We are often asked which CAD package is "best" for sheet metal. The honest answer is that SolidWorks, CATIA and Autodesk Inventor will all produce a correct folded part, a clean flat pattern and a usable drawing in capable hands. The differences that matter in practice are where each tool is normally used, how it stores bend data, how it exchanges files with the rest of a supply chain, and how long it takes a new designer to become productive.
This article compares the three from the point of view of someone who designs folded parts for fabrication every day. Feature names and capabilities change from release to release, so treat the details as a guide and check the current documentation for the version you use.
Who uses what
- SolidWorks is widespread in general machinery, special-purpose equipment, product design and the fabrication shops that supply them. Its sheet metal tools sit inside the normal part environment, which suits mixed parts and small to medium assemblies.
- CATIA, through its Generative Sheetmetal Design workbench in V5 and the equivalent sheet metal apps on the 3DEXPERIENCE platform, is common in aerospace, automotive and other large OEM programmes. Its strengths are very large assemblies, complex surfaces and tight integration with the OEM data management that the rest of the programme runs on.
- Autodesk Inventor is popular in machinery, conveyors and industrial equipment, especially in companies that already use AutoCAD or other Autodesk tools. Its drawing output has a strong AutoCAD and DWG heritage, which many workshops find comfortable.
For a fabricator or a design consultant, the client usually decides the tool. A tier-one aerospace supplier will expect CATIA data; a machine builder may send SolidWorks or Inventor models and expect native files back.
The core sheet metal features
The good news is that the modelling approach is almost identical in all three. You set the material rules, create a base flange or wall from a sketch, add flanges to its edges, then add hems, cuts and formed features before generating the flat pattern.
- Base flange or wall: the first sheet body, from a closed or open sketch. Called Base Flange in SolidWorks, Face or Contour Flange in Inventor, and Wall in CATIA.
- Edge flanges: flanges added along an existing edge, with control of length, angle, relief and whether the length is measured to the inside, outside or mould line.
- Mitre flanges and corner treatment: SolidWorks has a dedicated Miter Flange feature; Inventor and CATIA handle mitred corners through their flange, corner seam and corner relief options.
- Hems: open, closed, teardrop and rolled hems are available in all three, though the exact options differ.
- Lofted transitions: Lofted Bend in SolidWorks, Lofted Flange in Inventor and the Hopper feature in CATIA, used for transitions such as square-to-round ducts and hoppers.
- Unfold and refold: temporarily flattening part of the model to add a cut across a bend, then folding it back. All three support this.
- Forming tools and punches: louvres, dimples, lances and embosses. SolidWorks uses forming tools from its design library, Inventor uses punch tools based on iFeatures, and CATIA provides stamping features plus user-defined stamps.
Sheet metal rules, gauge tables and bend data
This is where most flat pattern errors are born, and it matters far more than the feature list. Every package stores a thickness, a default inside radius and a bend calculation method. The method can be a K-factor, a bend allowance, a bend deduction or a bend table that gives a value for each combination of thickness, radius and angle.
- SolidWorks keeps material settings in sheet metal parameters, optionally driven by gauge tables that list thickness, radius and K-factor or bend allowance by gauge.
- Inventor uses sheet metal rules and unfold rules, held as styles, with options for a linear K-factor, a bend table or a custom equation.
- CATIA sets thickness, default bend radius and K-factor in its sheet metal parameters. The K-factor is a formula that can be edited, and bend values can be driven from design tables.
The principle is the same whichever tool you use. Build one table per material and thickness from your fabricator's actual bend data, store it centrally, and make every model use it. Our article on bend allowance and K-factor explains how to measure the values with a simple test bend.
Flat patterns and DXF export
For most fabrication work the flat pattern DXF is the real deliverable: it goes straight to the laser or punch programming software. All three packages can export a flat pattern to DXF, and SolidWorks and Inventor can also write DWG. What you need to control is what goes into the file.
- Export at 1:1 in millimetres, with arcs and circles as true arcs rather than short line segments where possible.
