Version 3

    Applies to Versions : All

     

    Most software has these little nuances, and they are generally mentioned in documentation, but rarely in a way that would help you understand why it is there, or when you might use it, and human nature causes us to miss these bits when we are first learning… so I wanted to create this Knowledge Article to draw attention to a few of these.  They are not major features, but I sometimes find these little things to be extremely helpful, once you know they exist.

    Always Drag and the CTRL Key

    The default behavior when moving connected objects in Altium CircuitStudio is to “Always Drag” this was enabled by default to match behavior of other tools.  However, this is not the native behavior of Altium Schematic tools so I wanted to use a section here to briefly explain the behavior.

     

    Traditionally Altium\Protel Schematic tools would not default to keep items connected while moving, if you wanted to drag the items and keep them connected you would hold the CTRL key prior to moving.  This traditional behavior is only active if the Always Drag preference is Disabled, so if you are used to, or prefer, this way of working and wish to restore that behavior uncheck the Always Drag preference in the Schematic >> General page of the System Preferences.

     

    While Always Drag is active(Default Behavior), this behavior is toggled. Instead of CTRL invoking a drag command, with Always Drag enabled, the CTRL key instead Suppresses the drag functionality.

     

    Either way, knowing that the CTRL key will toggle this behavior will allow you to better utilize the default behavior you prefer, just in case this was not yet discovered

    Changing defaults during placement

    When initially placing an item, such as a Net Label, a Port, or a Power Object, after you have invoked the command, but before you have placed the item into your design and it is still held on your cursor - Press TAB and alter the properties of the item prior to placement, and this will update the defaults for your next placement.  If you place the object first, then access the properties of the placed item, it will only change that item and the defaults will remain unchanged.

     

    This is good to know for a few reasons

    1. You may have changed a default on accident and not know how it changed
    2. You changed a default, but now want to change it back
    3. You may not like the existing default, and intentionally want to update it to suit your preference

    CircuitStudio TAB to Change Defaults

    Morph tool

    Hovering over an item, while another is held on your cursor, you have the ability to press the Insert key on your Numpad and this will do one of two things.

    1. If you are holding a component, and hovering over another component and press INS the component on your cursor will morph and pick up the properties of the component underneath.

    1. If you are holding a text item such as a Net Label, Port, Power Object, etc and you press INS while hovering over another object, it will pick up the text of that object, without turning into it.  E.g. I can hover a Port over a Net Label and press INS to pick up the text underneath.   This can be very handy when creating ports for a group of signals you plan to pass to another sheet, as seen in the animation here.

     

    Shift+Drag to copy and Increment

    If you hold the SHIFT key, then click and drag on an item, or selection of items, within the Schematic a copy of that object will appear on your cursor, automatically incremented if applicable.  This is a quick and easy way to continue placement of a group of similar objects, in the event you did not do a continual placement and need to add new parts without starting over again from the Library for instance.  Keep in mind that the autoincrement does not check existing designators or values, and duplicates can be created. It’s effectively a copy/paste with an autoincrement and requiring a few less clicks. But handy in a pinch to save a little time here and there if you know it’s available.  Where I find myself using it most often is creating a set of equal length wires, instead of clicking to create each one.

     

     

    Alt+Click on an electrical object for a quick net highlight

    Quick note on ‘dim’ highlighting:

    A ‘dim’ is just a reductive highlight method and does not prevent editing as ‘mask’ does, although they can be difficult to distinguish if your view levels are similar.

    Use the Dim Level slider on the View tab of your ribbon to control the strength of the ‘dim’ effect on the other objects

    Now, back to the ALT+Click highlight…It is important to mention this will only work if your Project has been compiled, so if you have not compiled yet access Home | Project >> Compile   With the Project Compiled hold ALT and Left-click on an electrical item in the Schematic you will dim out all other objects and this will give you a quick graphical highlight and zoom of where that net connects on your current sheet.

    CTRL+Double-click on a Sheet Entry or Port for quick navigation through your hierarchy

    While hovering over a Sheet entry or Port CTRL+Double-click will take you to a corresponding sheet entry, or port on another sheet. You can continue CTRL+Double-click to navigate through the hierarchy.  This will also ‘dim’ other objects to help highlight what you are targeting, but again this will not prevent you from continuing your navigation. 

     

    I hope this is helpful!