SolidWorks Sheet Metal, Weldments, Surface, and Toolbox

SolidWorks · Sheet Metal · Weldments · Surface

Overview

Apart from solid modeling, sheet metal, weldments, and surfaces each have their own distinct workflow and mental model. Sheet metal centers on bends and flat patterns, weldments on frame paths and cut lists, and surfaces on freeform geometry and imported-file repair. The common thread is that you have to start in the right mode from the beginning. Hacking something together as a solid and converting to sheet metal later — or patching surfaces onto a solid — eventually comes back as flat-pattern errors, weld-bead problems, or Knit failures. This guide lays out practical use of Base Flange/Edge Flange/Miter/Hem/Jog/Forming Tool/Flat Pattern, Structural Member/Gusset/End Cap/Weld Bead/Cut List, Boundary/Filled/Knit/Trim/Thicken, and running Toolbox and the Hole Wizard in the real world. For part-modeling fundamentals see 02-part-modeling.md.

1. Sheet Metal — Sheet Metal Design

1.1 Design Principles

The heart of a sheet metal part is that thickness, bend radius, and K-Factor are all linked together, so that the Flat Pattern (unfolded drawing) comes out correctly at the end.

Material thickness: Once set by the first Base Flange, the same thickness applies to the entire part. Avoid Multi-Thickness (mixing different thicknesses in one part) where possible — complexity spirals quickly.
Inside bend radius: Must honor the minimum for the material/thickness. For cold-rolled steel at or below 3mm, an inside radius of 0.76mm (0.030 in) is common industry practice. Go below that and cracks appear, or press-die life is cut short.
K-Factor: The neutral-axis position ratio that determines the unfolded length. Korean shops typically correct sheets per material in the 0.33–0.50 range. Use 0.5 as the default, but for precision sheet metal, fix the value after measured tests at the actual factory.

Note Modeling as a solid first and then switching with Insert → Sheet Metal → Convert to Sheet Metal only works for simple shapes. For complex flange structures, it is safer to start with Base Flange.

1.2 Key Sheet Metal Features

Feature	Role
Base Flange / Tab	The starting point for sheet metal. Assigning thickness to a closed 2D sketch automatically adds `Sheet-Metal` and `Flat-Pattern` history entries.
Edge Flange	Adds a perpendicular flange to an existing edge. Set End Condition and Position (Material Inside/Outside, etc.).
Miter Flange	Adds continuous flanges along multiple edges at once. Useful for box-shaped sheet metal and enclosures.
Hem	Folds an edge over itself. Open / Closed / Tear Drop / Rolled. For safety and stiffness.
Jog	Two bends in one feature, producing a stepped offset flange.
Sketched Bend	Bends along a straight line in a planar sketch.
Corner/Bend Relief	Relieves stress concentration at bent corners. Rectangular / Tear / Obround.
Forming Tool	Stamping features like louvers, embosses, and ribs. Drag-and-drop from the Design Library.
Unfold / Fold	Temporarily unfolds specific bends to apply a Cut-Extrude in the flat state → then Fold back.
Flat Pattern	The full unfolded pattern. Toggle with `Flatten` to check instantly; Bend Lines and Bend Notes can be included on the drawing.

Example menu path: Insert → Sheet Metal → Edge Flange.

Tip When applying a Cut-Extrude to a sheet metal part, check Normal Cut in the PropertyManager. A cut that crosses a bent face is then represented perpendicular to the material thickness in the flat state, matching how laser cutting sees it.

1.3 Gauge Table

Compile the thicknesses, bend radii, and K-Factors your factory actually uses into an Excel .xlsx gauge table and register it with SolidWorks.

Path setup: Tools → Options → System Options → File Locations → Sheet Metal Gauge Table Folder.
When creating a Base Flange, picking a gauge entry from the dropdown applies thickness, radius, and K-Factor in one shot.

Tip Maintaining separate gauge tables by factory and material means that switching vendors on the same part just requires switching the table — the unfolded length is recalculated automatically.

