Configuring Schematic Library Pin Object Properties in Altium Designer

Parent page: Pin

Schematic Library Editor object properties are definable options that specify the visual style, content and behavior of the placed object. The property settings for each type of object are defined in two different ways:

• Pre-placement settings – most Pin object properties, or those that can logically be pre-defined, are available as editable default settings on the Schematic – Defaults page of the Preferences dialog (access from the button at the top-right of the design space). Select the object in the Primitive List to reveal its options on the right.

• Post-placement settings – all Pin object properties are available for editing in the Properties panel when a placed Pin is selected in the design space.

General Tab

Location (Properties panel only)

• (X/Y) 
  • X (first field) – the current X (horizontal) coordinate of the reference point of the object, relative to the current design space origin. Edit to change the X position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default.
  • Y (second field) – The current Y (vertical) coordinate of the reference point of the object, relative to the current origin. Edit to change the Y position of the object. The value can be entered in either metric or imperial; include the units when entering a value whose units are not the current default.
• Rotation – use the drop-down to select the rotation.

Properties (Properties panel only)

• Designator – the numerical identifier of the pin. Each pin in a part must have a unique designator. Use or to determine whether the Designator for the pin is displayed or hidden (respectively) when the parent part is placed on a schematic sheet.
• Name – use to specify an optional display name for the pin. By default, a newly placed pin will be named using the designator value. Supplying a display name is particularly useful for IC-type components where a meaningful name enables you to see quickly how the pin is being used. Use the eye icon to determine whether the Name for the pin is displayed or hidden when the parent part is placed on a schematic sheet.​
• Electrical Type – use the drop-down to set the electrical type of the pin. This is used when compiling a project or analyzing a schematic document to detect electrical connection errors (using the Electrical Rules Check feature).
• Description – enter a meaningful description of the pin, if desired.
• Pin Package Length – enter the pin-package length. The unit will automatically be entered after you press Enter.
• Propagation Delay – this field lists the propagation delay, which is the amount of time it takes for the head of the signal to travel from the sender to the receiver.
• Part Number – this field is available when the pin is being added to a multi-part component. Use the up/down arrows to specify the part to which the pin is to be associated. A multi-part component also includes a non-graphical part, Part Zero. Part Zero is used for pins that are to be included in all parts of the multi-part component, for example, power pins.
• Pin Length – use to specify the length of the pin in accordance with the currently defined units of measurement. Click the color box to edit the color of the pin.

Symbols (Properties panel only)

• Inside – use to optionally add a symbol to the pin on the inside of the component graphic.

• Inside Edge – use to optionally add a symbol to the pin on the inside edge of the component graphic.
• Outside Edge – use to optionally add a symbol to the pin on the outside edge of the component graphic.
• Outside – use to optionally add a symbol to the pin on the outside of the component graphic.
• Line Width – use this field to determine the width of the line used to draw the symbols. This provides support for meeting GOST standards, which stipulates that these symbols should be of the same width as the line used to draw the component's symbol.
  The Line Width setting will also apply to the automatic symbol used in relation to the pin's defined Electrical Type.

Font Settings (Properties panel only)

• Designator
  • Custom Settings – enable to access the Font Settings below to customize the font.
  • Font Settings – use the controls to configure the font, font size, color, and special settings such as bold and underlining.
  • Custom Position – enable to access the controls below to customize the position.
  • Margin – enter the desired margin.
  • Orientation – use the drop-down to select the orientation.
  • To – use the drop-down to select the desired object of the designator.
• Name
  • Custom Settings – enable to access the Font Settings below to customize the font.
  • Font Settings – use the controls to configure the font, font size, color, and special settings such as bold and underlining.
  • Custom Position – enable to access the controls below to customize the position.
  • Margin – enter the desired margin.
  • Orientation – use the drop-down to select the orientation.
  • To – use the drop-down to select the desired object of the name.

Parameters Tab

Parameters  (Properties panel only)

Use this region to manage parameters attached to the currently selected pin object.

• Grid – this region lists all of the parameters currently defined for the pin. Use the  icon to lock/unlock the associated parameter.
  • Name – the name of the parameter. For a rule-type parameter, this entry will be locked as Rule.
  • Value – the value of the parameter. For a rule-type parameter, the entry will reflect the rule type along with a listing of its defined constraints.
• Font – click to open a menu to select the desired font, font size, color, and attributes to bold, italicize, etc., if desired.
• Other – click to open a drop-down to change additional options:
  • Show Parameter Name – enable to show the parameter name within the Schematic Library editor.
  • Allow Synchronization with Database – enable to synchronize with the database. This option is used to control if the comment can be updated. By default, these options are enabled to always allow synchronization with the source library/database. You may disable this option to prevent that comment from being included in an update process.
  • X/Y – enter the X and Y coordinates desired.
  • Rotation – use the drop-down to select the rotation.
  • Autoposition – check to enable auto-positioning, meaning that the text will remain in the chosen position as the component is moved and rotated.
• Add – click to add a parameter. Use  to delete the currently selected parameter.