Pin Properties

Modified by Susan Riege on Aug 16, 2018
Contents
Other Related Resources
Pin (Object)
Component Pin Editor (Dialog)

Parent page: Sch Dialogs

The Pin Properties dialog

Summary

This dialog provides controls to specify the properties of a Pin object. 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.

Access

The Pin Properties dialog can be accessed during placement by pressing the Tab key.

After placement, the dialog can be accessed in one of the following ways:

  • Double-click on the placed pin object.
  • Place the cursor over the pin object, right-click then choose Properties from the context menu.

Logical Tab

Pin Properties dialog - Logical tab

Use the dialog's Logical tab to modify electrical and graphical properties of the pin object.

Options/Controls

  • Display Name - use this field 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 the provision of a meaningful name enables you to quickly see for what the pin is being used. Note that while the pin name is optional, it is required when the pin is going to be hidden. A hidden pin is automatically connected to other hidden pins with the same name and to nets with the same name when a net-list is created.
    • Visible - use this option to determine whether the Display Name for the pin is displayed (enabled) or hidden (disabled) when the parent part is placed on a schematic sheet.
  • Designator - the numerical identifier of the pin. Each pin in a part must have a unique designator.
    • Visible - use this option to determine whether the Designator for the pin is displayed (enabled) or hidden (disabled) when the parent part is placed on a schematic sheet.
  • Electrical Type - use this field to set the electrical type of the pin. This type is used when compiling a project or analyzing a schematic document to detect electrical connection errors (using the Electrical Rules Check feature). Available types are: Input, I/O, Output, Open Collector, Passive, HiZ, Open Emitter, and Power.
  • Description - use this field to provide an optional description for the pin, perhaps a concise summary of its purpose.
  • Hide - enable this option to hide the pin. This is typically the case for power pins of multi-part components when their display would otherwise cause unnecessary clutter on the schematic sheet.
    • Connect To - use this field to specify the net to which the hidden pin is to be explicitly connected. This is typically a power net, such as VCC or GND.
Hidden pins for a component can be revealed on the sheet in the Schematic Editor or Schematic Library Editor by enabling the Show All Pins On Sheet (Even if Hidden) option in the associated Properties for Schematic Component dialog or Library Component Properties dialog. Alternatively, in the Schematic Library Editor, the display of hidden pins can be toggled by clicking Tools | Options | from the main menus.
  • Part Number -  this field is available when the pin is being added to a multi-part component. Use the associated up/down arrows of the field 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.
For a multi-part component, the power net connections should ideally be assigned through use of Part Zero. For each pin that is required to connect to a power net in this way, enable the Hide option, leave the Connect To field blank, and set the Part Number field to 0.
  • Preview Window - this area of the dialog provides instant visual feedback as you change various options enabling you to adjust the look and feel of the pin to meet design requirements.

Symbols

Use this area of the dialog to add additional symbols to the pin. Such symbols can be used to visually enhance the component by showing, in a purely graphical way, the electrical characteristic of the pin.

  • Inside - use this field to optionally add a symbol to the pin on the inside of the component graphic. Choose from: No Symbol, Postponed Output, Open Collector, HiZ, High Current, Pulse, Schmitt, Open Collector Pull Up, Open Emitter, Open Emitter Pull Up, Shift Left, and Open Output.
  • Inside Edge - use this field to optionally add a symbol to the pin on the inside edge of the component graphic. Choose from: No Symbol and Clock.
  • Outside Edge - use this field to optionally add a symbol to the pin on the outside edge of the component graphic. Choose from: No Symbol, Dot, Active Low Input, and Active Low Output.
  • Outside - use this field to optionally add a symbol to the pin on the outside of the component graphic. Choose from: No Symbol, Right Left Signal Flow, Analog Signal In, Not Logic Connection, Digital Signal In, Left Right Signal Flow, and Bidirectional Signal Flow.
These symbols are purely graphical. The true electrical property of the pin is determined by the entry set for the pin's Electrical Type.
  • Line Width - use this field to determine the width of the line used to draw the symbols. Choose from either Small or Smallest.

Graphical

  • Location X/Y - the current X (horizontal) and Y (vertical) coordinates for the non-electrical end of the pin (the end that is placed against the component symbol's outline). Edit these values to change the position of the pin in the horizontal and/or vertical planes respectively.
  • Length - use this field to specify the length of the pin in accordance with the currently defined units of measurement.
  • Orientation - specify the orientation of the pin counter-clockwise in relation to the horizontal. Options available are: 0 degrees, 90 degrees, 180 degrees, 270 degrees.
  • Color - click the color sample to change the color of the pin using the standard Choose Color dialog.
The Color option affects all graphical aspects of the pin - its line, its Display Name, its Designator, and any additional pin symbols (Inside, Inside Edge, Outside Edge, Outside). The Display Name and Designator colors can, however, be changed independently using the respective Use local font setting control.
  • Locked - enable this option to protect the pin from being edited graphically.
An object that has its Locked property enabled cannot be selected or graphically edited. Double-click on the locked object directly then disable the Locked property to graphically edit the object.

