Cennik O nas Pobierz za darmodla Windows 8.1 / 10 / 11
Support

User Manual

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

The ZofzPCB main window: menu bar, a fully assembled board in 3D and the side panel with layers
CHAPTER 01

Loading your project

Eight articles covering every way to get your design files into ZofzPCB.

Feature overview →
1.1 Auto Load (Gerber set)

The fastest way to load a Gerber project. ZofzPCB scans your folder, identifies your files, and proposes the stackup automatically.

When to use this

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.

Steps

  1. Go to File → Auto Load (Gerber Set)
  2. Select the folder containing your Gerber files
  3. ZofzPCB scans the folder and displays the detected files with their proposed layer assignments
    Open dialog with Gerber Autoload: rule Protel99se matched, with the detected layers, drill file, IPC-356 netlist and BOM listed
  4. Review the assignments: confirm that top copper, bottom copper, drill files, and board outline are correctly identified
  5. If any file is misidentified, right-click its row and select Remove or reassign it manually
  6. Press Execute Auto Load
  7. The stackup dialog opens: review and complete the stackup parameters before proceeding
  8. Press OK: Read & Render

How the autoloader works

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.

Eagle exports: Eagle's default Gerber export creates files in multiple subdirectories. Move all files into a single folder before using Auto Load.
1.2 Manual Compose (Gerber set)

Full manual control over file assignment and layer order. Use this when Auto Load does not correctly identify your files.

When to use this

Auto Load produced incorrect or incomplete layer assignments, or your project uses a non-standard naming convention.

Steps

  1. Go to File → New (For Manual Compose)
  2. A Stackup dialog and a File Explorer window open side by side
  3. Drag and drop your Gerber files from the File Explorer into the correct slots in the Stackup dialog
  4. To add core or pre-preg dielectric layers, right-click the Name column and select Add Uniform Layer
    Stackup dialog with the layer stack, drill plates, IPC-356 netlist and BOM, one core layer selected
  5. Arrange layers in the correct order (top to bottom, component side to solder side) by dragging rows up and down
  6. Assign drill plate parameters: specify start and end copper layers and set the via type
  7. Check the polarity of each layer: solder mask and paste are typically negative; copper is typically positive
  8. Press OK: Read & Render

Stackup dialog columns

ColumnDescription
NameFilename if a Gerber file is assigned to this layer
TypeLayer type: copper, solder mask, silkscreen, core, pre-preg etc.
ParAdditional parameters: polarity, special settings
ThickLayer thickness. For copper, enter in oz (oz per square foot)

Drill plate via types

TypeDescription
Non-platedPlain, non-conductive hole
PlatedConductive barrel: standard through-hole
FiledConductive barrel, metal filled or capped
µVia↓Blind via: metalized from bottom
µVia↑Blind via: metalized from top
µVia↓ FiledBlind via, filled, metalized from bottom
µVia↑ FiledBlind via, filled, metalized from top
1.3 Loading ODB++

ODB++ loads as a single file, no stackup configuration needed.

When to use this

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.

Steps

  1. Go to File → Open
  2. Navigate to your ODB++ file and select it
  3. ZofzPCB reads the file and builds the board automatically, no manual layer assignment required
  4. The stackup dialog opens for review: ODB++ includes stackup information so most parameters will be pre-filled
  5. Confirm the stackup and press OK: Read & Render
ODB++ files may use .gz compression. ZofzPCB reads them directly: you do not need to extract them first.
ODB++ files cannot be loaded from within a ZIP archive. Extract before loading.
1.4 Loading IPC-2581

IPC-2581 is a single XML file containing everything ZofzPCB needs, including stackup, netlist, and component data.

When to use this

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.

Steps

  1. Go to File → Open
  2. Navigate to your IPC-2581 file (.xml) and select it
    File → Open with an IPC-2581 XML file selected, the board already shown in 3D behind the dialog
  3. ZofzPCB reads the file and builds the board automatically
  4. The stackup dialog opens for review: all parameters should be pre-filled
    Stackup dialog pre-filled from the IPC-2581 file
  5. Confirm and press OK: Read & Render
    Board from the IPC-2581 file rendered in 3D

Why IPC-2581 is the recommended format

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.

IPC-2581 files can be loaded directly from ZIP archives.
1.5 Loading from ZIP

ZofzPCB can read Gerber sets, .camset files, and IPC-2581 files directly from ZIP archives without extracting them first.

