Parent page: Schematic Objects
A pin is an electrical design primitive. Pins give a component (part) its electrical properties and define the connection points on the part for the incoming and outgoing signals.
Pins can only be placed in the Schematic Library Editor. Use one of the following methods to place a pin:
After launching the command, the cursor will change to a cross-hair and you will enter pin placement mode. Placement is made by performing the following sequence of actions:
Additional actions that can be performed during placement – while the pin is still floating on the cursor, and before the electrical end of the pin is anchored – are:
Pins can also be added through the Component Pin Editor dialog, which is accessed via the Edit Pins button in the Library Component Properties dialog.
Click the Add button to add a new pin, then define the properties in the dialog. Note that multiple pins can be added and defined. You can also use Tab and Shift+Tab to step between the fields. When you click OK to close the dialog, the new pin(s) are placed on the sheet to the bottom right of the component, ready to be positioned.
For many components there will be a series of pins that have numerical names and numbers. The auto-increment feature can be used to speed the placement of these pins. Auto-increment is invoked automatically if the pin properties are edited before placement (press Tab while the pin is floating on the cursor). The feature works for both the Designator and the Display Name - the pin Designator uses the Primary auto-increment field and the pin Display Name uses the Secondary auto-increment field. It supports ascending alpha and numeric values, and descending numeric values.
To move a pin, click and hold on it - the cursor will jump to the electrical hotspot end of the pin - then move it to the new location, placing it with the electrical end away from the component body.
While dragging, the pin can be rotated (Spacebar/Shift+Spacebar) or mirrored (X or Y keys to mirror along the X-axis or Y-axis respectively).
Dialog page: Pin Properties
This method of editing uses the Pin Properties dialog to modify the properties of a pin object.
The Pin Properties dialog can be accessed prior to entering placement mode, from the Schematic – Default Primitives page of the Preferences dialog. This allows the default properties for the pin object to be changed, which will be applied when placing subsequent pins.
During placement, the dialog can be accessed by pressing the Tab key.
After placement, the dialog can be accessed in one of the following ways:
The location of the pin Display Name and pin Designator (number) is defined globally by the Pin Margin settings on the Schematic - General page of the Preferences dialog. This is an environment setting, meaning it applies for the PC where the setting is defined. The settings define a relative distance the text is away from the non-electrical end of the pin.
The font used for the pin Display Name and pin Designator (number) - for a component placed on a schematic sheet - is defined at the document level in the Document Options dialog. Click the Change System Font button to set it.
For pins, these system-level settings of position and font can be overridden locally. Controls for customization of the position and font for a pin's Name and Designator can be found on the Logical tab of the Pin Properties dialog when editing a pin in either the Schematic Library or Schematic Editor. While the controls themselves are the same for both attributes, separate sets of controls allow them to be customized independently of each other.
Use the Customize Position option to change the default settings for position to an overriding, customized position. For the Margin, enter a new value directly in the associated field. For the Orientation, use the drop downs to choose the angle (
0 Degrees or
90 Degrees) and the reference (
Use the Use local font setting option to change from following the default system font, to an overriding, customized font. To do so, simply click on the font control to the right of the option to access the standard Font dialog. The control doubles as a notification for the font currently chosen, or 'in-force'.
When representing a component in the schematic editing domain, each pin defined as part of that device's schematic symbol can have one or more symbols displayed. These are symbols displayed on the Inside, Inside Edge, Outside, or Outside Edge, in relation to the main component symbol outline, as required. Examples might include a Clock symbol on the Inside Edge, or a Dot symbol on the Outside Edge. Such symbols greatly improve the readability of the design through visual indication of the purpose of the signal traversing a particular pin.
Use the Line Width property - available in the Symbols region of the Pin Properties dialog - to determine the width of the line used to draw these symbols. Choose from either Small or Smallest.
An Inspector panel enables the user to interrogate and edit the properties of one or more design objects in the active document. Used in conjunction with appropriate filtering - by using the applicable Filter panel or the Find Similar Objects dialog - the panel can be used to make changes to multiple objects of the same kind, from one convenient location.
A List panel allows the user to display design objects from one or more documents in tabular format, enabling quick inspection and modification of object attributes. Used in conjunction with appropriate filtering - by using the applicable Filter panel or the Find Similar Objects dialog - it enables the display of just those objects falling under the scope of the active filter – allowing the designer to target and edit multiple design objects with greater accuracy and efficiency.
Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.