extend slightly beyond the bend line to prevent distortion.
- Minimum Flange Length: A flange (the portion of material after a bend) must be long enough for the press brake die to grip. The minimum flange length is typically 4 times the material thickness plus the bend radius. Shorter flanges cannot be formed reliably.
Export Formats
Different manufacturing processes require different file formats. Sending the wrong format to a shop wastes time and can introduce errors.
| Format |
Best For |
What It Contains |
Notes |
| STL |
3D Printing |
Triangle mesh (surface only) |
Universal for FDM/SLA slicers. No color, no units metadata. Set resolution to "fine" when exporting. |
| STEP (.stp) |
CNC Shops |
Exact B-rep geometry with tolerances |
Industry standard for exchanging solid models. Preserves curves, surfaces, and feature accuracy. |
| DXF |
Laser Cutting |
2D vector geometry |
Export sketches or flat patterns as DXF. Ensure correct scale (mm vs inches) before sending. |
| 3MF |
Modern 3D Printing |
Mesh + color + materials + units |
Replacement for STL. Includes units, print settings, and multi-material support. Preferred by modern slicers. |
DFM Checklist
Follow this workflow every time you prepare a part for manufacturing.
1
Choose Manufacturing Method
Select the process based on quantity, material, geometry complexity, and budget. One-off prototypes suit 3D printing; production runs favor CNC or injection molding.
2
Design Within Constraints
Apply the specific rules of your chosen process from the start. Do not design freely and hope to fix manufacturability later.
3
Check Minimum Features
Verify that holes, slots, ribs, and thin sections meet the minimum feature sizes for the process. Flag anything below threshold.
4
Verify Wall Thickness
Ensure no walls are thinner than the process minimum. For FDM, 1.2mm. For CNC, depends on material but typically 0.8mm for aluminum.
5
Add Draft Angles if Needed
Injection molding and casting require draft angles (1-3 degrees) on vertical walls so parts release from the mold. CNC and 3D printing generally do not need draft.
6
Run DFM Analysis
Use your CAD tool's built-in DFM analysis or a service like Xometry's instant quote to flag problem areas automatically.
7
Export Correct Format
STL/3MF for 3D printing, STEP for CNC, DXF for laser cutting. Double-check units and resolution settings before exporting.
DFM Tip: Design for the easiest manufacturing method first, then optimize. Start with the simplest process that can produce your part (often 3D printing for prototyping), validate the design, and then adapt it for the final production method (CNC, sheet metal, etc.). This iterative approach catches functional problems early when changes are cheap, and manufacturing problems later when the design is stable.