When to use this

Your design files are delivered or stored as a ZIP archive.

What works with ZIP

FormatZIP supported?
Gerber file setYes. Treated as a folder
.camset configuration fileYes. Read and save
IPC-2581Yes. Extracted automatically
.zofzproj rendered projectNo. Uses its own LZMA compression
ODB++No. May use its own gz compression

Steps

  1. Go to File → Auto Load or File → Open as normal
  2. Navigate to the ZIP file: ZofzPCB displays the ZIP contents as if it were a folder
  3. Proceed with loading as normal
Only ZIP format is supported. Extract 7z and RAR archives first.
1.6 Custom autoload rules

Autoload recognizes files by their names. If your CAD tool uses names ZofzPCB doesn't know, add your own rules:

  • Click Edit Rules in the autoload panel. This opens CAM_Load_Rules.txt (in %APPDATA%\ZofzPCB); the file explains its format at the top.
  • Write file masks in lowercase.
  • Masks can include a folder, e.g. Drill_PTH *\*.drl for drill files in a subfolder.
  • Examples from users, Altium: 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.
  • Updates keep your rules. Reset Rules on the Gerber Load dialog restores the rules that ship with ZofzPCB.
1.7 Auto-Offset and the Drill / Pad Fit Warning

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.

1.8 Panel outlines

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.

Good to know: plated slots drawn as milling lines. Plated slots that are drawn as milling lines on a mechanical or outline layer (common in Eagle and Allegro output) are not recognized and don't appear in 3D.
CHAPTER 02

Configuring the stackup

Seven articles covering stackup setup: the critical step between loading your files and rendering your board.

Feature overview →
2.1 Reviewing the stackup

Before ZofzPCB renders your board it proposes a stackup. This is your moment to review and complete it.

When to use this

Every time you load a Gerber set, before pressing Read & Render.

What to check

  1. Layer order: top copper at the top, bottom copper at the bottom, inner layers in correct sequence
  2. All copper layers present: count them against your CAD tool's layer stack
  3. Board outline identified: the PCB boundary layer must be assigned
  4. Drill files linked: each drill file assigned to the correct copper layer span
  5. Dielectric layers present: core and pre-preg between each copper layer
For 3D visualisation only: basic layer order and assignments are sufficient. ZofzPCB renders a visually correct prototype without full stackup detail.
For DFM validation: complete material, thickness, and copper weight data is essential.
2.2 Layer types and thickness

Gerber files carry copper artwork but not stackup parameters. Enter these manually for accurate DFM validation.

Gerber file parameters dialog with layer type, polarity and thickness settings

When to use this

After loading a Gerber set, when you want full stackup parameters for DFM validation or accurate STEP export.

Parameters to enter

ParameterDescription
Layer typeCore or pre-preg for dielectric layers
ThicknessLayer thickness in millimetres
Copper weightTypically 1oz, 2oz, or 0.5oz per copper layer
MaterialFR4, Rogers, polyimide, or other substrate

Steps

  1. Open the Stackup dialog (Stackup → Display/Edit)
  2. For each dielectric layer, click the Type column and select Core or Pre-preg
  3. Click the Thick column and enter the thickness in mm
  4. For copper layers, enter the copper weight using oz notation (e.g. 1oz)
  5. Enter the total PCB thickness in the Board Outline thickness field: ZofzPCB adjusts the core/pre-preg layers to match
Tip: If you know the total board thickness but not individual layer thicknesses, enter the total in the Board Outline field. ZofzPCB distributes the remaining thickness across the dielectric layers proportionally.
2.3 Drill plates and via types

Configure drill files to correctly represent through-holes, blind vias, buried vias, and µVias.

Drill file parameters dialog with start layer, end layer and via type

When to use this

When your board uses multiple drill files, non-standard via types, or blind and buried vias.

Drill plate columns

ColumnDescription
NameFilename of the drill file
From/ToStart and end copper layer numbers
TypeVia type: see table below

Via types

TypeDescription
Non-platedPlain, non-conductive hole
PlatedConductive barrel: standard through-hole
FiledConductive barrel, metal filled or capped
µVia↓Blind via: metalized from bottom
µVia↑Blind via: metalized from top
µVia↓ FiledBlind via, filled, metalized from bottom
µVia↑ FiledBlind via, filled, metalized from top

Steps

  1. In the Stackup dialog, locate the Drill Plates section
  2. Set From and To columns to the copper layers the drill spans
  3. Set the Type column to the correct via type
  4. If a drill file contains both holes and routing, add both to the Drill Plates list
2.4 Board outline

The board outline defines the physical boundary of the PCB. ZofzPCB needs it to correctly render and clip the board.

