Task-oriented documentation for ZofzPCB. New to ZofzPCB? Start with the Quick-start Guide to get your first board loaded in minutes.

Eight articles covering every way to get your design files into ZofzPCB.
Feature overview →The fastest way to load a Gerber project. ZofzPCB scans your folder, identifies your files, and proposes the stackup automatically.
You have a folder containing your Gerber files (copper layers, drill files, board outline) and want to get into the 3D view as quickly as possible.

ZofzPCB identifies files by matching their names and extensions against a set of naming rules stored in %APPDATA%\ZofzPCB\CAM_Load_Rules.txt. This file contains rules for common CAD tool conventions including KiCad, Eagle, Altium, and Protel. If your files use non-standard naming, the autoloader may not detect all layers correctly: use Manual Compose instead.
Full manual control over file assignment and layer order. Use this when Auto Load does not correctly identify your files.
Auto Load produced incorrect or incomplete layer assignments, or your project uses a non-standard naming convention.

| Column | Description |
|---|---|
| Name | Filename if a Gerber file is assigned to this layer |
| Type | Layer type: copper, solder mask, silkscreen, core, pre-preg etc. |
| Par | Additional parameters: polarity, special settings |
| Thick | Layer thickness. For copper, enter in oz (oz per square foot) |
| Type | Description |
|---|---|
| Non-plated | Plain, non-conductive hole |
| Plated | Conductive barrel: standard through-hole |
| Filed | Conductive barrel, metal filled or capped |
| µVia↓ | Blind via: metalized from bottom |
| µVia↑ | Blind via: metalized from top |
| µVia↓ Filed | Blind via, filled, metalized from bottom |
| µVia↑ Filed | Blind via, filled, metalized from top |
ODB++ loads as a single file, no stackup configuration needed.
Your CAD tool exports ODB++ format. ODB++ is a self-contained format that includes layer data, netlist, component information, and stackup in a single file or compressed folder.
.gz compression. ZofzPCB reads them directly: you do not need to extract them first.IPC-2581 is a single XML file containing everything ZofzPCB needs, including stackup, netlist, and component data.
Your CAD tool exports IPC-2581 format. It is the most complete single-file format supported by ZofzPCB: layer data, stackup, netlist, BOM, and component information in one structured file.
.xml) and select it



Because IPC-2581 carries complete design information in a single file, loading is simpler and the 3D model is typically more accurate than a Gerber set. If your CAD tool supports it, use it.
ZofzPCB can read Gerber sets, .camset files, and IPC-2581 files directly from ZIP archives without extracting them first.
Your design files are delivered or stored as a ZIP archive.
| Format | ZIP supported? |
|---|---|
| Gerber file set | Yes. Treated as a folder |
| .camset configuration file | Yes. Read and save |
| IPC-2581 | Yes. Extracted automatically |
| .zofzproj rendered project | No. Uses its own LZMA compression |
| ODB++ | No. May use its own gz compression |
Autoload recognizes files by their names. If your CAD tool uses names ZofzPCB doesn't know, add your own rules:
Edit Rules in the autoload panel. This opens CAM_Load_Rules.txt (in %APPDATA%\ZofzPCB); the file explains its format at the top.Drill_PTH *\*.drl for drill files in a subfolder.Drill_PTH *_pth_drill.gbr, Drill_NPTH *_npth_drill.gbr, BoardOutline *_profile.gbr. P-CAD: .tps/.bps paste, .gto/.gbo silkscreen, .tms/.bms solder mask, .top/.bot/.inN copper, .gko outline, .ncd plated drills.Reset Rules on the Gerber Load dialog restores the rules that ship with ZofzPCB.Gerber and drill files are often exported with different offsets, so ZofzPCB shifts the drill data onto the pads automatically (Auto-Offset, on by default). The Drill / Pad Fit Warning means only a few drill holes matched pads. If your files are exported correctly, turn Auto-Offset off: right-click Drill Plates, Setup Excellon Format.
ZofzPCB builds the board shape from the board outline layer. For a panel, set how the outline is interpreted in the Board Outline setup; ZofzPCB remembers the setting. Closed shapes on the outline layer, such as the letters “P” or “0”, create extra outlines, so keep text off that layer.
Seven articles covering stackup setup: the critical step between loading your files and rendering your board.
Feature overview →Before ZofzPCB renders your board it proposes a stackup. This is your moment to review and complete it.
Every time you load a Gerber set, before pressing Read & Render.
Gerber files carry copper artwork but not stackup parameters. Enter these manually for accurate DFM validation.

