In short: Altium Designer wraps schematics, PCB, libraries, rules and output jobs into one project-centric, rule-driven environment where a single compile-and-ECO step keeps the schematic and board in sync, whereas KiCad uses lighter, file-based tools with explicit netlist-style updates and a more open, text-based rule system.
Why the workflow matters more than the feature list
Interviewers for PCB roles rarely ask which button draws a track. They ask how you keep a 12-layer board with 800 components consistent across schematic revisions, library changes and fabrication releases. Altium Designer is built around that question: everything hangs off a project, rules are queries over design objects, and releases are scripted. Understanding that model also explains why engineers moving to or from KiCad often feel lost for a week. If you are new to the overall sequence of steps, our guide to the PCB design flow gives the vendor-neutral baseline that both tools implement.
The project as the unit of work
In Altium everything starts with a .PrjPcb file. It does not contain the design itself; it is a manifest listing the source documents and the project options: the schematic sheets (.SchDoc), the board (.PcbDoc), local libraries (.SchLib, .PcbLib), and output job files (.OutJob). It also stores compile settings, error-reporting severities (for example, whether a floating net label is a warning or a fatal error) and comparator rules that control what an ECO may change.
Because the project owns the rules for netlist generation, "compile" is a real step. Altium builds a connectivity model from all sheets, resolves hierarchy (flat or hierarchical, including repeated channels via Repeat(...) sheet symbols) and flags violations such as duplicate designators or unconnected pins before anything reaches the board.
Schematic libraries: components as managed data
A classic Altium component is a schematic symbol in a .SchLib with one or more footprint models linked from a .PcbLib, plus parameters such as manufacturer part number, value and tolerance. Older flows bundled these into an integrated library (.IntLib); most teams now use database libraries (.DbLib) that map a row in an SQL or spreadsheet table to a symbol, footprint and supply-chain data, or managed components in an Altium 365 workspace with revision history.
The reason this matters: a footprint error is the costliest library mistake. A 0.5 mm pitch QFN with a pad 0.1 mm too wide produces solder bridges across a whole batch. Managed libraries give you review, versioning and a single source, so ECO updates carry a known component revision. KiCad stores symbols in .kicad_sym and footprints as individual .kicad_mod files collected in .pretty folders, resolved through global and project library tables (sym-lib-table, fp-lib-table). It is simpler and Git-friendly, but governance of parameters and sourcing is mostly up to you.
Key fact: In Altium the link between a schematic part and its footprint is a component model assignment, and ECO compares footprints by name and library identity, so renaming a footprint without updating the symbol shows up as a removed-and-added part, not a modification.
Design rules: queries, scopes and priorities
Altium's PCB Rules and Constraints Editor stores rules in the .PcbDoc, grouped into categories: Electrical (clearance, short-circuit, un-routed net), Routing (width, via style, differential pairs), Plane, Manufacturing (annular ring, hole size, silk-to-mask clearance), High Speed, Placement and Signal Integrity. Each rule has a scope expressed as a query, for example InNetClass('DDR_Data') or InNet('GND') And OnLayer('Top Layer'), and a priority. When two rules match the same object, the lowest priority number wins.
A concrete example: a default clearance rule of 0.15 mm (6 mil) for the whole board, a higher-priority 0.30 mm rule between HV_Net and everything else for a 48 V domain, and a width rule that fixes USB_D pair traces to 0.18 mm to meet 90 Ω differential impedance on a specific stackup. The latter depends directly on the numbers in your PCB stackup design, which is why the stackup editor and impedance rules should be set up before routing. The generic reasoning behind clearance and width limits is covered in PCB design rules.
Newer Altium versions also provide a Constraint Manager: a spreadsheet-like view where nets, net classes and differential pairs are rows and constraints are columns. Instead of writing a query for each requirement, you select a class and fill in values, which suits high-speed work such as DDR byte lanes where length matching (for example ±25 mil within a byte group) is set per group. Under the hood it still generates rules, so you can debug them in the rules editor.
From schematic to board: compile, ECO and keeping sync
The signature Altium move is the Engineering Change Order. After compile, Design > Update PCB Document builds a list of changes: add components, add nets, add rooms, remove orphaned objects. You review each line, validate, then execute. The same dialog works in the other direction, so a swapped pin or renamed net on the board can be pushed back to the schematic. That bidirectional model is the reason Altium teams rarely hand-edit the netlist. If you routed a differential pair and later renamed it from USB_DP to USBP on the sheet, the ECO renames the board net and keeps the routing and its rules intact when the class still matches.
Output jobs and release
An .OutJob is a saved recipe for every fabrication and assembly deliverable: Gerber X2 or ODB++, NC drill, IPC-356 netlist, pick-and-place, bill of materials, assembly PDFs and 3D STEP. You configure it once, and the same job regenerates identical packages for revision A, B and C. Pair that with checks from the PCB design for manufacturing guide, such as minimum annular ring and solder-mask slivers, and your output job becomes a repeatable gate rather than a manual checklist. Altium 365 extends this with release-to-workspace snapshots so a manufacturer or reviewer sees exactly what was frozen.
Key fact: Run the Design Rule Check with "Create report file" and "Stop when 500 violations found" off for sign-off; a truncated DRC is the most common reason an unrouted net reaches fabrication.
Altium versus KiCad at a glance
| Area | Altium Designer | KiCad |
|---|---|---|
| Project file | .PrjPcb manifest with compile options | .kicad_pro with separate .kicad_sch, .kicad_pcb |
| Schematic to board | Compile plus ECO, bidirectional | Update PCB from Schematic; back-annotation for pin or footprint swaps |
| Rules | Query-scoped rules, priorities, Constraint Manager | Net classes plus text-based custom rules (.kicad_dru) |
| Libraries | Local, database or managed workspace components | Library tables, plain files, easy to version in Git |
| Outputs | .OutJob with release management | Plot and fabrication dialogs; Jobsets in recent releases |
| Cost model | Commercial subscription | Free and open source (GPL) |
Neither tool is universally better. For a single engineer building 4-layer boards with a few hundred parts, KiCad is fast and transparent. For teams that need component governance, constraint-driven high-speed layout, rigid-flex stackups or HDI via structures (see HDI PCB design), Altium's integrated model pays off. Knowing both and being able to explain the differences is a strong interview signal. If you want structured, hands-on practice, explore the CourseTron course catalogue, and for tool-based training and placement support see ChipXpert.
Ready to design boards like a pro? Join the CourseTron PCB design course and practise stackups, rules and release packages on real projects. Browse the courses.
Frequently asked questions
Is a .PrjPcb file the design itself?
No. It is a manifest that lists documents and stores project options such as compile severities and ECO comparator settings. The schematic and board data live in the separate .SchDoc and .PcbDoc files.
What decides which Altium rule applies when several match?
Priority. Every rule has a numeric priority and the lowest number among rules whose scope query matches both objects is applied. Keep specific rules (a high-voltage net) above general ones (All).
Can Altium and KiCad projects be exchanged?
Both support importing foreign formats to some degree, but rules, constraints and library links rarely survive cleanly. Plan on re-checking net classes, clearances and footprints after any migration.
Why use an OutJob instead of exporting Gerbers manually?
An OutJob stores layer selection, drill formats, BOM columns and naming once, so every release is reproducible and reviewable. Manual exports vary by person and are a common source of fabrication errors.