Methods ZofzPCB supports

  • Standard outline layer: a dedicated Gerber layer for the board boundary (most common). Detected automatically in Auto Load.
  • Meta drawing: the outline is drawn on a copper or silkscreen layer using thin tracks. Set a thickness threshold via right-click on the layer in the Stackup dialog.
    Board outline drawn with thin tracks on a copper layer (meta drawing)
  • Identify outline: for M2M files where the outline must be inferred:
    Identify outline options for inferring the board edge
OptionDescription
Accept all detected loopsAll detected outlines define multiple PCBs
Auto recognitionFinds a division line between the PCB and drawing text
Take the greatest loopAssumes the largest shape is the PCB
Take 2–10 greatest loopsFor boards with multiple outlines or cutouts
Gerber drawing with board, dimension lines and text merged into one shape
Board outline separated from the drawing

Steps (standard)

  1. In the Stackup dialog, confirm the Board Outline layer is assigned to the correct Gerber file
  2. Enter the total PCB thickness in the Board Outline Thick field
2.5 Saving your stackup (.camset)

Save your stackup configuration so you don't have to re-enter settings when you regenerate Gerber files.

What .camset saves

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

Note: .camset does NOT save the rendered board itself, only the configuration. Use .zofzproj for the full rendered board.

To save

  1. Go to File → Save As
  2. In the Save As Type dropdown, select .camset
  3. Choose a filename and location: keep it in the same folder as your Gerber files
  4. Press Save

To load

  1. Go to File → Open and select the .camset file
  2. ZofzPCB re-reads the Gerber files using the saved settings
  3. Or double-click the .camset file directly
2.6 Saving your project (.zofzproj)

Save the complete rendered board, including all component models and settings, as a single project file.

Difference between .camset and .zofzproj

.camset.zofzproj
Saves rendered boardNoYes
Saves configurationYesYes
File sizeSmallLarger
Use caseRe-load after Gerber regenerationSave complete session

To save

  1. Go to File → Save As
  2. Select .zofzproj in the Save As Type dropdown
  3. Choose a filename and press Save

To save as view-only (free)

  1. In the Save As dialog, check the View-Only Mode option before saving
  2. The file can be opened by anyone in the free version: they can view but not modify or export
.zofzproj uses LZMA compression and cannot be read from or written to ZIP archives.
2.7 Blind and buried via spans

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.

CHAPTER 03

Viewing in 3D

Ten articles covering navigation, layer control, cross-sections, and rendering options.

Feature overview →
3.2 Layer panel and toggles

Turn individual layers on and off to focus on what matters.

Side panel with view modes and the layer list next to the 3D board

The right panel

The right panel contains checkboxes for every layer in your stackup, plus:

  • Components: toggle 3D component models on/off
  • Verticals: toggle via barrels and pads on/off
  • Transparency slider: make all layers semi-transparent
  • Hollow: render the board as a hollow shell

Steps

  1. The right panel is visible by default on the right side of the screen
  2. Click any layer checkbox to hide or show it
  3. Use the Components checkbox to toggle all component models at once
  4. Drag the Transparency slider to make layers semi-transparent
3.3 Peel and expand layers

Separate the layers of your board to inspect the stackup from the inside.

Peel

Removes layers from the top down, like peeling back the board one layer at a time.

  • Press F6 to peel the top layer
  • Press repeatedly to peel multiple layers
  • Press F7 to compress (restore) layers

Expand (Spread)

Separates all layers vertically, creating a gap between each layer.

  • Press F7 to spread all layers apart
  • Drag the Spread slider in the right panel for fine control
  • Press F7 again to compress back to normal

Material density / Hollow

The Hollow checkbox makes dielectric layers transparent, revealing the copper inside without physically separating layers.

3.4 Cross-section

Cut through your board at any angle to inspect inner layers, via stacks, and copper connections.

