Pogo test tool documentation
Pogo analyses your PCB fabrication output for design-for-test: it reconstructs nets from the copper, finds probe-accessible test points, and produces an optimised pogo-pin plan plus a bed-of-nails vs flying-probe verdict. This guide covers getting your files in, using the analysis view, tuning the probe filters, and exporting the plan.
Preparing your files
Pogo works from your manufacturing output — the same Gerbers, drill file, and placement data your board house receives — not your schematic or design file. That's deliberate: a pad is only probeable where the soldermask leaves copper exposed, so the analysis needs the copper, mask, and drill layers exactly as they'll be fabricated.
Upload a single zip
Upload is a single .zip archive. Loose, individual files are not supported — collect your fab outputs into one zip and drop that. Most EDA tools can output a zip directly, or just compress the export folder.
What goes in the zip
Include everything below. File names and extensions vary by tool — Pogo detects layers by content and by common naming conventions (KiCad, Altium, Protel), so you don't need to rename anything.
| Layer / file | Needed? | What it's for |
|---|---|---|
| Top & bottom copper (Gerber) | Required | Net reconstruction — which pads/traces are connected. |
| Top & bottom soldermask (Gerber) | Required | Which copper is exposed — i.e. probeable. |
| Board outline / Edge.Cuts (Gerber) | Required | Board extent, orientation, and cutouts. |
Drill file (Excellon .drl) | Required | Vias & holes — affects where a probe tip can land. |
| Pick-and-place / position CSV | Recommended | Component footprints & refs — enables component-aware probing and the editing view. |
| Inner copper layers (Gerber) | If present | Multi-layer net continuity. |
| Silkscreen (Gerber) | Optional | Rendered on the board preview only. |
| IPC-D-356 netlist | Optional | Real net names instead of anonymous copper nets. |
Minimum
Copper + soldermask + board outline + drill is enough for the probe-access analysis. Add the pick-and-place CSV to unlock component names, the editing view, and better net grouping.
Export from KiCad
KiCad 7 / 8, from the PCB Editor (Pcbnew):
- Gerbers: File → Plot. Set format Gerber, pick an output folder, and enable the copper, soldermask, edge-cuts (and silkscreen) layers. Click Plot.
- Drill: in the same dialog click Generate Drill Files → format Excellon → Generate Drill File.
- Placement: File → Fabrication Outputs → Component Placement (.pos). Choose CSV, units mm, and separate files off (one file is fine).
- Zip the output folder (all Gerbers + the
.drl+ the.pos/CSV) and drop it into Pogo.
Export from Altium
Altium Designer, from the PCB document (or an Output Job):
- Gerbers: File → Fabrication Outputs → Gerber Files. Units mm/inch either way; include copper, soldermask, mechanical/outline, and silkscreen layers. Generate.
- Drill: File → Fabrication Outputs → NC Drill Files. Keep default Excellon settings. Generate.
- Placement: File → Assembly Outputs → Generates pick and place files. Format CSV, units mm.
- Collect the generated outputs (the
Project Outputsfolder), zip them, and drop the zip into Pogo.
Using a different tool (Eagle, Fusion, Allegro, …)? Any tool that outputs standard RS-274X Gerbers, Excellon drill, and a component position CSV works — zip those three together.
The analysis view
Right after upload, Pogo renders your board and runs the design-for-test pass. You'll see:
- The board preview — copper, mask, drills, and component outlines, top and bottom.
- The net explorer — click any pad to highlight its entire net across layers, so you can see exactly what's connected.
- The testability summary — how many nets are probeable vs unreachable, the board's minimum test-point pitch, and the single- vs double-sided fixture verdict.
- The probe-class matrix — coverage at each standard fixture class (standard, fine, ultra-fine, and flying-probe).
The verdict is a prescriptive report you take back to your EDA tool — Pogo never edits or re-routes your design. Raw Gerbers yield anonymous nets (connected copper); to see real net names, include an IPC-D-356 netlist in the zip.
Editing components
Probe tips must land outside a component's body, on exposed pad copper. Pogo derives each component's keep-out from its footprint, but package data isn't always exact — so you can correct it in the browser and the plan re-optimises live.
Select a component (from the board or the test-point list), then in the Properties panel adjust:
- Dimensions (W × H) — the body footprint the probe must clear.
- Position offset (dX / dY) — nudge the keep-out if the placement is off.
- Rotation offset — correct a mis-rotated package.
When you change a component, Pogo re-runs test-point detection for just the affected side and updates the probe positions and coverage numbers — usually within a second or two. No re-upload needed.
Probe filters & selection
The filters define what fixture you're designing for. Changing them re-scopes the coverage numbers and the exported plan instantly. They're saved per project.
| Filter | What it does |
|---|---|
| Min probe Ø | Smallest pogo-pin tip your fixture can land. Pads that can only accept a smaller tip drop out of scope. Default 0.2 mm (the smallest common pin). |
| Min probe pitch | Minimum centre-to-centre spacing the fixture must respect. Set to off (0) for no constraint — the flying-probe case. A positive value drops conflicting probes and lowers coverage on dense areas. |
| Sides | Which side(s) you'll fixture — top, bottom, or both. Probes on an unselected side leave scope. Deselecting both means "no fixture" (nothing in scope). |
| Hide single-pad nets | Nets with only one accessible endpoint — usually not worth a probe. On by default. |
| Hide orphan nets | Isolated copper with no meaningful connectivity. On by default. |
The probe-class matrix
The matrix shows coverage at four standard fixture classes so you can see the cost/coverage trade-off at a glance:
| Class | Pitch | Min Ø | Meaning |
|---|---|---|---|
| Standard | 2.54 mm | 0.30 mm | Cheapest bed-of-nails; coarse boards. |
| Fine | 1.00 mm | 0.20 mm | The common sweet spot for modern boards. |
| Ultra-fine | 0.50 mm | 0.10 mm | Dense boards; higher fixture cost. |
| Flying-probe | none | 0.10 mm | No fixture NRE, high per-board time — the escape hatch for very dense boards. |
Pogo highlights the cheapest class that still hits high coverage as the recommendation. If you set a filter that doesn't match a standard class, a "current setting" row is added so the matrix always agrees with your headline number.
In-scope nets
"In scope" is the set of nets that count toward coverage after the filters above are applied — probeable, on a selected side, meeting the diameter/pitch limits, and not filtered out as single-pad/orphan. The coverage percentage is always relative to this in-scope set, so it reflects the fixture you're actually designing.
Spot something off?
Pogo's analysis is new and improving quickly. If a net looks mis-classified, a probe lands somewhere it shouldn't, or the coverage doesn't match what you'd expect for your board, tell us — concrete examples are exactly what sharpen the next version.
Send feedback & corrections →Exporting the pogo plan
When the plan looks right, export the optimised probe positions as a CSV to hand to your fixture house. It's generated server-side from your current filters and edits, so it always matches what's on screen.
Each row is one probe placement:
- Reference & net — the component/pad and the net it lands on.
- Side — top or bottom plate.
- X / Y (mm) — position, board-centre-relative.
- Diameter (mm) — the probe tip size that fits.
Note
Exports require a (free) account — sign in with your email and the download starts automatically. The free tier keeps up to three saved projects; larger workflows and batch/API access come with Pro.
Re-export any time you change a filter or a component — the plan re-optimises and the CSV always reflects the current state on screen.