Altium Designer Tips

Note [PCB+SCH] means command is available in PCB and Schematic mode, [PCB] means it is only available in the PCB editor. View » Desktop Layouts » descrives navigating the _View menu.

You Favorite Keyboard Shortcuts

  • [PCB+SCH] Space to rotate components, change routing orientation

  • [PCB+SCH] Tab to change properties of the component you are placing

  • [PCB+SCH] Page Up/Down zooms in and out of the design

  • [PCB+SCH] Ctrl+Mousewheel zooms in/out

  • [PCB+SCH] Shift+Mousewheel pans left/right

  • [PCB+SCH] Hold Shift while dragging, makes Altium pan faster.

  • [PCB] Ctrl+D Snaps components to the grid, making it easier to align them. If you move multiple components at once, the will probbably result in the being all off the grid.

  • [PCB] Ctrl+Click on a net highlights everything connected to that net

  • [PCB] Q switches between metric and imperial units

  • [PCB] P open the place menu, P __» __T starts the interactive routing tool

  • [PCB] +/- change the routing layer, inserting a via in accordance with your current design rules.

  • [PCB] Ctrl+M measures the distance between two points

  • [PCB] L brings up the layer dialog for showing and hiding the different board layers

General Environment Tips

  • You can reposition all of the Altium panels, windows, etc. After you have it the way you like save it. View » Desktop Layouts » Save Layout. If you mess it up, reset to the default layout View » Desktop Layouts » Default

  • Learn the keyboard shortcuts.

  • Cross probing is the process of selecting a component in either the schematic, or PCB editor and Altium will locate and/or select their PCB or Schematic counterparts. The easiest way to do this is to use Tools » Cross Probe and select the relevant component.

  • The inspector is the way to edit the same parameters on multiple components simultaneously, for example, you would use the inspector to change the footprint on all your resistors.

    • Ensure the inspector panel is visible in SCH/PCB. View » Workspace Panels » SCH/PCB » SCH/PCB Inspector

  • The inspector requires the components you wish to modify be selected. The easiest way to select multiple components is to start by Finding Similar objects.

    • Right click on one of the components you wish to modify, select Find Similar

    • In the window which pops up, change Any to Same on fields describing those components you wish to select.

    • Ensure Run Inspector is ticked and click OK.

    • The Inspector panel will now feature a number of fields which you may edit. Changes to these fields will be applied to all selected components.

  • Use The Help

    • [PCB] Ctrl + F1 while moving/routing a component will show you relevant key strokes

    • [PCB+SCH] F1 over an object/panel will show you relevant help

  • Use The Design Rules

    • From the PCB select Design » Rules. You should set rules in accordance with the capabilities of the manufacturer who will be making the PCB. At a minimum, ensure there are sensible values for the Routing » Width and Electrical » Clearance rules.

PCB Routing Tips

  • If you are overwhelmed by the number of connections when routing a PCB, and you intend to pour a ground plane, you should hide the GND net. View » Connections » Hide Net

  • If your board features a few polygon planes, such as ground planes, it is easier to manage them through Tools » Polygon Pours » Polygon Manager. Multiple pours on many layers slow down Altium and make routing hard. Shelve polygons to alleviate this.

  • If you become overwhelmed by the complexity of components on multiple layers, try single layer mode, Shift+S (which hides everything except that on the current layer).

Schematic Tips

  • Give the nets meaningful names (these names will appear in the PCB document and this will aid placement and routing)

  • When you add a new component, give it a designator that is not currently in use. The easiest way to do this is use the Tools » Annotate » Update Changes List » Accept and Create ECO. However be careful, if you are deleting one component, and adding another, with the same designator Altium can get confused.

  • When a component pin, port or power port is butted up to a pin of another component it makes an electrical connection. Using the command Edit » Move » Drag, or holding Ctrl when clicking and dragging, and moving either of the objects a wire is automatically placed between the objects

Those Oh My God What Have I Done Moments

  • OMG I can't click on anything and all the components are grayed out You probably have a mask set. Clear the mask by selecting Clear in the bottom right corner of the window.

  • The most common reason for being unable to import changes from the schematic editor to the PCB is because you have forgotten to give components a valid designator (i.e. it still is suffixed with a ?), or the footprint for a component can not be found.

  • When you import changes from the schematic editor to the PCB you will often see Failed to Match .... Components Using Unique Identifiers. Normally this is because you have copy and pasted components, moving them between sheets for example. In this case the warning is harmless (you should make it go away by matching the SCH and PCB components in Project » Component Links window). It can however be a sign that you have made a mistake in the schematic (see explanation above).

Note: Some page content has been adapted from http://www.eda.co.uk/techwatch.htm