Cross-section through the board: a plated via passing through all copper layers, with its hole size shown
Hold Delete to set the angle, hold Delete again to move the cut

Steps

  1. Point the mouse at the place where you want to cut.
  2. Hold Delete and move the mouse to set the angle of the cut. The angle snaps in 45° steps; hold Shift as well for any angle. Release Delete.
  3. Hold Delete again and move the mouse to move the cut through the board.
  4. Press Escape to leave the cross-section and return to the full board view.

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.

Tips

  • Position over a via stack to verify all layers are correctly connected
  • Use a diagonal cut to inspect angled traces
  • Combine with Spread to see each layer's cross-section separately
  • Use Orthogonal camera mode for a true 2D cross-section view
3.5 Colour presets and picker

Change how your board looks by applying colour presets or customising individual layer colours.

View menu with colour presets
Colour picker for a layer

Colour presets

Go to View → Color Presets to select a built-in colour scheme.

Custom colour picker

  1. Go to View → Color Picker
  2. Select the layer you want to change
  3. Choose a colour: the change applies immediately

Colour settings are saved in your .camset and .zofzproj files.

3.6 Render effects and lighting

Fine-tune the 3D rendering appearance: wireframe, subsampling, thick layers, camera projection, and lighting.

Render effects settings
Light parameters relative to the camera
Light parameters relative to the board geometry
Board rendered with exaggerated layer thickness

View menu options

OptionDescription
WireframeShow board as wireframe outline only
SubSamplingReduce render quality for better performance
Thick layersExaggerate layer thickness for clearer visualisation
Camera FOVAdjust field of view
Net selection effectsVisual style for highlighted nets
Render effectsPost-processing effects on the 3D view
LightAdjust light direction and intensity
Performance tip: Lowering SubSampling has the biggest impact on rendering performance. See 10.4 Performance and GPU.
3.7 Screenshot and autopilot

Capture high-resolution images of your board and use autopilot for automated rotation.

Screenshot dialog
Autopilot settings for automatic camera movement

Screenshot

  1. Position the board as you want it
  2. Go to Screenshot in the menu bar
  3. Choose resolution and file format
  4. Select a save location and press Save

Screenshots capture the exact view: colour scheme, layer visibility, cross-sections, and any measurements or annotations currently visible.

Autopilot

Rotates the board automatically in a smooth continuous movement, useful for presentation sequences.

  1. Go to Autopilot in the menu bar
  2. Set rotation speed and axis
  3. Press Start / Stop
3.8 Show one layer alone

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.

3.9 Mouse and keyboard

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.

3.10 Colors for realistic screenshots

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:

EntryValue
CopperFFCB7B48
Plated H.00D0D3D2
VolumeFF6E7672
Edge InFF5F786C
Edge Out008FA69A
Background001B2B16
CHAPTER 04

Components

Six articles covering 3D component models, from automatic generation to custom building.

Feature overview → Background: IPC-356 and 3D components →
4.1 Auto 3D modeler

ZofzPCB automatically generates 3D component models from your BOM and PCB footprints, no library setup required.

How it works

The auto-modeler reads your BOM and IPC-356 netlist, then uses the PCB footprint geometry to generate a 3D model for each component.

VariantDescription
ExtrudedFree: simplified block-shaped models from the footprint outline
RealisticFree: more detailed models with pin geometry and body shape
Components shown as extruded block models
Extruded models
Components shown as detailed parametric models
Parametric models

Requirements

  1. A BOM file in CSV format must be loaded
  2. An IPC-356 netlist must be loaded
  3. Component references in the BOM must match those in the netlist
If component references were truncated during IPC-356 export (the format limits names to 6 characters), some components may not be matched. See 4.4 IPC-356 and BOM matching.
4.2 Component library

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

Component editor with model parameters

Accessing the library

  1. Go to Components in the menu bar
  2. The component list shows all components loaded from your BOM
  3. Components with 3D models show a model indicator
  4. Components without models are listed but appear as empty footprints in the 3D view

Adjusting component models

For each component you can:

  • Adjust model parameters: fine-tune the auto-generated model dimensions
  • Replace with Body Builder model: assign a custom model
  • Override component height: set an exact height for the component body

Adjustments are saved in .camset and .zofzproj files and applied every time you reload the project.

Modeling a capacitor, step 1 of 6
Modeling a capacitor, step 2 of 6
Modeling a capacitor, step 3 of 6
Modeling a capacitor, step 4 of 6
Modeling a capacitor, step 5 of 6
Modeling a capacitor, step 6 of 6
Board with component models generated automatically from the footprints
4.3 Body Builder

Create precise custom 3D models for components the auto-modeler cannot fully capture.

