Resources
Design guide for fabricated parts
Practical rules of thumb for bent, cut, welded, and machined parts, plus how to prepare files. Following them makes parts easier to build, more accurate, and less expensive.
About these guidelines: These are widely used industry rules of thumb, not guarantees. The right values depend on the material, temper, thickness, and tooling. If a dimension is critical, ask us before you finalize the design. We're happy to review drawings for free.
Before you start: what makes a part easy to quote
The fastest quotes come from complete information. Every request should tell us:
- What it is: a drawing, CAD file, sketch, or photo with key dimensions
- What it's made of: material, grade if known, and thickness
- How many: quantity now, and expected repeat volume
- How it's finished: raw, painted, powder-coated, or galvanized
- When you need it, and whether you'll pick it up or need delivery
Bent and formed sheet metal
In the rules below, T is the material thickness and R is the inside bend radius.
| Feature | Rule of thumb | Why it matters |
|---|---|---|
| Inside bend radius | R ≈ 1 × T for mild steel and stainless; about 0.5 × T for 5052 aluminum; about 2.5 × T for 6061-T6 | Too tight a radius cracks harder materials on the outside of the bend. |
| Minimum flange length | ≥ 4 × T | Short flanges can't be held and formed accurately. |
| Hole to bend line | ≥ 2.5 × T + R | Holes closer than this stretch out of round during bending. |
| Bend relief | Width ≥ 1 × T; depth ≥ R + T | Prevents tearing where a bend runs into an edge. |
| Bend radii | Use the same radius on every bend | Avoids tool changes and extra setup time. |
| Tolerances | Expect roughly ±0.015 in. per bend and about ±1° on angles; they add up across bends | Dimension critical features from one reference edge to limit stack-up. |
Values compiled from Fabcon's sheet metal DFM guide and SendCutSend's bending guide. See sources below.
Cut parts: holes, edges, and profiles
| Feature | Rule of thumb | Why it matters |
|---|---|---|
| Hole diameter | ≥ 1 × T | Smaller holes are hard to cut cleanly and may need drilling. |
| Hole to edge | ≥ 1–1.5 × T (2–3 × T for threaded holes) | Keeps the edge from bulging or tearing. |
| Hole to hole | ≥ 2 × T center to center | Leaves enough material between features. |
| Slots and notches | Width ≥ 1 × T | Narrower features distort or don't cut cleanly. |
| Inside corners | Radius ≥ 0.5 × T | Sharp inside corners concentrate stress and can crack. |
Welded parts
- Use one weld symbol standard. Call out welds with AWS A2.4 symbols (or ISO), but never mix the two on one drawing. Under AWS, a symbol below the reference line means the arrow side; above it means the other side.
- Specify size where strength matters. Give fillet weld size where the design depends on it. For intermittent welds, give both the length and the pitch (center-to-center spacing).
- Don't default to continuous welds. Where strength allows, intermittent (stitch) welds reduce heat, distortion, and cost. Use "weld all around" only when a sealed or continuous joint is truly needed.
- Leave room to weld. Every joint needs torch access. Enclosed corners and tight gaps may need a different joint design.
- Plan for galvanizing. Hollow sections that will be hot-dip galvanized need vent and drain holes so the part can be fully coated, and so trapped moisture doesn't turn to high-pressure steam in the zinc bath.
- Machine after welding when location matters. Welding heat moves material. Critical holes and faces should be finish-machined after welding.
Machined parts
- Tight tolerances only where needed. Apply tight tolerances only where the function requires them. Everything else can use standard tolerances, which costs less.
- Round internal corners. End mills are round, so internal corners will have a radius. Make it at least one-third of the cavity depth.
- Keep cavities shallow. Limit cavity depth to about four times its length. Deeper pockets need special tooling.
- Limit thread depth. Threads longer than about three times the hole diameter rarely add strength. In blind holes, leave unthreaded depth of at least half the diameter at the bottom.
- Mind thin walls. Metal walls thinner than about 0.8 mm (0.03 in.) tend to vibrate and deflect during machining.
File preparation checklist
- DXF for flat and cut parts: drawn at 1:1 scale, units stated, outer profile closed, no title block or dimensions in the cut geometry
- STEP for 3D parts and assemblies, so we can check bends and fit
- PDF drawing with dimensions, tolerances, thread and weld callouts, material, finish, and quantity
- Revision letter or date on every file, so we always build the current version
- No CAD? A clear sketch or photo with key dimensions is a perfectly good place to start
Ten ways to lower the cost of your parts
- Use standard material thicknesses and common grades.
- Use one bend radius throughout a part.
- Reserve tight tolerances for features that need them.
- Keep holes and features away from bends.
- Combine several small parts into one formed part where you can.
- Use stitch welds instead of continuous welds when strength allows.
- Order in quantities that make sense. Setup cost is shared across every part.
- Give us complete information up front so nothing needs re-quoting.
- Allow realistic lead times. Rush work costs more.
- Ask us to review the design before you finalize it.
Sources
Ready for a quote?
Send your files and get a free estimate.