After loading a Gerber set, when you want full stackup parameters for DFM validation or accurate STEP export.
| Parameter | Description |
|---|---|
| Layer type | Core or pre-preg for dielectric layers |
| Thickness | Layer thickness in millimetres |
| Copper weight | Typically 1oz, 2oz, or 0.5oz per copper layer |
| Material | FR4, Rogers, polyimide, or other substrate |
1oz)Configure drill files to correctly represent through-holes, blind vias, buried vias, and µVias.

When your board uses multiple drill files, non-standard via types, or blind and buried vias.
| Column | Description |
|---|---|
| Name | Filename of the drill file |
| From/To | Start and end copper layer numbers |
| Type | Via type: see table below |
| Type | Description |
|---|---|
| Non-plated | Plain, non-conductive hole |
| Plated | Conductive barrel: standard through-hole |
| Filed | Conductive barrel, metal filled or capped |
| µVia↓ | Blind via: metalized from bottom |
| µVia↑ | Blind via: metalized from top |
| µVia↓ Filed | Blind via, filled, metalized from bottom |
| µVia↑ Filed | Blind via, filled, metalized from top |
The board outline defines the physical boundary of the PCB. ZofzPCB needs it to correctly render and clip the board.


| Option | Description |
|---|---|
| Accept all detected loops | All detected outlines define multiple PCBs |
| Auto recognition | Finds a division line between the PCB and drawing text |
| Take the greatest loop | Assumes the largest shape is the PCB |
| Take 2–10 greatest loops | For boards with multiple outlines or cutouts |


Save your stackup configuration so you don't have to re-enter settings when you regenerate Gerber files.
Layer assignments and order · Layer types, thicknesses, and materials · Drill plate assignments · IPC-356 and BOM filenames · Colour settings · Gerber/drill/IPC-356 file format parameters · Board outline settings · Camera positions · Component model adjustments and Body Builder models
Save the complete rendered board, including all component models and settings, as a single project file.
| .camset | .zofzproj | |
|---|---|---|
| Saves rendered board | No | Yes |
| Saves configuration | Yes | Yes |
| File size | Small | Larger |
| Use case | Re-load after Gerber regeneration | Save complete session |
Each drill plate has a from/to span. Right-click the from/to column to set it: top (copper 1), btm (last copper), thru (top to bottom) or the copper numbers of an inner span. Autoload can read the span from the file name: a mask like *_*_drill_N_N.gbr uses the two numbers as the from and to copper layers.
Ten articles covering navigation, layer control, cross-sections, and rendering options.
Feature overview →Turn individual layers on and off to focus on what matters.

The right panel contains checkboxes for every layer in your stackup, plus:
Separate the layers of your board to inspect the stackup from the inside.
Removes layers from the top down, like peeling back the board one layer at a time.
Separates all layers vertically, creating a gap between each layer.
The Hollow checkbox makes dielectric layers transparent, revealing the copper inside without physically separating layers.
Cut through your board at any angle to inspect inner layers, via stacks, and copper connections.

The first Delete sets the angle, the second moves the cut. The view updates in real time. Alternatively, right-click and choose Set Measurement Target → Cross-cut.
Change how your board looks by applying colour presets or customising individual layer colours.


Go to View → Color Presets to select a built-in colour scheme.
Colour settings are saved in your .camset and .zofzproj files.
Fine-tune the 3D rendering appearance: wireframe, subsampling, thick layers, camera projection, and lighting.




| Option | Description |
|---|---|
| Wireframe | Show board as wireframe outline only |
| SubSampling | Reduce render quality for better performance |
| Thick layers | Exaggerate layer thickness for clearer visualisation |
| Camera FOV | Adjust field of view |
| Net selection effects | Visual style for highlighted nets |
| Render effects | Post-processing effects on the 3D view |
| Light | Adjust light direction and intensity |
Capture high-resolution images of your board and use autopilot for automated rotation.


