Homebrew PCB Design for RF Circuits: From Schematic to Working Board

Manhattan style construction and ugly-building got me through my first dozen projects. They work. But when I needed to build ten copies of a 2-meter preamp for our club, or when trace lengths started mattering at 50 MHz, I finally committed to learning proper PCB design. The learning curve was steep — RF layout is unforgiving — but having JLCPCB ship me five perfect boards for $7 changed everything.

Here's what I wish someone had told me before my first dozen failed RF boards.

Choose Your Tool: KiCad Is the Answer

For ham radio PCB design, KiCad is the clear winner. It's free, open-source, runs on everything, and has matured enormously since version 6. The schematic editor is solid, the PCB layout tool handles RF work competently, and the community support is massive.

Alternatives:

• EasyEDA: Browser-based, integrated with LCSC parts library. Good for simple boards, frustrating for RF layout because you have limited control over copper pours and trace geometry.
• Altium/OrCAD: Professional tools. Overkill and expensive for ham projects unless your day job provides a license.
• Eagle: Autodesk killed the free tier's usefulness. Let it rest.

Install KiCad 8 or later. The 3D viewer alone is worth it for checking component clearances.

RF PCB Fundamentals: What Makes RF Different

Ground Planes Are Not Optional

At DC, ground is ground. At RF, ground is a return path, and its geometry affects everything. Every RF PCB should have a continuous, unbroken ground plane on at least one layer. For two-layer boards (which is what most of us are making), that means:

• Top layer: Signal traces, components
• Bottom layer: Solid ground plane, broken only by necessary vias and pads

Every ground connection should have a via directly to the ground plane — short, fat, and close to the component. Not routed across the board to some distant ground point.

Trace Width = Impedance

For most ham HF work below 30 MHz, trace impedance barely matters for short runs. But the moment you cross into VHF or work with matched systems (filters, amplifiers), you need controlled impedance traces.

For a standard 1.6mm FR4 board with 1oz copper and a ground plane on the back:

• 50-ohm microstrip: approximately 2.9mm wide
• 75-ohm microstrip: approximately 1.5mm wide

Use an online microstrip calculator (the one at eeweb.com works well) to dial in exact numbers for your specific board stackup. JLCPCB's standard 2-layer 1.6mm FR4 with 1oz copper has an Er (dielectric constant) of about 4.5.

Keep It Short

At 30 MHz, a wavelength is 10 meters — trace lengths of a few centimeters are electrically insignificant. At 146 MHz, a wavelength is about 2 meters, and a 5cm trace is already 2.5% of a wavelength. At 432 MHz, every centimeter matters.

Rule of thumb: if a trace is longer than 1/20th of a wavelength, treat it as a transmission line and control its impedance.

Schematic Design for RF

Power Supply Decoupling

Every IC and every amplifier stage gets its own decoupling capacitors. Not one cap — multiple:

• 100 nF (0805 MLCC) for general HF/VHF decoupling
• 10 nF for higher frequencies
• 10 µF electrolytic or tantalum for bulk storage

Place these in the schematic right at the power pins. Don't rely on adding them during layout — you'll forget or misplace them.

Signal Flow: Left to Right

Draw your schematic with signal flow going left to right, input to output. For an RF chain: antenna → filter → amplifier → mixer → filter → IF amplifier. This convention maps directly to your physical layout and makes the board easier to route without signal paths crossing.

Label Everything

Use meaningful reference designators and add notes. "C7: 47pF, must be NP0/C0G" is infinitely more useful when you're populating boards six months later than "C7: 47p."

PCB Layout: Where RF Dreams Die

Component Placement Strategy

1. Place connectors first. SMA connectors, power input, control headers — these are mechanically constrained.
2. Place the RF chain linearly. Input on the left, output on the right. Each stage in sequence. Don't wrap the signal path back on itself — that's asking for feedback and oscillation.
3. Group bypass caps with their ICs. A decoupling cap should be within 3mm of its associated power pin.
4. Separate high-level and low-level stages. Your power amplifier output should be physically distant from your sensitive receiver input. Shield walls (grounded rows of vias) help.

The Golden Rules of RF Layout

Rule 1: Never route RF traces on the bottom layer. Keep the bottom ground plane intact. Route everything on top, using the shortest path possible.

Rule 2: Via stitching around RF sections. Place grounded vias every 5-10mm around the perimeter of RF sections and between stages. This creates a via fence that reduces coupling between sections.

Rule 3: Keep traces straight. Right-angle bends create impedance discontinuities. Use 45-degree angles or gentle curves for RF traces.

Rule 4: Pad-to-trace transitions. Where a trace meets a component pad, taper smoothly rather than abruptly changing width.

Rule 5: Crystal and oscillator isolation. Local oscillator circuits radiate. Surround them with via fences and, if possible, add a shield can footprint (those little tin boxes you see on commercial radios).