1.4 Sheet Metal Best Practices

One part = one thickness is the default. Reserve Multi-Thickness for exceptional cases.
Edge- and hole-to-edge distance ≥ 2.5 × thickness.
Hole-to-hole distance ≥ 2 × thickness.
Bend line-to-hole distance ≥ 2.5 × thickness + bend radius. Anything closer deforms the hole during bending.
Always include one Flat Pattern view on the drawing. Independently of any isometric assembly view, you need the flat pattern laid out for laser cutting.
Use the Cut List to automatically aggregate material, thickness, and unfolded area, and link it to the BOM.

2. Weldments — Welded Structures

2.1 Basic Workflow

Draw the frame path with a 3D Sketch or by combining multiple 2D Sketches.
Apply profiles (square tube, round bar, H-beam, etc.) to the path with the Structural Member feature.
Clean up the intersections with Trim/Extend.
Add Gussets (reinforcing plates), End Caps (closing plates), and Weld Beads where needed.
A Cut List is generated automatically and provides the basis for BOM and drawing automation.

Menu path: Insert → Weldments → Structural Member.

2.2 Using Structural Member

Supported standards: ANSI, ISO, KS, JIS, GB, DIN.
Types: Square Tube, Rectangular Tube, Pipe, C-Channel, Angle (L), I-Beam, etc.
The Apply Corner Treatment option automatically cleans up intersections. Pick from End Miter, End Butt1, End Butt2.
A single Structural Member feature should use only one profile. If you need to mix profiles, split into separate features.

Tip The profile library lives at <install path>\lang\<language>\weldment profiles. Adding aluminum-profile specs (Bosch Rexroth, Item, Misumi, etc.) dramatically speeds up frame design.

Tip For domestic standards like KS D 3530, .sldlfp files can be downloaded directly from 3DContentCentral, Misumi, or Bosch Rexroth.

2.3 Trim/Extend, Gusset, End Cap, Weld Bead

Trim/Extend: Cleans up Structural Member intersections. Pick the Trimming Boundary as Face, Plane, or Body. The Weld Gap option leaves the required welding clearance.
Gusset: A V-shape reinforcing plate between two members. Polygonal / Triangular shapes, with specified thickness.
End Cap: A flat closing plate at the end of an open profile. Specify thickness and offset.
Weld Bead: A weld bead between two faces. Fillet Weld / Butt Weld. The Cosmetic Weld Bead available since 2011 represents the bead graphically rather than as an actual solid while still aggregating length in the Cut List (saving file size).

2.4 Cut List — BOM Automation

Each Structural Member body is automatically grouped into a Cut List Item. Cut List properties include Length, Angle1, Angle2, Total Length, Description, Material, and Quantity by default, and you can add custom properties for paint codes or surface finishes.

Insert into a drawing: Insert → Tables → Weldment Cut List → pick a drive view → place.

Tip Save Cut List formats as .sldwldtbt for reuse on new drawings.

Tip Group multiple Structural Members and right-click → Create Sub-weldment. The Cut List splits along assembly units, which makes it easy to organize the welding sequence.

3. Surface Modeling

3.1 Why Surface

Freeform geometry (automotive exteriors, appliance housings, water bottles, handpieces, etc.) is hard to express with solid features alone. And when a STEP/IGES file from a supplier fails to convert to a solid due to missing faces or self-intersections, the surface tools are what you use to repair the file. Surface bodies have zero thickness, so you finish either by Knitting → converting to solid or by Thicken (applying thickness).

3.2 Main Surface Commands

Command	Purpose
Extruded/Revolved/Swept/Lofted Surface	The surface counterparts of the solid features.
Boundary Surface	Creates a face from a 4-sided curve network. Bidirectional continuity control (Tangent/Curvature).
Filled Surface	Patches the interior of a closed boundary.
Planar Surface	Closed 2D sketch → planar face.
Offset Surface	Offsets an existing face by a set distance. Also used with distance 0 to extract a face.
Ruled Surface	Extends from an edge at a specified direction/angle.
Knit Surface	Stitches multiple faces into a single Surface Body.
Trim / Untrim Surface	Trim with a tool surface / reverse the trim.
Delete Face	Deletes faces. With Delete and Patch / Delete and Fill options for auto-patching.
Extend Surface	Extends a face.
Thicken	Applies thickness to a face to turn it solid.

