How to Use Altium Designer: Schematic Entry and PCB Layout Workflow

Detailed Explanation

Altium Designer's PCB workflow follows the same conceptual stages as any modern EDA tool — capture the schematic, assign physical footprints, transfer the design to a PCB, place and route it, then generate fabrication data — but Altium's implementation is built around integrated library management and a rule-driven design system that differs meaningfully from a lighter-weight tool. For a comparison against KiCad's approach to the same workflow, see Altium Designer vs KiCad; for the general concept of translating a schematic into a physical board, see What Is Schematic Capture?.

Project Structure

An Altium project (.PrjPcb) is a container that links together a schematic document (.SchDoc — one or more sheets, supporting flat or hierarchical multi-sheet designs), a PCB document (.PcbDoc), and references to the libraries used. Unlike file-based tools where every project file lives in a Git-friendly plain-text format, Altium's native documents are binary. Version control with Git is possible and commonly used, but diffs are not human-readable — most professional Altium teams instead rely on Altium 365 (Altium's cloud platform) for release management, revision history, and multi-user collaboration rather than file-level Git diffing.

Library-Centric Component Model

Altium's library model bundles everything a component needs into a single managed unit: the schematic symbol, one or more PCB footprints, a supplier/part-number link, and optionally a 3D STEP model and SPICE simulation model. Components are sourced from:

• Local libraries — schematic library (.SchLib) and PCB library (.PcbLib) files maintained within the project or a shared library folder.
• Database libraries — an external database (SQL, Excel, or Altium's own format) that centralises part data for an entire organisation, keeping symbol/footprint/supplier data consistent across many projects.
• Altium 365 vaults — a cloud-hosted, version-controlled component library with lifecycle states (draft, released, obsolete), letting a team enforce which parts are approved for use in new designs.

For teams managing hundreds or thousands of parts across multiple products, the database/vault model is a significant advantage over maintaining local library files per project — it keeps a single source of truth for footprint and symbol accuracy rather than parts drifting between projects over time.

Schematic Entry

Place components from the library, wire nets with the wiring tool, and use net labels, power ports, and off-page connectors to define connectivity across single or multi-sheet schematics. Altium's Electrical Rule Check (ERC) flags unconnected pins, conflicting net names, and power pin driver conflicts before the design is transferred to layout — functionally equivalent to KiCad's ERC, though Altium's rule set is more extensively configurable per-project.

Transferring to the PCB: Update PCB Document

With the schematic and an empty (or existing) PCB document open in the same project, Design → Update PCB Document compares the current schematic netlist against the PCB and generates an Engineering Change Order (ECO) — an explicit, reviewable list of every component addition, removal, and net change about to be applied. This is a meaningful workflow difference from a silent netlist import: the ECO dialog requires the designer to validate and execute the changes, giving a clear checkpoint before modifications land on the board, which is particularly valuable on large or hierarchical designs where an unreviewed bulk update could introduce unintended changes. If Validate Changes reports no differences despite a genuine schematic edit, the edited sheet is usually outside the project's current compiled state — see this ECO troubleshooting thread for the project-compilation fix.

Design Rules

Altium centralises layout constraints in the Design Rules dialog (Design → Rules), covering clearance, routing width, differential pair impedance, length matching, via constraints, and dozens of other categories. Rules can be scoped to specific nets, net classes, or board regions using query-based rule scopes — for example, applying a tighter clearance rule only to a high-voltage isolation zone rather than the whole board. Violations are flagged in real time during placement and routing (an online DRC), and a full batch DRC run before fabrication output catches anything not caught interactively.

Placement and Routing

Component placement uses standard move/rotate/align tools, with Altium's Room and Rule-based placement zones useful for enforcing keep-out areas or grouping related circuitry on larger boards. The interactive router supports the same push-and-shove, walkaround, and interactive modes found in other modern EDA tools, but Altium is generally regarded as stronger for dense, high-speed layouts: differential pair routing includes automatic accordion/trombone length tuning, and interactive length matching can be applied across an entire bus of nets simultaneously rather than one pair at a time. This depth is a large part of why teams doing serious high-speed digital or RF work often retain Altium over a lighter-weight tool — see Altium Designer vs KiCad for the fuller capability comparison.

Fabrication Output

Altium generates industry-standard fabrication data through File → Fabrication Outputs: Gerber (RS-274X or Gerber X2), NC drill files, and — increasingly the preferred format for complex boards — IPC-2581, a single XML-based file that combines layer geometry, drill data, netlist, and stackup information in one deliverable, reducing the ambiguity possible when a fabricator has to reconcile many separate Gerber and drill files manually. ODB++ export is also natively supported for fabricators that prefer it over Gerber. See what fabrication output files does a PCB need? for the general set of deliverables any tool must produce.

Design Considerations

• Set up a database or vault library early, not after the project has grown. Retrofitting centralised library management onto a project that started with ad hoc local libraries is significantly more work than establishing it from the first schematic sheet.
• Use ECO review deliberately, not as a rubber-stamp step. On a large hierarchical schematic, the ECO list after a significant schematic change can be long — actually read it before executing, rather than clicking through, to catch unintended net or footprint changes.
• Scope design rules narrowly where a board has mixed requirements (e.g. a high-voltage isolation section alongside dense digital routing) rather than relying on one board-wide rule set that's either too loose in the sensitive area or unnecessarily restrictive everywhere else.
• Decide the IPC-2581 vs Gerber/ODB++ output question with your fabricator up front. Not every fabricator's front-end accepts IPC-2581 without extra processing time; confirm the preferred format before generating a large batch of fabrication data late in the project. Zeus Design provides professional PCB layout in both Altium Designer and KiCad, matched to whichever toolchain best fits a project's team and long-term maintenance needs.

Common Mistakes

• Treating Altium's binary project files like plain-text KiCad files for Git collaboration. Binary diffs are not human-reviewable; teams that try to run an Altium project through the same Git branch-and-merge workflow as a text-based tool run into unresolvable merge conflicts. Use Altium 365 for collaborative revision control instead.
• Skipping the ECO review step out of habit. Clicking through the Engineering Change Order dialog without reading it defeats its purpose as a review checkpoint and can let an unintended schematic change propagate silently to the board.
• Building components without properly linked footprints and 3D models, which surfaces later as mechanical fit issues (STEP model missing or wrong) or fabrication mismatches (footprint doesn't match the schematic symbol's intended package) that a properly maintained library component would have caught earlier.
• Applying one board-wide design rule set to a board with genuinely different regions (e.g. isolation-critical high-voltage sections vs dense digital routing), rather than using query-based rule scoping to apply the right constraint to the right area.
• Choosing Gerber output by default without checking whether IPC-2581 would give the fabricator a cleaner, less ambiguous data package for a complex multi-layer board — especially relevant on boards with tight stackup or impedance requirements where separate Gerber/drill files leave more room for fabricator misinterpretation.