Shutdown Circuit
On This Page
Net Classes & Board Setup
Net Classes and Design Rules
A net class is a named group of nets that share the same design rules: minimum trace width, clearance, and via size. KiCad applies these rules during interactive routing and flags violations in the DRC. Without net classes you have a single global rule set, which means every trace is treated the same regardless of its electrical role.
On boards with mixed voltage levels this becomes a problem. In FSAE applications you will commonly have a 12 V GLV system and a high-voltage tractive system on the same board, or at least adjacent connectors. The clearance required between HV and LV copper depends on your insulation coordination analysis, but it is always larger than the standard 0.2 mm signal clearance. Assigning HV nets to a dedicated net class with appropriate clearance means KiCad enforces the separation and the DRC catches any violation before fabrication.
Power rails carrying significant current also need wider traces than signal nets. Assign your power supply nets (12 V, 5 V, GND) to a net class with a minimum trace width appropriate for the expected current. A rough rule of thumb is 0.5 mm per amp for 1 oz copper in free air, but use a trace width calculator for anything carrying more than a couple of amps. Set your signal net class to a narrower default (0.2 mm is typical for low-current digital signals) to keep the board compact.
Net classes are defined in Board Setup under Design Rules. Nets are assigned to classes in the Net Inspector or directly via the netlist. Apply net classes before routing so the constraints are in effect from the first trace.
Multi-Layer PCBs
The course board is two-layer, which covers the vast majority of low-to-medium complexity circuits. Beyond two layers, boards are typically four-layer or more. The two extra layers in a four-layer stackup are usually dedicated to power and ground planes, sandwiched between the signal layers. This gives every signal layer a reference plane directly adjacent to it, which dramatically reduces impedance and EMC problems at higher frequencies.
For FSAE boards where digital signals are running at any meaningful speed, or where noise immunity matters (shutdown circuit sense lines, for instance), a four-layer stackup is worth considering. The cost difference from a two-layer board at low quantities is modest.
Autorouting
Autorouting
KiCad integrates the FreeRouting autorouter via a plugin available through the Plugin and Content Manager. The autorouter takes the unrouted netlist and attempts to complete all connections within the defined design rules. It respects net class constraints — trace widths and clearances — so the class configuration must be correct before running it.
The recommended workflow:
- Route critical nets by hand first: high-current power traces, high-speed signal paths, differential pairs, and any net where the physical path affects circuit behaviour.
- After the critical nets are locked in, run the autorouter on the remainder. Low-priority nets like status LED current-limiting resistors are good candidates — they are not high speed and not high power, so their routing geometry does not matter much.
- Review the autorouted result. Check that trace widths are correct, that vias are placed sensibly, and that the copper pour still fills cleanly. The autorouter may produce suboptimal results — a trace that adds an unnecessary via, or a route that is clearly longer than needed. Fix those by hand.
Component placement quality directly affects autorouter performance. If related components are grouped together so that the nets between them are short, the autorouter has an easier job and produces cleaner results.
Do not start with a fully unrouted board and expect the autorouter to produce a production-quality layout. Use it to handle tedious mechanical connections, not as a substitute for design intent.
Custom Artwork
Custom Silkscreen Artwork
KiCad includes an image converter tool (File > Import > Raster Image, or via the bitmap-to-component converter) that converts a black-and-white image into a silkscreen footprint. The workflow:
- Prepare a black-and-white image of your artwork. Logos with clear outlines convert well; photographs or gradients do not.
- Open the image converter, load the file, and set the output size in millimetres. Measure the space available on your board, lock the aspect ratio, and set the target width.
- Select Front Silkscreen as the output layer. Export to clipboard for a one-off placement, or export to a footprint file if the same artwork will appear on multiple boards or designs.
- Paste into the PCB editor with Ctrl+V. The artwork comes in as a footprint marked "not in schematic" so it is not removed by a netlist update. Hide the auto-generated reference designator in the footprint properties.
- To place the artwork on the back of the board, select the footprint and press F to flip it.
For FSAE teams, putting the team logo on the board is both practical identification and a sign of a finished design. Store the source image file in an artwork/ directory inside your PCB project directory so the source is always with the design.
CAD Import/Export
CAD Export for Mechanical Assembly (STEP)
Once the board layout is complete, export a STEP model so the mechanical team can verify that the board fits the enclosure and that connector openings, LED positions, and component heights are correct.
Go to File > Export > STEP. The STEP file includes the board outline, copper layers, and any 3D models attached to footprints. Before exporting, check that your footprints have 3D models assigned — connectors and ICs are the most important ones for mechanical clearance checking.
Import the STEP file into Onshape, Creo, SolidWorks, or whatever tool the rest of the team uses. Drop it into the enclosure assembly and check for conflicts. Connector bodies protruding through panel cutouts, tall capacitors fouling a lid, or mounting hole misalignment are all easier to catch at this stage than after boards are assembled.
Custom Board Outlines (DXF Import/Export)
Custom Board Outlines from MCAD (DXF Import)
In FSAE and other constrained mechanical environments, the PCB must fit a specific enclosure, bracket, or chassis location. The board shape and mounting hole positions are usually defined in the mechanical CAD model before the PCB design starts. Measuring coordinates by hand is slow and error-prone. Export the board outline directly from MCAD and import it into KiCad.
The process using Onshape (or any other MCAD tool):
- In the MCAD assembly, create a sketch on the face or plane that defines the PCB mounting surface. Draw the board outline and mark the mounting hole centres. Confirm hole diameters — M3 hardware requires a 3.2 mm clearance hole in the PCB.
- Right-click the face or sketch and export as DXF. DXF Release 14 is broadly compatible. Set units to millimetres.
- In KiCad PCB editor, go to File > Import > Graphics. Select the DXF file. Choose Edge.Cuts as the target layer. Set scale to 1 and units to millimetres. Use interactive placement to position the outline.
- The imported geometry comes in as a grouped object. Confirm it looks correct in the 3D view — KiCad renders the board outline as the physical board edge.
Mounting holes imported this way will be in exactly the right position relative to the board outline. Place the mounting hole footprints over the DXF circles on the Edge.Cuts layer, or delete the DXF circles and use proper KiCad mounting hole footprints centred on those coordinates.