3.3 Surface Best Practices

Knit incrementally. Stitching every face in one go makes it hard to find the error source — build up in groups of two or three.
Check Entity (Tools → Check): Diagnoses open edges, minimum curvature radius, short edges, and self-intersections.
Keep Construction Surface for reference only and don't mix it into the final body.
Setting Filled Surface's Boundary Condition to Tangent or higher produces a smooth blend.
Boundary Surface demands a 4-sided curve network, giving cleaner results than Loft. Use Loft to connect simple profiles, and Boundary when you need bidirectional continuity for a blend.

3.4 Surface ↔ Solid Conversion

Solid → Surface: Offset Surface with distance 0, or uncheck Delete and Patch in Delete Face.
Surface → Solid:

Knit all faces into a closed volume and it becomes a solid automatically.
Thicken on one or both sides to add thickness.
Check the Try to form solid option on the Knit feature.

3.5 Repairing Imported Files

If an imported STEP/IGES file fails to convert to a solid, work through the following in order.

Import Diagnostics runs automatically — it attempts auto-fixes for Face Problems / Gap Problems.
Manual repair: patch missing faces with Fill Surface → Knit → Thicken.
Try feature recognition with the FeatureWorks add-in — it rebuilds an editable history tree (success rates are low for complex shapes).

Note Imported files have unit mismatches (mm vs inch), origin-point differences, and tolerances that differ from your local standard. After conversion, verify by measurement (key dimensions) before anything else.

4. Toolbox — Standard Parts Library

4.1 How Toolbox Works

Toolbox is a drag-and-drop library of bolts, nuts, washers, bearings, keys, and gears standardized to ANSI/ISO/KS/JIS/DIN/GB. Included with SolidWorks Professional and above.

4.2 Toolbox Part Management Options

Option	Description	Suitable environment
Create Parts	Creates a new file each time you use a part	PDM environments (enables per-file revision control)
Create Configurations	Many Configurations inside a single file	Small teams, individual work

Note Running Create Configurations in a PDM environment causes frequent Version conflicts as multiple users edit Configurations of the same file concurrently. Recommend Create Parts in PDM environments.

4.3 Toolbox Customization Best Practices

Install Toolbox on a network path so every engineer references the same library.
Right after the initial install, back up the entire folder. Bad edits are hard to reverse.
Create a custom standard: Copy the original ANSI/ISO into a branch called Company_Standard. Never touch the originals.
Keep only frequently used sizes to simplify the UI → fewer selection errors.
Password-protect to prevent tampering with company standards. Note that a lost password cannot be recovered.
Include the year in the install folder name (SOLIDWORKS Data 2024). Prevents conflicts during version upgrades.

4.4 Recovering Toolbox File Errors

Auto-recovery via Toolbox Settings → Database Upgrade.
If swBrowser.sldedb is corrupted, restore from backup.
If the latest Toolbox install conflicts with existing file paths, uninstall and reinstall.

5. Hole Wizard

5.1 Overview

Menu path: Features → Hole Wizard. Generates standard holes per specification and links automatically to the Hole Callout.

Supported types: Counterbore, Countersink, Hole, Straight Tap, Tapered Tap, Legacy Hole, Counterbore Slot, Counterbore Countersink Slot, Slot.

5.2 Best Practices

Specifying hole positions via points in a 2D sketch gives the best editability. Place Center Marks → Smart Dimension.
Advanced Hole: Use when a single hole has different diameters or depths per layer (e.g., upper counterbore + lower tap).
If you need a custom standard, modify the Hole Wizard Standard to your company baseline and deploy it over the network alongside Toolbox.

Tip Hole Wizard holes link 1:1 to drawing Hole Callouts, so putting every hole through the Hole Wizard where possible raises long-term drawing quality. Legacy Holes or plain Cut-Extrude holes yield lower Hole Callout accuracy.

Field Checklist

Sheet metal parts started with a Base Flange
Material thickness, bend radius, and K-Factor match measured factory values
Gauge Tables registered per factory
Bend-line-to-hole distances meet the minimum rule
Flat Pattern drawing view included
Normal Cut option applied on Cut-Extrudes
Weldment path sketches split into sketchable 2D where possible
Structural Member Corner Treatment specified at creation time
Cut List properties (Length/Angle/Material) filled in
After Knitting surfaces, open edges verified with Check Entity
Imported files validated post-Import Diagnostics by re-measuring key dimensions
Toolbox on a network path with backups
Hole Wizard holes and Legacy Holes not mixed