Job search
Hardware Engineering Portfolio: Package a PCB Design for Technical Review
Make a small PCB design inspectable with native KiCad sources and exports, a real rule-check repair, and explicit boundaries around fabrication and powered testing.
A hardware engineering portfolio should let another engineer trace a design from circuit intent to connected pads, inspect the rules you checked, and identify the exact files behind the result. Package editable sources, readable exports, a bill of materials, and a revision-specific review record. A polished board image alone cannot establish those relationships.
For this article, we created an original small RC board and actually ran KiCad 10.0.7 electrical and design-rule checks, including schematic parity. We exported native schematic and layout PDFs, Gerbers, drill data, a netlist, and a BOM. An intentionally incomplete layout failed; its repaired revision passed the configured checks. The board was not manufactured, assembled, powered, or measured. Use recent roles on LandOffer.ai to choose which hardware responsibility your evidence should support.

Define the circuit before showing the board
Start with the intended connection and the assumptions that make it meaningful. Our teaching design has two two-pin connectors, a 1 kΩ series resistor, and a 100 nF shunt capacitor. J1 carries input and ground; J2 carries output and ground. R1 joins the input and output nets, while C1 joins output to ground.
This is a passive RC design exercise. The ideal unloaded cutoff calculation is approximately 1,592 Hz, using the nominal component values. That calculation is not a frequency-response measurement, a SPICE result, or a claim about source and load conditions. Component tolerances, parasitics, and a real connected circuit could change the behavior. No specific physical resistor, capacitor, or connector was qualified.
The current KiCad getting-started guide distinguishes the schematic’s component connections from the board’s physical implementation. That distinction gives a portfolio reviewer useful questions: does the circuit describe the intended function, do the footprints match the intended parts, and do the routed nets implement the circuit? ERC, layout connectivity, and physical part fit address different questions; none should silently stand in for the other two.
Keep those questions beside the project’s purpose. A simple board can show careful evidence handling, but it cannot substitute for experience with high-speed interfaces, power conversion, RF layout, or environmental qualification. Keep the project description tied to the circuit decisions and checks you can show a reviewer.
Worked asset one: a complete, inspectable design packet
The first completed asset is our revision-B review packet. Its board outline measures 30 × 16 mm along the outline centerlines, with two copper layers, four component footprints, eight plated through-hole pads, and three named nets. The routes are on the front copper layer; through-hole pads also appear on the back layer. Two-layer documentation does not imply that we routed signal tracks on both sides.
| Circuit connection | Schematic intent | Layout implementation checked |
|---|---|---|
| J1 pin 1 to R1 pin 1 | Input net | /VIN connection |
| R1 pin 2, C1 pin 1, J2 pin 1 | Filter output node | /OUT connections |
| J1 pin 2, C1 pin 2, J2 pin 2 | Shared return | /GND connections |
We authored the schematic in KiCad’s native format and created the board with the Python bindings bundled with the official application. Standard passive and connector symbols and footprints were copied from that bundled library and attributed as library content. The circuit, placement, routing, and review fixtures are original; the standard library definitions are not.
The footprint choices include a 7.62 mm resistor pitch, a 2.50 mm capacitor pitch, and 2.54 mm connector spacing. The copied footprint geometries define those pitches, but no selected component datasheet was checked against them. Optional standard-library 3D model references remain unbundled; no 3D fit inspection was performed. The BOM retains references, values, footprint names, quantities, and population status. Missing selected manufacturer part numbers remain a fabrication blocker.
The packet keeps the project file, schematic, board, custom rule file, local library tables, and copied symbol and footprint definitions together. KiCad’s project documentation explains that project settings and associated files matter; opening a board alone can lose design information. Keep the rules and local library definitions beside the sources so the reviewer can interpret the saved reports and reopen the same design.
Keep editable sources and readable exports together
Editable files allow deeper investigation. PDFs offer a quick reading route when the reviewer does not have your EDA environment. Our schematic PDF preserves the revision, title, references, values, and named connections. The layout PDF shows the actual native board geometry. We rendered and inspected the actual exported PDFs, including a close view of the schematic. The images represent those native exports, rather than a drawing made to resemble an EDA screenshot.
The real CLI export generated seven Gerber layers: front and back copper, front and back solder mask, front and back silkscreen, and the board outline. It also produced a Gerber job file. Some selected layers have little or no content in this small design. A file’s presence is not a reason to invent features on that layer.
The Excellon drill file and native drill report agree on eight plated holes: four at 0.8 mm and four at 1.0 mm, with no non-plated holes reported. The output uses metric absolute coordinates. The file headers and drill entries were inspected; this was not an independent CAM rendering or a fabricator’s acceptance check.
Treat these saved manufacturing exports as review material. No fabrication order, manufacturer approval, or authorization to build follows from the export operation. That distinction matters when presenting Gerbers in an application. Generating them demonstrates that you can produce an output package from a known source revision. It does not establish that a manufacturer has accepted the stackup, copper weight, annular rings, mask rules, materials, or part fit.
Worked asset two: a failed check and a verified repair
The second completed asset is a revision investigation with actual native check reports and a separate package audit. Revision A deliberately omitted the front-layer ground-return segment between the lower return route and J2 pin 2. The missing segment is 5.46 mm long in the repaired geometry.