When to use this

  • Exotic, custom, or proprietary components with non-standard geometries
  • Exact 3D fidelity needed for mechanical interference checks or STEP export
  • Component body shape critical for enclosure design or thermal simulation

How it works

The Body Builder is a geometric editor where you define:

  • Body dimensions: length, width, height
  • Pin geometry: pin positions, sizes, and lead style
  • Body shape: rectangular, cylindrical, or custom

Models are saved to your project's component library and reusable across all boards.

Steps

  1. Open the component library (Components menu)
  2. Select the component you want to model
  3. Click Body Builder
  4. Define the body dimensions
  5. Add pins and set their positions
  6. Press Save: the model is applied immediately
Body Builder, step 1 of 11
Body Builder, step 2 of 11
Body Builder, step 3 of 11
Body Builder, step 4 of 11
Body Builder, step 5 of 11
Body Builder, step 6 of 11
Body Builder, step 7 of 11
Body Builder, step 8 of 11
Body Builder, step 9 of 11
Body Builder, step 10 of 11
Body Builder, step 11 of 11
Time-lapse: building a DB-9 connector
4.4 IPC-356 and BOM matching

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

Raw IPC-356 netlist file in a text editor
Pads without a net in the IPC-356 file, first example
Pads without a net in the IPC-356 file, second example
Unconnected pads missing from the IPC-356 file
IPC-356 file parameters dialog

How matching works

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).

Common issue: truncated references

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.

Solutions:

  • Keep reference designators to 6 characters or fewer
  • Check for duplicate truncated names: two references truncating to the same string will both fail
  • Some CAD tools allow longer designators as a non-standard extension: check your export settings

Checking for errors

Go to Netlist → Errors to see components that could not be matched.

4.5 Change a component's model

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.

Tip for Body Builder: in the tree list, Up and Down move between entries, and Enter finishes editing and jumps to the next line.
4.6 Components missing in 3D

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.

CHAPTER 05

Inspecting your design

Eight articles covering design inspection: components, nets, vias, holes, and schematic crosscheck.

Feature overview →
5.1 Browsing components

Find, highlight, and zoom to any component on your board instantly.

Components list with a connector selected and highlighted on the 3D board
Tooltip showing component and pin under the mouse pointer
Right-click menu on a component

Steps

  1. Go to Components in the menu bar, or use the right panel component list
  2. Click any component: ZofzPCB highlights it and zooms to it across all layers simultaneously
  3. Or click the component directly on the board to select and zoom

Keyboard navigation

  • N: jump to next component
  • P: jump to previous component

What you can see per component

  • 3D model in full context
  • Pin positions and designators
  • Component reference and value from the BOM
  • Net assignments for each pin
5.2 Browsing nets and pins

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

Components pin list with one pin selected; the pin and its whole net highlighted on the board
Select a pin to highlight it, and with Show Pin Net, its whole net.
Browse Detected Connections with the net RX1_AV1.2 selected and highlighted through the board in 3D

Browsing nets

  1. Go to Netlist → Nets
  2. Click any net: ZofzPCB highlights all copper belonging to that net across every layer
  3. Or click any trace, pad, or copper area on the board directly to highlight its net

Browsing pins

  1. Go to Netlist → Nodes PCB or Netlist → Nodes IPC
  2. Expand any net to see its pins
  3. Click any pin: ZofzPCB highlights and zooms to it
Nodes PCB: nets as detected from the copper data. Nodes IPC: nets as defined in the IPC-356 file. These should match. If they don't, see 5.4 Netlist error checking.
5.3 Browsing holes and vias

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

Hole browser

  1. Go to Vias/Holes in the menu bar
  2. The hole browser lists every hole and via
  3. For each hole you see: hole diameter · pad diameter · annular ring width · clearance to adjacent copper · layer span
  4. Click any hole to highlight and zoom to it
Holes List with drill sizes and coordinates, one hole selected and shown on the board
The hole browser groups all holes by size; select one to find it on the board.

Cut-through stack view

For any selected via, the hole browser shows a cross-section of the via stack, displaying all the copper layers it connects through.

5.4 Netlist error checking

Verify that the copper connections on your board match the IPC-356 netlist, and identify any discrepancies.

