Altium Help & Tips

This page contains a few random notes on how to use Altium.  This page isn’t intended to be a tutorial – they are just my personal notes. You can find a tutorial here.

Feel free to email me if you have a question.

  • Creating Gerber, Drill files & Pick and Place
    • File –> Fabrication Outputs –> Gerber Files
    • File –> Fabrication Outputs –> NC Drill Files
      • Verification of hole placement (Camtastic)
        • File –> Import –> Drill . . . (overlays holes on gerber files for visual spot check)
    • File –> Assembly Outputs –> Generate Pick and Place Files
  • Update Free Primitives From Component pads
    • Problem:   You’ve created your own footprint and used a sheet of copper over pins or vias. When placed in the PCB layout green error markers indicate a short circuit
    • Solution:  From the PCB Layout
      Design –> Netlist –> Update Free Primitives From Component pads . . .
  • Hiding and Displaying Rats Nest
    • View –> Connections –> Show All
    • Hide GND net:   View -> Connections -> Hide Net
  • No connection lines visible or on (ratsnest or nets aren’t showing)
    • Go to Design –> Board Layers & Colors… (can also press L or double click at bottom left of layout view where it says LS) and then make sure all layers are on.
  • Only GND connection lines (ratsnest) are missing ( View –> Connections –> Show All  doesn’t work)
    • If one of the internal planes has been set to GND then GND vias will not show a GND connection line or “ratsnest” (as it should be – since they’re connected)
    • A polygon pour assigned to GND has been shelved (turned off to make layout easier to see) resulting in the appearance of missing GND nets – when really the connection is already made – and hence no GND connection line.
  • Break snippet union
    • Problem: when attempting to drag a single component by holding the left mouse button and dragging more than one component will drag.
    • Solution (break snippets union):
      • Highlight the affected components
      • Right click and select Unions –> Break Object from Union
      • In the Confirm Break Objects Union dialog uncheck all components (or leave checked what you’d like to remain in the union).
      • click OK
  • Can’t rotate multiple components using the spacebar (while dragging multiple selected parts with mouse)
    • settings –> Schematic –> Graphical Editing –> (uncheck) Aways Drag
    • “Always Drag” when checked keeps connections/nets together on the schematic if you move a placed part that is already connected to some other part – the wires/nets ‘stretch’ if you move the part.  Unfortunately, this prevents rotating multiple objects with the spacebar.   Therefore, uncheck Always Drag in settings.  The good news is that you can still use the Always Drag feature when you want it by using the ctrl key while moving a part – if you want the wires to remain connected.
    • There is another way to rotate multiple parts with Always Drag checked.  Instead of selecting multiple parts, then dragging with your mouse and finally attempting to rotate using the spacebar- you can select multiple parts and then use the space bar to rotate before dragging.   However, my personal work flow usually includes rotation of parts while dragging – so I prefer to uncheck Always Drag.
  • Create Union (in PCB)
    • Tools>Convert>Create Union from selected objects
  • Specific No ERC directive (for suppression of schematic compile error messages)
    • Problem:  When placing the Specific No ERC directive on the schematic (Using: Place –> Directive –> Specific No ERC) the resulting Place Specific NoERC dialog box indicates no errors existed even after pressing the Recompile project button.
    • Solution: place a Generic No ERC, then double click and configure. A list of specific errors will appear after clicking the Suppress Specific Violations (select to choose) radio button.  Check those errors and warnings you wish to suppress.
  • Need to change net name for existing route
    • Edit » Select » Connected Copper command (Ctrl+H)
    • Then use the PCB inspector to change the net name.
  • When annotating multi-part components get moved around (parts swapped).
    • Can be prevented by checking the Lock Part ID box (double click on the part)
  • Adding a Miter (RF bends)
    • first select the tracks that you wish to have RF miters (or select connected coper using  edit –> select –> connected copper).  Then select:
      tools –> convert –> Convert Selected Tracks to Chamfered Path
      (Seems to work only with 90 degree bends)
  • Unions
    • When importing a critical layout (such as a microwave filter) into the PCB it can be very beneficial and convenient to create a union – to group all the constituent parts making up the critical circuit.  First, highlight all objects (usually metal layers) and then select:
      Tools –>  Convert –>  Create Union from selected objects
  • Units (PCB)
    • design –> board options
    • press the “Q” key to change units.
  • Measuring Length of a line
    • ctrl-H will select connected copper
    • reports –> Measure Selected Coper
  • Change net of connected copper (routed track)
    • ctrl-H –> select copper –> press esc
    • F11 to bring up the PCB inspector
  • Title Bock Parameters
    • Design –> Document Options is is where you set variables to be used in the title block.
    • Project –> Project Options, select the Parameters Tab.  This is where you create variables to be used in the title block (and probably other places as well)
  • Number Schematic Sheets
    • Tools –> Number Schematic Sheets…
  • If you’ve accidentally tiled every window (Example: you have 20 windows open and they all got tiled into tiny squares  on your screen & you just cannot figure out how to undo the mess)
    • Support has informed me that right clicking on a tab (schematic, pcb, etc.) and selecting Merge All will make things better again.  I haven’t tested this (I closed every project and re-opened).   But, you may want to leave all projects open – in which case Merge All is supposed to work.