Screenshots capture the exact view: colour scheme, layer visibility, cross-sections, and any measurements or annotations currently visible.
Rotates the board automatically in a smooth continuous movement, useful for presentation sequences.
Click a layer's name (right of its checkbox) to show only that layer. Reset returns to the full board. In Spread mode, tick Single to peel layer by layer.
Hold Ctrl while turning the mouse wheel to zoom more slowly, Shift to zoom faster; this also works on the numeric keypad. All controls: Help → Mouse & Keyboard. A printable shortcut list (PDF) is in the Help menu.
In the color picker, the hex field takes 8 digits. For entries with an Opaque slider, put FF in front of the color; for entries without one (Plated H. In/Out, Edge Out, Background), put 00 in front. The colors we use for screenshots and cross-sections:
| Entry | Value |
|---|---|
| Copper | FFCB7B48 |
| Plated H. | 00D0D3D2 |
| Volume | FF6E7672 |
| Edge In | FF5F786C |
| Edge Out | 008FA69A |
| Background | 001B2B16 |
Six articles covering 3D component models, from automatic generation to custom building.
Feature overview → Background: IPC-356 and 3D components →ZofzPCB automatically generates 3D component models from your BOM and PCB footprints, no library setup required.
The auto-modeler reads your BOM and IPC-356 netlist, then uses the PCB footprint geometry to generate a 3D model for each component.
| Variant | Description |
|---|---|
| Extruded | Free: simplified block-shaped models from the footprint outline |
| Realistic | Free: more detailed models with pin geometry and body shape |


Browse and manage the 3D component model library for your project.

For each component you can:
Adjustments are saved in .camset and .zofzproj files and applied every time you reload the project.







Create precise custom 3D models for components the auto-modeler cannot fully capture.
The Body Builder is a geometric editor where you define:
Models are saved to your project's component library and reusable across all boards.











How ZofzPCB uses your netlist and BOM together to place component models, and what to do when matching fails.




ZofzPCB uses the IPC-356 netlist to identify component positions and pin connections, then matches these to BOM entries using the component reference designator (e.g. U1, C3, R12).
The IPC-356 format limits component reference names to 6 characters. Longer references (e.g. BTN_DOWN) are truncated (e.g. BTN_DN), causing a mismatch.
Go to Netlist → Errors to see components that could not be matched.
Right-click the component, then Component → Model. To change many parts at once, load a CSV BOM with your Gerbers. When ZofzPCB recognizes its columns, you can apply a model to all components with the same footprint or the same name. Check the result in the Components List (main menu: Components): it shows footprint and component name columns when the BOM was recognized.
Up and Down move between entries, and Enter finishes editing and jumps to the next line.ZofzPCB detects components from the IPC-356 netlist. Pads that aren't connected to a net can be missing from the export, and then the component may not appear. Export an IPC-356 file that includes all pads, and a BOM with one reference designator per line. For an empty footprint, right-click it and pick a model from the Hidden Component List.
Eight articles covering design inspection: components, nets, vias, holes, and schematic crosscheck.
Feature overview →Find, highlight, and zoom to any component on your board instantly.



Trace any signal through your entire board in 3D, across all layers simultaneously.


Inspect every hole and via on your board, including clearances, annular rings, and cut-through stack views.

For any selected via, the hole browser shows a cross-section of the via stack, displaying all the copper layers it connects through.
Verify that the copper connections on your board match the IPC-356 netlist, and identify any discrepancies.
Navigate between your PCB in ZofzPCB and your schematic editor simultaneously.

| Mode | Description |
|---|---|
| Disabled | Commands not sent; P and N keys act for selection |
| CPN: Comp Pad Net | C, P, N keys send crosscheck commands |
| C: cross-check | C key sends crosscheck; P and N keys act for selection |
| On Hover | Mouse hover triggers crosscheck |
Components → Display only → TH or SMT. A black square in the Components checkbox in the right panel means a filter is active; click the checkbox to show all components again.
File → Export → Netlist CSV writes one line per pad with these columns: component, pin, net, SMD/THT, side, x, y. The number of lines minus one is the total pad count.
The Holes List groups all holes by type, diameter and layer span and shows how many there are. Select an entry to highlight those holes on the board; the status bar shows the count for the selected tool and for all holes. For each hole, the list shows annular ring and clearance per layer. Press H to jump between the board and the list.
Four articles covering measurements: distances, clearances, net markers, and annotations.
Feature overview →Measure the distance between any two objects on your board in X, Y, Z, and XY.


| Object | Examples |
|---|---|
| Pads | Pad centre, pad edge |
| Holes | Hole centre, hole edge |
| Tracks | Track centre, track edge |
| Component bodies | Body edge, body centre |
| Board edge | Any point on the outline |





Add visual markers to nets on the board for annotation and inspection.



Add custom text annotations to the 3D view.
Switch to a true 1:1 scale 2D view for precise measurements and 2D-style inspection.

| Mode | Best for |
|---|---|
| Perspective | General 3D inspection, component visualisation |
| Orthogonal | Measurements, 2D-style review, printouts, cross-sections |
Compare Designs plugin: Three articles covering revision comparison.
Feature overview →Load two board revisions into ZofzPCB to prepare for comparison.

