Simple 5V

5 V supply + op-amp signal buffer

Open Simple_5V.kicad_pro in KiCad 10. The project contains the complete schematic and a 38 × 38 mm routed PCB. Seven electronic components; six direct-solder wire terminals. No custom symbols or footprint libraries.

Use

• J1: +8–9 V DC input. J2: input ground. Use a regulated DC source and correct polarity.
• J3: approximately +5 V output, up to 50 mA external load at room temperature without a heatsink. J4: common ground.
• J5: signal input, referenced to common ground. J6: buffered output. Connect the signal source ground to J2/J4.
• Recommended signal range 0.1–4.5 V, DC or low-frequency signals up to about 10 kHz, output load 10 kΩ or higher, and short wiring with modest capacitance (target ≤100 pF). R2 introduces about 1% attenuation into 10 kΩ. Do not drive a speaker, motor, or long capacitive cable from J6. Keep J5 within the powered supply rails; connect a source or ground J5 rather than leaving it floating.
• This is a voltage follower: output follows input, while the op-amp reduces loading on the source. It does not increase voltage amplitude.

Parts / assembly

C1–C3 are nonpolar. Their voltage rating and dielectric cannot be determined from the photos; select known-rated stock. C1 should retain ≥330 nF at 9 V DC bias. R1 supplies roughly 6 mA minimum regulator load and dissipates approximately 31 mW. At 9 V input with a 50 mA external load, regulator dissipation is approximately 0.28 W including quiescent current. This is deliberately a low-current design, not a 1.5 A supply.

U1: with its marked face toward you and leads down, pins left-to-right are 1 IN, 2 GND, 3 OUT; metal tab is GND. Match the body/tab outline on the top assembly drawing.

U2: match the DIP notch and square pin-1 pad. 1 NC; 2 inverting input; 3 noninverting input; 4 GND; 5 NC; 6 output; 7 +5 V; 8 CS tied to GND (enabled). Pins 2 and 6 are connected before the 100 Ω output resistor. Pins 1 and 5 remain electrically unconnected.

The installed KiCad library has no MCP6273 symbol. The existing Amplifier_Operational:MCP603-xP symbol has the same verified eight-pin functions and is used with the actual value MCP6273-E/P and its correct datasheet. Do not interpret the library identifier as the BOM part number.

Single-sided construction

All traces, SMD pads, and the filled ground plane are on B.Cu; there are zero vias and zero jumpers. Use the supplied Fabrication files, which contain only one copper layer. Standard KiCad through-hole footprints retain front pad annuli in the editor; do not manufacture F.Cu. A conventional single-sided, unplated-hole board is suitable; solder all leads from the bottom. The front copper annuli are not required for any connection. The Gerber job metadata is omitted to avoid implying a two-copper-layer stackup.

Verification and assumptions

• ERC: 0 errors, 0 warnings; report included.
• KiCad GUI DRC with ground refill: 0 violations, 0 unconnected pads; report included. The default ignored checks are listed in that report; no individual violations were excluded.
• Independent exported-netlist comparison: every connected schematic pin matches the PCB net. No vias; every track on B.Cu. KiCad's GUI schematic-parity tab was not run; this comparison verified electrical equivalence separately.
• Board and schematic visually inspected. Board saved with filled ground copper.
• Bin labels identify U1/U2; the photos do not establish the individual IC body markings conclusively. Confirm L7805CV and MCP6273-E/P on the selected parts before fitting. No substitute pinout is assumed.
• No physical prototype or component measurements were performed. Capacitor stock ratings and exact resistor values are assembly assumptions. No reverse-polarity protection is included; do not back-power J3/J6.

Sources

Pinouts, operating ranges, application decoupling and minimum-load requirements were checked against the ST L78 datasheet and Microchip MCP6271/1R/2/3/4/5 datasheet. Symbol and footprint geometry were checked against the installed standard KiCad 10 libraries.

Repository organization

Project files

• AIPCB.kicad_pro
• Simple_5V.kicad_pro

Open the appropriate .kicad_pro file in KiCad; .pro entries are legacy projects. Keep schematics, boards, local libraries, library tables, and supporting files together. Hierarchical schematic sheets are part of their parent design.

Git workflow

Automatic backups, recovery files, editor state, and filesystem metadata are ignored. Existing fabrication outputs and local component libraries are retained. For existing repositories, ignore rules do not automatically untrack previously committed files.

Review and save a meaningful design revision with:

git status --short
git diff
git add -- <changed-files>
git commit -m "Describe the design change"

Documentation images

Add a clear 3D board view at docs/images/board-3d.png and, optionally, a PCB layout view at docs/images/pcb-layout.png. A schematic PDF is useful for reading circuit details. Once present, embed an image in this README with ![Board 3D view](docs/images/board-3d.png). For folders with several designs, use a separate named image for each.

Design notes to complete

Describe purpose, power and connectors, revision status, assembly requirements, and what has been physically tested. The repository setup does not establish electrical correctness or manufacturing readiness.

Repository portability notes

• Computer-specific library path: fp-lib-table → /Applications/KiCad/KiCad.app/Contents/SharedSupport/footprints/Capacitor_SMD.pretty.
• Computer-specific library path: fp-lib-table → /Applications/KiCad/KiCad.app/Contents/SharedSupport/footprints/Connector_Wire.pretty.
• Computer-specific library path: fp-lib-table → /Applications/KiCad/KiCad.app/Contents/SharedSupport/footprints/Package_DIP.pretty.
• Computer-specific library path: fp-lib-table → /Applications/KiCad/KiCad.app/Contents/SharedSupport/footprints/Package_TO_SOT_THT.pretty.
• Computer-specific library path: fp-lib-table → /Applications/KiCad/KiCad.app/Contents/SharedSupport/footprints/Resistor_SMD.pretty.
• Computer-specific library path: sym-lib-table → /Applications/KiCad/KiCad.app/Contents/SharedSupport/symbols/Amplifier_Operational.kicad_sym.
• Computer-specific library path: sym-lib-table → /Applications/KiCad/KiCad.app/Contents/SharedSupport/symbols/Connector_Generic.kicad_sym.
• Computer-specific library path: sym-lib-table → /Applications/KiCad/KiCad.app/Contents/SharedSupport/symbols/Device.kicad_sym.
• Computer-specific library path: sym-lib-table → /Applications/KiCad/KiCad.app/Contents/SharedSupport/symbols/Regulator_Linear.kicad_sym.
• Computer-specific library path: sym-lib-table → /Applications/KiCad/KiCad.app/Contents/SharedSupport/symbols/power.kicad_sym.