  • Rules – Importing & Exporting
    • From PCB editor Design –> Rules then right-click “design rules” at the top of the tree and select Export Rules…  The “Choose Design Rule Type” menu/dialog appears
    • Highlight rules you wish to export/import from the click okay.  Next you save the file *.RUL to where ever you like.  ☺︎
  • Grids not showing in Layout
    • Check the following
      • Make sure that “Default Grid Color – Small” and “Default Grid Color – Large” are checked in the View Configurations dialog.   Design–>Board Layers & Colors…    ( or use the keyboard shortcut key – L )
      • Make sure that you’re not zoomed out too far (grids turn off when they get tiny)
      • Make sure you’re viewing in the defined PCB area and not outside of it.  Altium places rooms outside the defined board area.  You can layout your design outside of the board area if you want – but there aren’t any girds outside of the board area.
  • BOM Generation using Output Jobs
    • File –> New –> Output Job File  (or right click on project and select Add New to Project –> Output Job File)
    • The Outputs menu appears: Under Report Outputs click the little arrow –> bill of materials –> [Project]
    • Name the Bill of materials (something like Assembly BOM, Cost BOM, etc.) – then double click to bring up the parameters/BOM data.  Here you select Grouped Columns, and add needed columns.  I group using the following: Supplier Part Number 1, Value, Comment, Footprint.
    • Choose an Excel Template (link to an existing Excel template)
    • Select/highlight the PDF under the Output Containers, next clicked the little round radio button under Enabled on the same light as the Report Output you just created.
    • Printing in color:
      • 1) Open the Output Job file
        2) Right-click on your Schematic Prints output
        3) Select “Page Setup…”
        4) Choose[Color] for your “Color Set”
        5) Click [Close] to accept the changes
  • Printing same size PDF (Output Jobs)
    • right-click and select “Page Setup..” and slepect fromdropdown under printer paper (example select letter)  Located Under Outputs locate each item slated for printing (usually Schematics & PCB under Documentation and Report Outputs for the BOM)
    • select Change –> Advanced – located under output container (where you see the little pdf icon).  Then page size and orientation select page setup dialog
  • Adding additional BOM items (external to the PCB)
    • How to add items such as AC to DC power adaptors, screws, fasteners, plastic standoffs to the BOM
    • Create as schematic symbol as you would with any regular component and be sure to select under Properties  Type –> Mechanical
    • Now all of these items will show up in the BOM.
  • Copying a project from existing
    • DO NOT use save as.  (I’ve already made that mistake before)
    • File –> New Project  – name the project, if the “Create Project Folder” is checked then a directory with the same name as “Name” above will be created.
    • Next copy the schematic files and PCB files to the newly created directory (*.PcBDoc and *.SchDoc) – it probably makes good sense to also rename these files at the same time.
    • Now, right click on project tree and select “Add Existing to Project”
  • Fractal Panels (panel split vertically)
    • Sounds like this is a bug of some sort.  The problem is that the panels on the left get split.  Instead of having all of your panels extened the full vertical height and on top of each other (tabbed).  They split so that one panel occupies the upper portion while the rest sit at the bottom. Although this allows for two panels to be seen at the same time you also lose vertical height of the visible panels.  I think most people do not wish to truncate the vertical height.  Another problem is that once you get the panels straightened out – they revert back to this unwanted state as you switch between the PCB editor, Schematic editor, and libraries. <– This is a known problem with the developers.  It goes round and round like that which can be very aggravating – having to constantly fuss with panels while trying to remain focused on your work.  Adding to the annoyance, in my case, was that I did not know how to re-adjust these panels (yet, needed to address the issue immediately since I’m working). I’d fumble around quite a lot trying to get all panels on top of each other and tabbed.  What a PITA!  After getting help through the Altium forum and a phone call to Altium I have learned the following:
      • When a panel is split vertically – right-click when the mouse cursor is over the letters of the panel (at the top of that panel) then yank that panel out.  After doing so insert the panel as a tab by mousing near the tabs at the bottom – you’ll see a little triangle appear indicating you are about to insert (easier to show a picture I suppose ).
      • You can rip a panel out by holding shift and right-click over the bar.  Or, as described above right-click over the letters and drag to remove a particular panel.
      • Desktop Layouts can be saved or loaded.  So, once you have your panels the way you like save them.  If the panels get split again you can load the previously good state.   View –> Desktop Layout –> Save Layouts
  • Keep schematic wires locked to components/nodes (Always Drag)
    • DXP –> Preferences –> Schematic –> Graphical Editing –> Always Drag
  • Turn off Auto Pan (when placing a component the schematic will pan automatically)
    • DXP –> Schematic –> Graphical Editing –> Style –> Auto Pan Off
  • Rooms – What are they for?
    • Good for local rules (example: logo with extremely skinny lines that trigger an DRC error – if sequestered to a room separate rules can be made)
    • Multichannel – copying
  • Hide Room
    • Press the L key –> View Configurations –> Show/Hide –> Hidden
  • Clicking DRC error (messages window) adjust zoom
    • PCB –>  PCB Rules and Violations –> Zoom Level . . .