Steps

  1. Ensure your IPC-356 netlist is loaded
  2. Go to Netlist → Test to run the comparison
  3. Go to Netlist → Errors to view the results: Missing connections: nets in the IPC-356 with no copper connection; Extra connections: copper connections not in the IPC-356
  4. Click any error to highlight and zoom to the affected area
  5. Go to Netlist → Save Report to export the results
5.5 CrossCheck: schematic sync

Navigate between your PCB in ZofzPCB and your schematic editor simultaneously.

Example of component and net data copied from ZofzPCB

CrossCheck modes

ModeDescription
DisabledCommands not sent; P and N keys act for selection
CPN: Comp Pad NetC, P, N keys send crosscheck commands
C: cross-checkC key sends crosscheck; P and N keys act for selection
On HoverMouse hover triggers crosscheck

Steps

  1. Set up the connection: see 9.2 Connecting to a schematic editor
  2. Go to Netlist → Cross Check and select your preferred mode
  3. Click or hover over a component or net: the schematic editor jumps to that element
5.6 Show only TH or SMD components

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.

5.7 Netlist CSV export

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.

5.8 Holes List

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.

CHAPTER 06

Measuring

Four articles covering measurements: distances, clearances, net markers, and annotations.

Feature overview →
6.1 Distance measurements

Measure the distance between any two objects on your board in X, Y, Z, and XY.

Steps

  1. Go to Measurements in the menu bar, or right-click → Measure
    Right-click menu with measurement options
    Right-click menu with measurement target selection
  2. Click the first object: a pad, hole, track edge, component body, or board edge
  3. Click the second object
  4. ZofzPCB displays X, Y, Z and XY distances between the two points

Measurable objects

ObjectExamples
PadsPad centre, pad edge
HolesHole centre, hole edge
TracksTrack centre, track edge
Component bodiesBody edge, body centre
Board edgeAny point on the outline
Measurement target: hole
Measurement target: pad
Measurement target: edge
Measurement target: track
Measurement target: net

Tips

  • Use Orthogonal camera mode for 2D-style measurements
  • Multiple measurements can be active simultaneously
  • Measurements are saved in .camset and .zofzproj files
6.2 Net markers

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

Selected net blinking in its highlight colour
Blink color only
Selected net uncovered by hiding layers above it
Uncover selection
Only the selected net visible
Show only selection

Steps

  1. Select a net by clicking on any copper belonging to it
  2. Go to Measurements → Net Marker
  3. A marker is placed on the selected net with the net name as its label
  4. Markers are visible in the 3D view and captured in screenshots

Managing markers

  • Multiple net markers can be placed simultaneously
  • Markers are saved in .camset and .zofzproj files
  • Remove a marker by selecting it and pressing Delete
6.3 Text balloons

Add custom text annotations to the 3D view.

Steps

  1. Go to Measurements → Text Balloon
  2. Click the point on the board where you want the balloon to point
  3. Type your annotation text and press Enter
  4. The balloon appears with a leader line pointing to the selected location

Tips

  • Text balloons are visible in screenshots
  • Saved in .camset and .zofzproj files
  • Drag a balloon to reposition it after placing
6.4 Orthogonal camera mode

Switch to a true 1:1 scale 2D view for precise measurements and 2D-style inspection.

Camera field-of-view settings

Steps

  1. Go to View → Camera FOV and select Orthogonal
  2. Navigate using the same mouse controls: pan with right button, zoom with scroll wheel
  3. All measurements in orthogonal mode are true 1:1 scale
  4. Return to perspective: View → Camera FOV → Perspective

When to use each mode

ModeBest for
PerspectiveGeneral 3D inspection, component visualisation
OrthogonalMeasurements, 2D-style review, printouts, cross-sections
CHAPTER 07

Compare revisions

Compare Designs plugin: Three articles covering revision comparison.

Feature overview →
7.1 Loading two versions

Load two board revisions into ZofzPCB to prepare for comparison.

ZofzPCB Compare Designs: two ODB++ revisions loaded, changed traces highlighted

Steps

  1. Load your current board version as normal
  2. Go to File → Compare
  3. Select the second board version: Gerber set, ODB++, IPC-2581, or .zofzproj
  4. ZofzPCB loads both versions and overlays them in the 3D view with differences highlighted

Requirements

  • Both boards must be the same design (same outline, same layer count)
  • Both must be loaded from compatible file formats
  • Best results when both versions share the same coordinate origin
7.2 Reading the diff overlay

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

ZofzPCB Compare Designs: a changed LED highlighted in red between two board revisions in 3D

What the overlay shows

IndicatorMeaning
Highlighted in copper colourElement exists in the new version but not the old
Dimmed or removedElement exists in the old version but not the new
UnchangedElement 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.

