Altium designator alignment not working — causes, fixes, and DFM notes

Designator alignment in Altium typically fails because the strings aren’t actually selected, they’re locked or set to Auto-position, or the Align command is run in the wrong editor; fix it by selecting the designator strings, unlocking and setting Auto-position to Manual, then using Edit > Align in the PCB editor.

Why Altium refuses to align designators?

• Nothing is selected, or the selection filter excludes Text/Strings (the Align menu operates only on the current selection)

• You’re in the wrong context (e.g., Draftsman or Library) or 3D view; board designator positions can only be aligned in the PCB editor 2D view

• The designator strings (or their parent components) are Locked or component primitives are locked

• Auto-position is enabled on designators, so Altium repositions them after you align

• You tried to align mixed objects (tracks, regions, text); align works on the selected set’s bounding boxes and may appear to do nothing if text isn’t part of the selection

Use the correct align command in PCB editor

In the PCB editor (2D view), Align is under Edit > Align (Left, Right, Horizontal Centers, Top, Bottom, Vertical Centers, Distribute, etc.). First ensure you’ve selected only designator strings. The reliable way is to use the PCB Filter: open the PCB Filter panel and enter the query IsDesignator to select all designators, or right‑click a designator > Find Similar Objects…, set Text Kind = Designator and Select = True. With the strings highlighted, run Edit > Align and choose the required option. If Align is greyed out, nothing eligible is selected or you are not in the PCB editor.

Step-by-step to fix alignment not working

Switch to PCB editor 2D view. Select your target designators via PCB Filter (IsDesignator) or Find Similar Objects. Open the Properties panel for the selection and uncheck Locked. In the same panel, set Auto-position (sometimes shown as Autoposition) to Manual so Altium stops moving them after rotations or ECOs. If components prevent edits, momentarily unlock the component or enable editing of placed component primitives, then re-apply the align command from Edit > Align. Finally, if designators seem to snap off-grid, lower the snap grid (for example, 0.05 mm or 2 mil) and retry alignment so bounding-box math lands on your grid.

How to keep Altium from re-moving designators?

Auto-position is the usual culprit. With the designators selected, set Auto-position = Manual in the Properties panel so they stay where you place them. If you have library components that force auto-position, update those library settings and recompile, or override on the PCB after placement. Also avoid batch operations that reset strings (for example, certain ECOs can re-apply defaults); verify after such operations that Auto-position remains Manual.

Batch edits with Filter, Inspector, and PCB List

For large boards, combine the PCB Filter with the Inspector/PCB List panels. Filter with IsDesignator and optionally layer scoping (e.g., IsDesignator And OnTopLayer). In the Inspector you can clear Locked for all selected strings, change Justification (e.g., Center-Top), toggle Keep Upright, and set Text Height and Width in one pass. The PCB List view can also edit X/Y for exact rows/columns if you need strict grid alignment; sort and fill values to impose uniform spacing, then run Edit > Align > Distribute to regularize gaps.

Silkscreen sizing that survives fabrication

Even if Altium alignment works, designators can be clipped by solder mask expansion or silkscreen-to-copper clearance during CAM. Use practical, fab-proven legend sizes: text height 1.0–1.5 mm (40–60 mil), stroke width ≥0.15 mm (6 mil). Maintain at least 0.20 mm (8 mil) clearance from pads and solder mask openings so the CAM cleaning step doesn’t trim characters. If you must go smaller, prefer 1.0 mm height with 0.12 mm stroke and add more clearance margin; always check the Gerber preview to confirm no overlaps before release.