Most sheet metal parts are not one-offs. The same bracket is needed in four lengths, the same enclosure in three sizes, the same cover plate with a different hole pattern for each customer. If every variant is modelled from scratch, every variant is a new chance to get a bend deduction, a hole position or a relief wrong. A parametric model, where a few named values drive the whole part, turns a family of parts into one well-checked model and a table of numbers.
This article covers the ideas behind parametric sheet metal design, a worked example of a bracket family, the modelling habits that keep such models robust, and the pitfalls we see most often.
Design intent first
Design intent is the set of rules the part has to obey when it changes. Before opening the CAD system, write them down in plain words. For a wall bracket they might be: the holes stay 20 mm from each end; the hole pitch never exceeds 100 mm; the upstand height is fixed by the mating part; longer brackets use thicker material. Every one of those rules should end up as a dimension, a relation or an equation in the model, not as something the designer remembers to adjust by hand.
It helps to separate dimensions into two kinds:
- Driving dimensions are the inputs. They are typed in, or come from a table, and they control the geometry. In the bracket example these are length L, height H, depth D and the end distance E.
- Driven dimensions are results. They are calculated from the inputs, either by equations or by the geometry itself. The number of holes n, the pitch P and the flat blank size are all driven.
A good parametric model has as few driving dimensions as possible, each with a clear name and a clear meaning. If changing one value forces you to change three others by hand, the intent has not been captured.
Global variables and equations
All the main CAD packages let you define named global variables and write equations that link them to sketch and feature dimensions. The syntax differs between systems, but the structure is the same: a short list of inputs at the top, then the derived values, then the dimensions that use them. Name the variables after what they mean, such as Length, FlangeHeight or HolePitchMax, not after the sketch they first appeared in.
Worked example: a bracket family
Take a simple L-bracket that fixes a rail to a wall. The upstand is H = 50 mm high, the base flange is D = 40 mm deep, both measured to the outside faces, and the base carries a row of 9 mm clearance holes for M8 fixings. The length L varies from 200 mm to 500 mm. The design rules are:
- End distance E = 20 mm from each end to the first hole centre.
- Maximum hole pitch Pmax = 100 mm, with at least two holes.
- Brackets longer than 300 mm use 3 mm material, shorter ones 2 mm. This is a placeholder design rule for the example, not a structural check: the real thickness should come from a calculation for the actual load.
- Inside bend radius equal to the thickness.
Written as equations, in a neutral syntax that maps easily onto any CAD package:
T = IF(L > 300, 3, 2)
Ri = T
n = MAX(2, INT((L − 2 × E) ÷ Pmax) + 1)
P = (L − 2 × E) ÷ (n − 1)INT rounds down. The MAX guard keeps at least two holes, and so avoids a divide-by-zero in P on short brackets.
The flat blank width follows from the outside dimensions and the bend deduction for one 90° bend, using the K-factor from the bend table for each thickness. Here we use the rule-of-thumb starting values from our bend allowance article: K = 0.45 for 2 mm and K = 0.50 for 3 mm.
BA = (π ÷ 180) × 90 × (Ri + K × T)
BD = 2 × (Ri + T) − BA
Flat width = H + D − BD- 2 mm: BA = 1.571 × (2 + 0.45 × 2) = 1.571 × 2.90 = 4.56 mm; BD = 2 × 4 − 4.56 = 3.44 mm; flat width = 50 + 40 − 3.44 = 86.56 mm.
- 3 mm: BA = 1.571 × (3 + 0.50 × 3) = 1.571 × 4.50 = 7.07 mm; BD = 2 × 6 − 7.07 = 4.93 mm; flat width = 50 + 40 − 4.93 = 85.07 mm.
For L = 400 mm, for example: (400 − 40) ÷ 100 = 3.6, which rounds down to 3, so n = 4 and P = 360 ÷ 3 = 120 mm. The full family follows:
| Configuration | L (mm) | T (mm) | n | P (mm) | Flat blank (mm) |
|---|---|---|---|---|---|
| BRK-200 | 200 | 2 | 2 | 160 | 200 × 86.56 |
| BRK-300 | 300 | 2 | 3 | 130 | 300 × 86.56 |
| BRK-400 | 400 | 3 | 4 | 120 | 400 × 85.07 |
| BRK-500 | 500 | 3 | 5 | 115 | 500 × 85.07 |
Configurations and families of parts
Once the equations work, the variants can live in one file. SolidWorks calls them configurations and can drive them from a design table, Inventor uses iParts or model states, and CATIA uses design tables linked to parameters. Each row becomes a separate part number with its own flat pattern and drawing, while the geometry rules are written only once.
Keep the table small and limited to true inputs. If the table also contains driven values such as n or P, sooner or later someone will edit one by hand and break the link to the rules. Where a value genuinely has to be overridden, give it its own clearly named column so the exception is visible.
Rules for robust models
- Sketch on reference planes and the origin, not on model faces. A face can disappear or change identity when a flange is added or removed; the default planes never do.
- Fully define every sketch, and dimension from datums that match the design intent: hole positions from the ends, not from each other in a chain.
- Keep sketches simple. Leave bend radii to the sheet metal features rather than sketching them as fillets, and avoid sketch fillets on corners that may close up to zero length in a short variant.
- Name the features and variables that matter: Upstand, BaseFlange, FixingHoles, Length. A tree full of Sketch14 and Cut-Extrude7 is hard to debug.
- Use patterns driven by the hole count and pitch variables, not copied features.
- Set the thickness, radius and K-factor through the sheet metal rules or gauge table, linked to the thickness variable, so the bend data changes with the material.
- Flex the model across its full range, smallest and largest variant and anything in between that triggers a rule change, before releasing it.
Linking to the flat pattern and nesting
The real payoff of a parametric sheet metal model is downstream. Each configuration has its own flat pattern, so the DXF for the laser and the blank size for the nest update automatically. Some teams add the flat blank width and length as driven custom properties, so they appear in the bill of materials and can be checked against the sheet size before nesting. A 2500 × 1250 mm sheet, for instance, holds fourteen of the 86.56 mm wide blanks across its 1250 mm width before allowing for kerf and margins, which is easy to check from the property rather than from a drawing.
When the flat pattern feeds production directly, add one check: compare a flat dimension from the model with a hand calculation for at least one variant of each thickness. If both agree, every row in the table can be trusted.
Common pitfalls
- Rounding: forgetting that INT and ROUND behave differently, so the hole count jumps one length too early or too late.
- Edge cases: a short variant where n becomes 1 and the pitch equation divides by zero, or a long one where the pitch drops below the minimum hole spacing.
- Holes too close to a bend: as T and Ri grow, the bend zone widens and can reach a hole that was fine on the thinner variant. Keep a rule of thumb of at least 2 × T plus Ri from hole edge to bend, and confirm it with your fabricator.
- Bend data not following the thickness: a 3 mm configuration still using the 2 mm K-factor.
- Drawings that reference faces lost in some configurations, leaving dangling dimensions.
Summary checklist
- Is the design intent written down and reflected in equations?
- Are driving and driven dimensions clearly separated and named?
- Are sketches on reference planes and fully defined?
- Does the bend data change with the thickness?
- Has the model been flexed across the full range, including rule changes?
- Has one flat length per thickness been checked by hand?
If you would like a second pair of eyes on a parametric model or a part family before it goes to the shop, send us your models and the rules behind them.