The problem
Motor controllers in two-wheelers and e-rickshaws are often housed in folded sheet-metal boxes because they are cheap at low volumes and quick to change. A box that looks fine in 3D can still be impossible to fold, crack at bends or fail to seal. Getting bend radius, K-factor, relief and flat pattern right is what makes a design manufacturable at a local fabrication shop.
Objectives
- Package an example controller board, heat sink and cable glands inside a two-piece folded enclosure.
- Model the base and cover with Base Flange, Edge Flange, Hem, Sketched Bend and forming tools.
- Set gauge, bend radius and K-factor from a gauge table and understand their effect on flat length.
- Produce flat patterns, bend lines and drawings with a bend table and export DXF for laser cutting.
- Check stiffness of the cover and fastener access before release.
What you need
Tools and toolboxes
- SOLIDWORKS Sheet Metal — Base Flange/Tab, Edge Flange, Miter Flange, Hem, Sketched Bend, Closed Corner, Corner Relief and Flat Pattern.
- Forming tools (Design Library) — Louvres, lances and embosses for ventilation and stiffening, inserted on the flat or folded body.
- SOLIDWORKS Assembly — Controller board, heat sink and connector placeholders with Interference Detection against the box.
- SOLIDWORKS Drawings — Flat pattern view with bend lines, Bend Table and folded views with hardware callouts.
- SOLIDWORKS Simulation (optional) — A quick static study of the cover with shell elements to check deflection under a hand load.
Software
- SOLIDWORKS 2023 or later
- A DXF viewer
Extra parts and data
- Sheet metal supplier gauge and bend data — Real bend radius and K-factor values from the fabricator make flat patterns match the folded part.
Key concepts
- K-factor
- The position of the neutral axis through the thickness, as a fraction of thickness. It sets how much material a bend consumes, and therefore the flat length.
- Bend relief
- A small cut where a bend meets an unbent edge, so the material tears in a controlled way rather than cracking or bulging.
- Gauge table
- A table of thickness, allowable bend radii and K-factor for a material, so every feature in the part uses consistent, shop-approved values.
- Minimum flange length
- A flange shorter than a few times the thickness cannot be held on a press-brake die, so flanges must meet the shop's minimum.
Step-by-step guide
- 1
Collect packaging data
Define an example controller: a 180 × 120 mm board with an aluminium heat sink 30 mm tall, a three-phase output connector, a battery input pair, a signal connector and two cable glands. Model these as simple blocks in an assembly with their mounting holes. Note the clearances needed: example 5 mm around the board, finger room for connectors and a creepage gap from high-voltage terminals to the metal wall that you take from the electronics designer.
Checkpoint: A placeholder assembly with every component, its mounting holes and a stated clearance envelope.
- 2
Set sheet metal parameters
Choose a material such as 1.2 mm cold-rolled steel or 1.5 mm aluminium, as an example. In the first Base Flange, pick a gauge table or enter thickness, an inside bend radius equal to about the thickness and a K-factor from your fabricator, defaulting to around 0.4 to 0.45 if no data is available. Set auto-relief to rectangular or obround with a ratio of about 0.5 so every new bend gets consistent relief.
Checkpoint: The sheet metal feature in the tree shows the gauge, radius and K-factor, and every later flange inherits them.
- 3
Model the base tray
Sketch the base footprint from the clearance envelope and create a Base Flange. Add Edge Flanges on four sides for the walls, then Closed Corner features so the corners meet with a small gap that can be spot-welded or left open. Add a return flange at the top edge with a Hem or a second Edge Flange to give the cover a landing surface. Keep each flange above the minimum length your shop's press brake can hold.
Checkpoint: The tray flattens without errors and the corner gaps and reliefs are visible in the flat pattern.
- 4
Add mounting and fastener features
Add board standoff holes and heat sink holes matched to the placeholder assembly. For cover screws, use clinch nut or self-clinching standoff holes sized from a supplier catalogue table, keeping them a safe distance from bends so the hole is not distorted. Cut connector and gland holes on the walls with Extruded Cut set to Normal Cut. Check every hole is at least about two to three thicknesses from a bend line.