Handling SMD vs. Through-Hole

Modern RF design lives in the SMD world. 0805-size components are easy to hand-solder and have excellent RF characteristics. Through-hole resistors and capacitors have significant lead inductance that matters above 50 MHz.

For HF-only projects, through-hole is perfectly fine. For VHF and above, use 0805 or 0603 SMD.

My compromise: 0805 for passives (easy to solder by hand), SOT-23/SOT-89 for transistors, SOIC for ICs. Nothing smaller than 0603 unless absolutely necessary.

Manufacturing: Getting Boards Made

JLCPCB Workflow

1. Export Gerbers from KiCad (use the JLCPCB-compatible preset if available)

2. Upload the zip file to jlcpcb.com

3. Options that matter for RF:

   • Layers: 2 (sufficient for most ham projects)
   • PCB thickness: 1.6mm standard
   • Copper weight: 1oz for signal boards, 2oz if carrying significant RF current
   • Surface finish: HASL is fine for prototypes, ENIG (gold) for edge connectors or fine-pitch parts
   • Impedance control: Available for extra cost, worth it for 50-ohm critical traces at VHF+

4. Order 5 boards (minimum quantity, usually $2-7 for small boards)

5. Shipping: Standard takes 2-3 weeks to the US, DHL takes 4-5 days

Design Rule Check (DRC)

Before exporting, run KiCad's DRC with these minimums for JLCPCB:

• Minimum trace width: 0.15mm (but use 0.25mm+ for reliability)
• Minimum clearance: 0.15mm
• Minimum via drill: 0.3mm
• Minimum via annular ring: 0.15mm

For RF traces at controlled impedance, you'll typically be at 2-3mm width anyway, so minimums aren't the constraint.

Real Example: 2-Meter Bandpass Filter

Let me walk through a concrete project: a 3-section hairpin bandpass filter for 144-148 MHz.

Schematic: Three coupled resonators with input/output taps. Coupling is controlled by the spacing between hairpin elements on the PCB itself — no separate coupling capacitors needed.

Layout decisions:

• Board size: 60mm × 30mm (fits in a small tin box)
• Substrate: Standard 1.6mm FR4 (lossy at VHF, but acceptable for a bandpass filter with 1-2 dB insertion loss)
• Resonator trace width: 3mm (50-ohm microstrip)
• Coupling gaps: 1.5mm between resonators (determined by simulation)
• Ground plane: Solid on bottom, stitched vias along edges
• Connectors: SMA edge-launch on both ends

Simulation: I used Qucs-S (free SPICE variant with RF capability) to simulate the filter response before committing to fabrication. The simulated -3 dB bandwidth was 5 MHz centered on 146 MHz. The actual board measured 5.2 MHz — close enough.

Cost: $5.40 for five boards, $6 for SMA connectors. Less than $15 total for five complete filter assemblies.

Common Mistakes I've Made (So You Don't Have To)

Mistake 1: Ground plane gaps under RF traces. I once routed a power trace on the bottom layer that cut right under my IF signal path. Created a slot antenna. Instant oscillation at 45 MHz.

Mistake 2: Ignoring via inductance. A single via has about 1 nH of inductance. At 400 MHz, that's 2.5 ohms of impedance. Multiple parallel vias reduce this. Use 3-4 vias for any RF ground connection at VHF.

Mistake 3: Component footprint errors. Always verify footprints against the actual component datasheet. KiCad's library is good but not perfect. I've had ICs arrive with pin 1 in the wrong corner because I trusted a library footprint without checking.

Mistake 4: Not adding test points. Put SMA footprints or probe-friendly pads at key points in the RF chain. You'll want to measure stage gain, check filter response, and troubleshoot without soldering temporary wires.

Mistake 5: Forgetting thermal relief on ground pads. Large ground planes act as heatsinks. Without thermal relief patterns on ground pads, you'll need a 400°C iron to solder anything. KiCad adds thermal reliefs by default — don't remove them unless you have a specific thermal management reason.

From Board to Box

Once you have a working PCB, put it in a proper enclosure. RF circuits need shielding. Hammond aluminum diecast boxes (like the 1590B series) are perfect. Mount SMA bulkhead connectors for input/output, and bond the PCB ground plane directly to the enclosure using multiple screws and standoffs.

The difference between a PCB sitting on a bench and the same PCB in a proper shielded enclosure is often 20-30 dB of improved isolation between stages. That's the difference between an unstable amplifier and a solid one.

Getting Started

Your first RF PCB project should be simple: a single-band bandpass filter, a crystal oscillator, or an attenuator pad. Something with a defined input and output that you can easily verify with a NanoVNA or oscilloscope.

Don't start with a complete transceiver PCB. Start small, learn the workflow, make your mistakes on $5 boards, and build up from there. The skills transfer — once you've mastered a bandpass filter layout, a multi-stage receiver is just more of the same principles applied sequentially.