- Put the cut outline, bend lines, etch marks and text on separate, clearly named layers. A bend line accidentally exported on the cut layer will be cut.
- Decide whether bend lines and bend notes (direction, angle, radius) should be in the DXF at all. Some shops want them, some strip them out.
- Check for open contours, duplicate entities and tiny spline segments before release. Most nesting software dislikes all three.
- Check that formed features export as the shop expects: some tools are punched, so the DXF may need only a centre mark or a tool reference.
Drawings and data exchange
Each package has an integrated drawing module that can place a flat pattern view with bend lines and a bend table, alongside the folded views. SolidWorks and Inventor both produce fabrication drawings quickly for typical machinery parts. Inventor can save drawings in DWG, which suits shops that work in AutoCAD. CATIA's Generative Drafting workbench is thorough and well suited to OEM drawing standards, but it usually takes longer to set up.
Native files carry the full feature history: SLDPRT and SLDASM for SolidWorks, CATPart and CATProduct for CATIA V5, IPT and IAM for Inventor. Between different systems, STEP is the usual neutral format. It transfers the solid geometry well but not the feature tree or the sheet metal definition. When a STEP file arrives, the receiving system has to recognise the bends again, using tools such as SolidWorks' Insert Bends or Convert to Sheet Metal, Inventor's Convert to Sheet Metal, or CATIA's recognition functions. These work well on clean, constant-thickness geometry and less well on parts with tapered sections or modelled clearances.
Side by side
| Aspect | SolidWorks | CATIA (Generative Sheetmetal Design) | Autodesk Inventor |
|---|---|---|---|
| Typical users | General machinery, product design, fabrication shops | Aerospace, automotive, large OEM programmes and their suppliers | Machinery and industrial equipment, Autodesk-based companies |
| Where sheet metal lives | Inside the normal part environment | Dedicated workbench with its own parameters | Dedicated sheet metal part environment |
| Material and bend rules | Sheet metal parameters and gauge tables | Sheet metal parameters, editable K-factor formula, design tables | Sheet metal rules and unfold rules held as styles |
| Lofted transitions | Lofted Bend | Hopper | Lofted Flange |
| Forming features | Forming tools from a library | Stamping features and user stamps | Punch tools (iFeatures) |
| Flat pattern export | DXF or DWG from the flat pattern | DXF from the unfolded part | DXF or DWG from the flat pattern |
| Drawings | Integrated, quick for machinery parts | Generative Drafting, suited to OEM standards | Integrated, DWG output with AutoCAD heritage |
| Learning curve | Generally seen as approachable | Generally seen as the steepest | Approachable, especially for AutoCAD users |
Learning curve and day-to-day productivity
SolidWorks and Inventor are both widely taught and have large user communities, so a new designer can usually model and detail simple folded parts within days. CATIA has a steeper start: the interface, the workbench structure and the data management around it take longer to learn. The payoff comes on large, surface-heavy assemblies and OEM programmes, where its structure is an advantage rather than a burden.
In all three, productivity on sheet metal depends less on the software than on the templates behind it. A good part template with the right rules, a library of standard forming tools, and a drawing template with a flat pattern view and bend table already set up will save more time than any difference between the packages.
Choosing in practice
- Work in the format your client or OEM uses. Converting through STEP loses the sheet metal definition, and someone has to rebuild it.
- If you supply several ecosystems, keep native seats where the volume justifies it and a robust STEP and DXF workflow for the rest.
- Whatever the tool, set up bend data from your fabricator's real tooling before modelling, not after the first part comes back wrong.
- Agree a DXF layer and entity standard with the shop, and check one flat length by hand on every new part family.
- Keep drawing templates with a flat pattern view, bend direction and bend table, so the assumptions are visible on paper.
The right tool is the one that fits your client's ecosystem and your team's skills. A flat pattern is only as accurate as the thickness, inside radius and K-factor or bend table behind it, and those numbers come from the press brake, not from the software brand.
If you would like a second pair of eyes on a flat pattern, a set of gauge tables or a DXF workflow in any of these packages, send us your drawings or models.