Navigating changes

  • Use the layer panel to focus on one layer at a time
  • Use cross-section to inspect changes on inner layers
  • Zoom to any highlighted area to inspect in detail
7.3 Filtering changes

Focus on specific layers or types of changes in the revision comparison view.

Filtering by layer

Use the layer panel to hide all layers except the one you want to review.

Filtering by change type

Use the compare controls to show:

  • Additions only: elements in the new version but not the old
  • Removals only: elements in the old version but not the new
  • Both: all changes

Tips

  • Combine layer filtering with cross-section to inspect inner layer changes in isolation
  • Use the component browser to check if specific components changed position or orientation
CHAPTER 08

Export and share

STEP export and View-Only Mode: Three articles covering how to get your board model out of ZofzPCB.

Feature overview →
8.1 STEP file exportSTEP Export plugin

Export a complete 3D model of your board for mechanical CAD, simulation, or documentation.

STEP export dialog in mechanical mode
Mechanical mode
STEP export dialog in thermal solver mode
Thermal solver mode

What the STEP file includes

  • Board outline and PCB shape
  • All copper layers
  • Every mounted component as a structured assembly element
  • Board thickness and stackup geometry

Steps

  1. Ensure your stackup dimensions are correctly entered, see 2.2 Layer types and thickness
  2. Ensure all components have 3D models, see 4.1 Auto 3D modeler and 4.3 Body Builder
  3. Go to File → Export STEP
  4. Choose a filename and save location
  5. Press Export

Compatible applications

SolidWorks · CATIA · Fusion 360 · FreeCAD · Any mechanical CAD or simulation tool that supports STEP (ISO 10303)

For the most accurate export, enter complete stackup data before exporting. Missing thickness data results in default values being used.
8.2 View-only sharing

Share an interactive 3D view of your board with colleagues or clients, no ZofzPCB installation required.

Save As dialog with the View-Only File option and the allowed functions checked
A board opened as a View-Only file in ZofzPCB, shown in 3D with components and silkscreen

What recipients can do: rotate, zoom, pan, inspect from any angle

What recipients cannot do: modify, export, or access source files

Method 1: Save as view-only .zofzproj

  1. Go to File → Save As
  2. Select .zofzproj as the file type
  3. Check the View-Only Mode option before saving
  4. Share the .zofzproj file: recipients open it in the free version of ZofzPCB

Method 2: pcbmodel.com gallery

Share your board publicly via the PCB Model gallery at pcbmodel.com.

8.3 Screenshot export

Save a high-resolution image of your current 3D view.

Steps

  1. Set up the view: angle, zoom, layer visibility, colour scheme, annotations
  2. Go to Screenshot in the menu bar
  3. Select output resolution and file format
  4. Choose a save location and press Save

Tips

  • Screenshots capture all visible annotations: measurements, net markers, text balloons
  • Use a high resolution for print-quality output
  • Use Orthogonal camera mode for a clean 2D-style top-down view
CHAPTER 09

CrossCheck: programmatic interface

Two articles covering ZofzPCB's programmatic interface for connecting to external tools.

9.1 What is CrossCheck?

CrossCheck is ZofzPCB's programmatic interface for connecting to external tools, primarily schematic editors.

Example of component and net data copied from ZofzPCB

Overview

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.

Use cases

  • Design review: click a component in ZofzPCB and jump to it in the schematic instantly
  • Error tracing: found a net error? Jump to the schematic to find the source
  • Cross-discipline review: share a live review session between PCB and schematic designers

How it works technically

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.

9.2 Connecting to a schematic editor

Set up a live connection between ZofzPCB and your schematic editor.

Supported tools

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

Steps (OrCad Capture)

  1. Open both ZofzPCB and OrCad Capture with the same design loaded in each
  2. In ZofzPCB, go to Netlist → Cross Check
  3. Select your preferred CrossCheck mode: CPN: Comp Pad Net: C, P, N keys send crosscheck commands; C: cross-check: only the C key sends commands; On Hover: mouse hover triggers commands automatically
  4. In OrCad, configure the external command receiver to accept ZofzPCB's commands
  5. Click a component in ZofzPCB: OrCad should navigate to the same component

Configuring key mapping

Keys and mouse functions used for CrossCheck commands can be customised in the CrossCheck submenu.