Understand the colour-coded change indicators in the revision comparison view.

| Indicator | Meaning |
|---|---|
| Highlighted in copper colour | Element exists in the new version but not the old |
| Dimmed or removed | Element exists in the old version but not the new |
| Unchanged | Element is identical in both versions |
The comparison works across all layers simultaneously: a change on an inner copper layer is just as visible as one on the surface.
Focus on specific layers or types of changes in the revision comparison view.
Use the layer panel to hide all layers except the one you want to review.
Use the compare controls to show:
Two articles covering ZofzPCB's programmatic interface for connecting to external tools.
CrossCheck is ZofzPCB's programmatic interface for connecting to external tools, primarily schematic editors.

CrossCheck allows ZofzPCB to communicate in real time with a schematic editor running alongside it. When you click a component or net in ZofzPCB, CrossCheck sends a command to the schematic editor to navigate to that same element, and vice versa.
ZofzPCB exposes a command interface that external tools can connect to. CrossCheck sends component, pad, and net identifiers to the connected tool, which then navigates accordingly. The keyboard and mouse control mapping is configurable.
Set up a live connection between ZofzPCB and your schematic editor.
CrossCheck has been tested and documented with OrCad Capture. Other schematic editors that support external command interfaces may also work.
For a live demo: zofzpcb.com/Cross-Check
Keys and mouse functions used for CrossCheck commands can be customised in the CrossCheck submenu.
Five reference articles covering shortcuts, file formats, system requirements, performance, and bug reporting.
| Action | Control |
|---|---|
| Rotate | Left mouse button + drag |
| Pan | Right mouse button + drag |
| Zoom | Scroll wheel |
| Reset view | Spacebar |
| Next component | N |
| Previous component | P |
| Action | Key |
|---|---|
| Peel top layer | F6 |
| Spread / compress layers | F7 |
| Set cross-section angle (45° steps) | Hold Delete + move mouse |
| Set any angle | Hold Shift + Delete + move mouse |
| Move the cut through the board | Hold Delete again + move mouse |
| Leave cross-section | Escape |
| Action | Control |
|---|---|
| Select object | Left click |
| Highlight net | Left click on copper |
| Context menu | Right click |
| Action | Key |
|---|---|
| CrossCheck component | C (in CPN or C mode) |
| CrossCheck pad | P (in CPN mode) |
| CrossCheck net | N (in CPN mode) |
| Format | Type | Notes |
|---|---|---|
| Gerber RS-274X | Layer images | Industry standard: most common |
| Gerber X2 | Layer images | Extended format with layer attributes |
| Excellon | Drill files | Standard drill format |
| Gerber (drill) | Drill files | Preferred over Excellon for accuracy |
| IPC-356 | Netlist | For component placement and net checking |
| BOM (CSV) | Bill of materials | For component models |
| ODB++ | Complete design | Single packed format |
| IPC-2581 | Complete design | Single XML format: recommended |
| ZIP | Archive | Gerber sets and IPC-2581 loadable from ZIP |
| Format | Type | Notes |
|---|---|---|
| .zofzproj | Rendered project | Complete saved board with all settings |
| .camset | Configuration | Stackup and settings only |
| STEP | 3D model | For mechanical CAD: STEP Export plugin |
| PNG / JPG | Screenshot | Static image export |
| Component | Minimum |
|---|---|
| Operating system | Windows 10 (64-bit) |
| Runtime | Microsoft VC++ Runtime (download link on the download page) |
| DirectX | DirectX 11 |
| Input | Scroll wheel mouse (required) |
| GPU | Integrated GPU of a modern PC or laptop |
| RAM | 4 GB |
| Component | Recommended |
|---|---|
| Operating system | Windows 11 (64-bit) |
| GPU | Dedicated gaming-level GPU |
| RAM | 8 GB or more |
Tips for improving 3D rendering speed, especially for large or complex boards.


| Board size | GPU recommendation |
|---|---|
| Small to medium | Integrated GPU sufficient |
| Large / many layers | Dedicated gaming GPU recommended |
How to report issues, unexpected behaviour, or crashes to the ZofzPCB team.
Use the contact form. Include:
Contact the team directly at zofz@zofzpcb.com
ZofzPCB version · Windows version · GPU model · Description and reproduction steps · Example files if relevant