Checkpoint: A distance check from every hole to the nearest bend meets your rule, recorded in a small table.
- 5
Add ventilation and stiffening
If the controller needs airflow, insert louvre forming tools from the Design Library on the side walls, oriented to shed water downward. Add embosses or a diagonal bead on the large cover to stiffen it. Alternatively, put the heat sink fins outside through a cut-out and seal the box. Decide the IP intent first, because louvres and an IP65 target are not compatible without labyrinths or filters.
Checkpoint: A written choice between a ventilated box and a sealed box with an external heat sink, with the IP intent stated.
- 6
Model the cover and check the assembly
Create the cover as a separate sheet metal part referenced to the tray's outer dimensions, with side flanges that overlap the tray return flange. Add a gasket groove or a formed lip if sealing is needed. Insert the tray, cover, board and fasteners in the assembly, mate them and run Interference Detection. Check that a screwdriver can reach every cover screw and that connectors can be unplugged without removing the board.
Checkpoint: Interference Detection reports no interferences other than intended fastener engagement, and tool access is confirmed with a simple tool body.
- 7
Check cover stiffness
As an optional check, run a static study on the cover in SOLIDWORKS Simulation using shell elements created from the sheet metal body. Fix the screw holes and apply an example 100 N hand load at the centre, which represents someone pressing on the box. Look at deflection rather than stress first, since a cover that flexes too much will break its seal. Compare with a hand calculation for a simply supported plate.
Checkpoint: Cover deflection stays under an example limit of 1 mm, or a stiffening bead is added and the study re-run.
- 8
Produce flat patterns and DXF
Unsuppress Flat Pattern for each part, check bend lines and the grain direction if it matters, and confirm the flat size fits the supplier's sheet. Right-click the flat pattern and export to DXF with bend lines on a separate layer. Measure a flat length and compare it with a hand calculation using bend allowance, so you understand where the number comes from.
Checkpoint: Hand-calculated flat length agrees with the SOLIDWORKS flat pattern within about 0.2 mm for one test bend.
- 9
Make the drawings and report
Create drawings with a folded isometric, orthographic views, a flat pattern view with bend lines and a Bend Table listing direction, angle and radius. Add hardware callouts for clinch nuts, a material and finish note such as powder coating as an example, and general tolerances. Write a report on packaging, the sealing decision, bend parameters and the stiffness check, and if possible get one part folded at a local shop and measured.
Checkpoint: A drawing package and DXF set that a fabricator can quote, and a measured prototype if one was made.
Testing & validation
- Every part flattens without errors and the flat pattern fits the stock sheet.
- Hand bend-allowance calculation matches the software flat length.
- Hole-to-bend distances and minimum flange lengths meet stated rules.
- Interference Detection passes and tool access is shown.
- Cover deflection is under the stated limit in simulation, checked against a plate formula.
Expected results
A two-piece sheet metal controller enclosure with folded and flat models, DXF cutting files, a drawing set with bend tables and hardware callouts, and short packaging, stiffness and sealing notes.
Take it further
- Add a die-cast heat sink lid and compare thermal paths with SOLIDWORKS Flow Simulation.
- Create configurations for a small and a large controller using a design table.
- Fold a prototype and compare measured flange lengths with the model.
Viva and review questions
What does the K-factor control?
Where the neutral axis sits in a bend, which sets how much length the bend takes from the flat blank. Using the wrong K-factor gives a flat pattern that folds to the wrong size.
Why do you need bend relief?
Without it the material at the end of a bend next to an unbent edge has to tear or bulge. A relief cut lets the bend form cleanly and avoids cracks.
Why keep holes away from bend lines?
Material near a bend stretches and distorts, so a hole too close becomes oval or moves. Keeping a few thicknesses away keeps hole size and position reliable.
Learn it at DIYguru
These DIYguru courses and programmes teach what this project needs.