Troubleshooting

If CrossCheck is not working, verify that both applications have the same design loaded (same component references), the correct CrossCheck mode is selected in ZofzPCB, and OrCad's external command interface is enabled.
CHAPTER 10

Reference

Five reference articles covering shortcuts, file formats, system requirements, performance, and bug reporting.

10.1 Keyboard and mouse shortcuts

Navigation

ActionControl
RotateLeft mouse button + drag
PanRight mouse button + drag
ZoomScroll wheel
Reset viewSpacebar
Next componentN
Previous componentP

Layer control

ActionKey
Peel top layerF6
Spread / compress layersF7
Set cross-section angle (45° steps)Hold Delete + move mouse
Set any angleHold Shift + Delete + move mouse
Move the cut through the boardHold Delete again + move mouse
Leave cross-sectionEscape

Selection

ActionControl
Select objectLeft click
Highlight netLeft click on copper
Context menuRight click

CrossCheck (when enabled)

ActionKey
CrossCheck componentC (in CPN or C mode)
CrossCheck padP (in CPN mode)
CrossCheck netN (in CPN mode)
10.2 Supported file formats

Input formats

FormatTypeNotes
Gerber RS-274XLayer imagesIndustry standard: most common
Gerber X2Layer imagesExtended format with layer attributes
ExcellonDrill filesStandard drill format
Gerber (drill)Drill filesPreferred over Excellon for accuracy
IPC-356NetlistFor component placement and net checking
BOM (CSV)Bill of materialsFor component models
ODB++Complete designSingle packed format
IPC-2581Complete designSingle XML format: recommended
ZIPArchiveGerber sets and IPC-2581 loadable from ZIP

Output formats

FormatTypeNotes
.zofzprojRendered projectComplete saved board with all settings
.camsetConfigurationStackup and settings only
STEP3D modelFor mechanical CAD: STEP Export plugin
PNG / JPGScreenshotStatic image export
10.3 System requirements

Minimum requirements

ComponentMinimum
Operating systemWindows 10 (64-bit)
RuntimeMicrosoft VC++ Runtime (download link on the download page)
DirectXDirectX 11
InputScroll wheel mouse (required)
GPUIntegrated GPU of a modern PC or laptop
RAM4 GB

Recommended for large boards

ComponentRecommended
Operating systemWindows 11 (64-bit)
GPUDedicated gaming-level GPU
RAM8 GB or more

GPU notes

  • Small to medium boards: integrated GPU sufficient
  • Large, complex boards: dedicated GPU strongly recommended
  • DirectX 11 required: if ZofzPCB does not start, update your graphics drivers
10.4 Performance and GPU

Tips for improving 3D rendering speed, especially for large or complex boards.

Board rendered in wireframe mode

Steps to improve performance

  1. Lower SubSampling: go to View → SubSampling and reduce the level. Biggest single impact on performance
    View menu with SubSampling levels
  2. Turn off unused layers: use the right panel to hide layers you don't need
  3. Toggle off components: uncheck Components in the right panel if 3D models aren't needed
  4. Close other GPU-intensive applications running in the background
  5. Check GPU assignment (laptops): make sure Windows is using the dedicated GPU for ZofzPCB: go to Windows Settings → Display → Graphics, find ZofzPCB and set to High performance
  6. Update graphics drivers: outdated drivers are a common cause of performance issues

Hardware recommendations

Board sizeGPU recommendation
Small to mediumIntegrated GPU sufficient
Large / many layersDedicated gaming GPU recommended
10.5 Reporting bugs

How to report issues, unexpected behaviour, or crashes to the ZofzPCB team.

Option 1: Contact form

Use the contact form. Include:

  • ZofzPCB version number (shown in the title bar)
  • Description of what happened and what you expected
  • Steps to reproduce the issue
  • Relevant files (Gerber set, .camset, or .zofzproj) if file-specific
  • A screenshot if it helps

Option 2: Email

Contact the team directly at zofz@zofzpcb.com

Helpful information to include

ZofzPCB version · Windows version · GPU model · Description and reproduction steps · Example files if relevant