Electronics Design AUAltium ECO says 'no differences found' after I added components to the schematic — PCB just isn't picking up the changes
Asked by drc_nightmare ·
Working through a board revision — added a small level-shifter IC and a couple of passives to the schematic, saved everything, then went to Design > Update PCB Document to push the changes over. The Engineering Change Order dialog opens, I hit Validate Changes, and... nothing. "No differences found" even though I can clearly see the new parts on the schematic sheet.
Closed and reopened both documents, still nothing. I know the schematic save actually took because I can see the new components when I reopen the .SchDoc. Is there some project-level thing I'm missing? This is my first multi-sheet Altium project (previous boards were all single-sheet) so wondering if that's related.
3 Replies
Ninety percent of the time this exact symptom (ECO opens fine, Validate runs, zero differences reported) means the ECO isn't actually comparing against the sheet you edited — usually one of two causes, and the multi-sheet detail you mentioned points straight at the first one.
1. The edited sheet isn't part of the active project. If you opened the .SchDoc directly (double-clicked it from Explorer, or it was already open from a previous session outside the project context) rather than opening it through the project panel, your edits exist in that document but Altium's ECO generation works from the project's compiled document list — not from "whatever .SchDoc happens to be open." Check the Projects panel: is the sheet you edited actually listed under the project tree, with no warning icon next to it? If it's shown as a "free document" (not part of any project) or the project needs recompiling, the ECO will look at a stale project compilation that doesn't include your edit.
Fix: Right-click the project name in the Projects panel → Compile Document (or Compile PCB Project), then regenerate the ECO. This forces Altium to re-read every sheet in the project and rebuild its internal netlist/component list before the comparison runs.
2. You edited the sheet from a design that's open in two places at once — e.g. the same project open in two Altium instances, or a linked/copied schematic sheet that exists in more than one project. The ECO diffs against whichever compiled state Altium currently has cached for that project, which may not be the copy you actually typed into.
Given this is your first multi-sheet project, I'd bet on #1. Compile the project first, always, before generating an ECO — I do it as muscle memory now specifically because of this exact failure mode.
Once you get the ECO actually detecting your added components, watch for the next failure mode in the same workflow: "Footprint Not Found" errors in the ECO validation for the new parts specifically. This happens when the schematic symbol's linked footprint isn't resolvable from the PCB library list currently active in this project — common right after adding a part from a manufacturer part search or a library you use on other projects but haven't added to this project's installed library list yet (Design > Add/Remove Library, or the project's library search path if you're not on a vault-managed setup).
Confirm the new component's Footprint parameter in the schematic (right-click → Properties → Footprint tab) actually resolves — if Altium can't find it there either, that's your answer, and it's a library-scope problem rather than an ECO problem. This is exactly the library-centric component model gotcha — a symbol and footprint are independent library entities linked by reference, and a project only sees the footprint if the containing library is actually enabled for that project.
Worth flagging since you mentioned this being your first multi-sheet project: this exact class of problem — "which library is actually active for this project," "is my schematic edit even part of the compiled project" — is the recurring papercut with local/path-based Altium libraries once you're working across more than one project or more than one machine. If you find yourself hitting this a few more times as the project grows, it's worth looking at Altium 365 workspace libraries (vault-managed) instead of local .SchLib/.PcbLib files on a shared drive — the vault resolves the "is this library actually available to this project right now" question centrally rather than per-machine per-project. Not a free lunch — it's a bigger setup investment and a workflow change for the whole team, not just you — but if this becomes a recurring cost across multiple designers, it's the actual fix rather than "remember to compile the project" as a permanent workaround. See the Altium vs KiCad comparison for the fuller trade-off between vault-based and Git-based library management.