The schematic was unchanged in connectivity, so its ERC reported no violations. The board check exposed the physical routing problem. With error, warning, and exclusion severities requested and schematic parity enabled, A returned exit code 5. It reported one unconnected-item error and one dangling-track warning; parity reported no mismatch after the naming correction described below.
Revision B adds the missing return route at the same 0.4 mm track width. The subsequent native DRC returned exit code 0, with no reported geometry violations, unconnected items, or schematic-parity issues. ERC again reported no violations. We retained A and its failed report rather than replacing the evidence with a clean screenshot.
| Saved revision | ERC result | DRC and parity result | Review decision |
|---|---|---|---|
| A, missing J2 return | Zero reported violations | One unconnected error, one dangling warning, zero parity issues | Keep as the diagnosed failure; do not release as B |
| B, return added | Zero reported violations | Zero reported violations, unconnected items, or parity issues | Ready for bounded technical review; fabrication still held |
An earlier setup check also caught a naming mistake: the authored board used VIN, OUT, and GND, while the schematic’s local labels exported as /VIN, /OUT, and /GND. Native parity reported eight warnings. We corrected the board net names and reran parity; we did not suppress those warnings or describe the initial mismatch as a clean result.

That history explains what the repair accomplished. It closed a known layout connection and aligned the schematic and board’s net names. It did not fix an observed physical prototype, establish electrical performance, or qualify a product. No physical prototype failure was measured in this exercise.
Explain the rule set behind a clean report
The exercise used 0.4 mm tracks and a custom minimum copper-clearance rule of 0.25 mm, alongside the saved project constraints. These are authored exercise settings. They were not copied from a confirmed manufacturer capability sheet, and a clean result under them cannot establish manufacturability for an unspecified process.
The KiCad CLI reference documents separate schematic ERC and board DRC commands. It also documents the schematic-parity option and the violation-sensitive exit-code option. We actually used those options. Retain the command, severity selection, and report with the exit code so a reviewer can see which check produced the verdict.
The reports retain KiCad’s default ignored-check lists. Requesting all severities does not enable every ignored check. For example, the saved DRC scope lists missing-courtyard and footprint-filter-related checks among ignored categories. The ERC report likewise retains ignored categories, including simulation-model issues. We did not change those defaults to hide a failure, and we do not call this an exhaustive audit.
Two final fresh-process verification runs reproduced the same normalized result summary while preserving the design-source hashes. Raw reports and exports contain generation timestamps, so their byte hashes can change when regenerated. Record the exact final output files in a manifest rather than promising byte-identical regeneration for timestamped documents.
Test whether the packet contains the reviewed revision
The separate package audit inspected all seven Gerber layer-function headers, metric units, revision-B identifiers, and the eight drill entries. It saved a manifest of the current B source files and exports. This is a completed local consistency check, not a replacement for native DRC or an independent Gerber viewer.
Two negative cases exercised the manifest comparison in memory. Substituting the actual A-board hash into B’s source slot produced a mismatch. Removing the drill-file entry from the candidate hash map produced a missing-file result. The checker rejected both candidate packages without deleting or changing the saved design files.
A hash does not prove which design generated an export. Here the manifest is supported by saved CLI command receipts identifying the input and output paths. Keep both kinds of evidence: the generation record links the operation to a revision, while hashes identify the exact bytes retained afterward.
The resulting decision is to share B for technical review and hold fabrication. Specific part selection, footprint-to-datasheet verification, manufacturer constraints, and an independent manufacturing-file review remain outstanding. The project also has no assembly inspection, continuity measurement, powered bring-up, signal capture, or environmental evidence. A future prototype would require its own identity and test record.
Present the work as a reviewable contribution
Give a reviewer a short route through the packet: circuit intent and assumptions, schematic, layout, failed A report, repaired B report, and the final manifest. Explain what you personally authored and what came from standard libraries. Include a close detail view of the circuit as well as the full PDF, so a large sheet does not hide a small design in an otherwise blank page.
A truthful project description for this exercise is: “Authored a small passive RC PCB review packet, ran native KiCad ERC and DRC with schematic parity, corrected an open return, and retained revision-specific fabrication exports and package checks.” It establishes design-documentation and rule-check work without implying that a physical product has been validated.
As you browse recent hardware-related roles on LandOffer.ai, compare that contribution with the employer’s required ownership. If the opening centers on board bring-up or high-speed measurement, treat those as evidence gaps. A reviewer can assess a narrow, inspectable design more accurately when its completed checks and untested boundaries are visible together.
Sources and Further Reading
- KiCad 10.0 getting-started guide: schematic, footprint, layout, rules, and fabrication workflow.
- KiCad 10.0 CLI reference: actual ERC, DRC, parity, export, and exit-code options used for this exercise.
- KiCad project and library documentation: associated files, configuration locations, and project-local libraries.
- Official KiCad macOS downloads: current 10.0.7 distribution used locally; no system-wide application installation was performed.
- KiCad schematic format and board format: editable source structures and generator provenance.
Documentation and original local design reviewed October 23, 2026. No fabricated board, powered circuit, manufacturing approval, or hiring outcome is claimed.