Name Position and Font

  • Customize Position - enable this option to change from following the default settings for position of the pin's Display Name to an overriding, customized position.
    • Margin - use this field to enter the required margin (space) between the pin's Display Name text and the edge of the component symbol outline.
    • Orientation - use this field to choose the orientation of the pin's Display Name text (0 Degrees or 90 Degrees).
      • To - use this field to set the reference point for orientation of the Display Name text. Choose from either Pin or Component.
With the Customize Position option disabled (default), the position of the pin's Display Name follows the default settings for Margin (5) and Orientation (0 Degrees To Pin). The value for the Margin is taken from the corresponding entry on the Schematic – General page of the Preferences dialog.
  • Use local font setting - enable this option to change from following the default font to an overriding, customized font using the font control to the right. This control serves two purposes. First, it reflects the currently chosen font – applied to the pin's Display Name text - in terms of Font Name, Font Size and Font Style. Second, when clicked it provides access to the standard Font dialog in which you can change the font as required.
By default, and for a component placed on a schematic sheet, the font used for the pin's Display Name text follows the document-level font set on the Sheet Options tab of the Document Options dialog (Project | Content | ).
Effects are also displayed when enabled (Strikeout, Underline). If Regular is used for the font's style, this will not be displayed visually in the control's string.

Designator Position and Font

  • Customize Position - enable this option to change from following the default settings for position of the pin's Designator to an overriding, customized position.
    • Margin - use this field to enter the required margin (space) between the pin's Designator text and the edge of the component symbol outline.
    • Orientation - use this field to choose the orientation of the pin's Designator text (0 Degrees or 90 Degrees).
      • To - use this field to set the reference point for orientation of the Designator text. Choose from either Pin or Component.
With the Customize Position option disabled (default), the position of the pin's Designator follows the default settings for Margin (8) and Orientation (0 Degrees To Pin). The value for the Margin is taken from the corresponding entry on the Schematic – General page of the Preferences dialog.
  • Use local font setting - enable this option to change from following the default font to an overriding, customized font using the font control to the right. This control serves two purposes. First, it reflects the currently chosen font – applied to the pin's Designator text - in terms of Font Name, Font Size and Font Style. Second, when clicked it provides access to the standard Font dialog in which you can change the font as required.
By default, and for a component placed on a schematic sheet, the font used for the pin's Designator text follows the document-level font set on the Sheet Options tab of the Document Options dialog (Project | Content | ).
Effects are also displayed when enabled (Strikeout, Underline). If Regular is used for the font's style, this will not be displayed visually in the control's string.

Parameters Tab

Pin Properties dialog - Parameters tab

Use the dialog's Parameters tab to manage parameters attached to the currently selected pin object. You can also add rule-based parameters.

Adding a parameter (as a rule) to a component pin on the schematic results in a PCB design rule being generated when the design is transferred to the PCB document with a scope that targets the corresponding Pad for that component.

Options/Controls

  • Parameters Grid - the main region of the tab lists all of the parameters currently defined for the pin in terms of:
    • Visible - use this option to determine the visibility of the parameter's value in the workspace. Note that this does not relate to the visibility of the parameter's Name, which can be determined for a standard (non-rule) parameter only in the Parameter Properties dialog.
    • 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.
    • Type - the type of parameter, which determines the valid entries that can be used for its value. Available types are: STRING, BOOLEAN, INTEGER, and FLOAT. For a rule-type parameter, this entry is always STRING.
A standard parameter (non-rule) can be modified with respect to any of these attributes directly in the grid. However, attempting to change a locked Name and/or Value attribute will raise an error and you will need to press Esc to abandon such changes.
A parameter added as a rule cannot be edited directly in the grid with respect to its Name, Value, or Type. Its Name and Type are set to Rule and STRING respectively, and are always un-editable. Its Value can only be edited by changing the constraints of the rule. To do this, select and edit the parameter then click the Edit Rules Button in the Parameter Properties dialog. This will give access to the Edit PCB Rule (From Schematic) dialog in which the changes to the constraints can be made.
  • Add - click this button to add a new parameter to the list. The Parameter Properties dialog will open. Use this to define the parameter, especially its Name, Value, Type, and whether or not its value is to be visible in the workspace.
  • Remove - click this button to delete the selected parameter(s) from the list of parameters.
  • Edit - click this button to open the Parameter Properties dialog to modify the currently selected parameter.
  • Add as Rule - click this button to add a new design rule directive parameter to the list. The Parameter Properties dialog will open, but this time will contain the Edit Rule Values button, which in turn gives access to the Choose Design Rule Type dialog in which you can choose, and subsequently define, the constraints of the required rule type.

Right-click Menu

The Parameters Grid right-click menu offers the following commands:

  • All On - use this command to quickly enable the Visible option for all parameters in the list.
  • All Off - use this command to quickly disable the Visible option for all parameters in the list.
  • Selected On - use this command to quickly enable the Visible option for all currently selected parameters in the list.
  • Selected Off - use this command to quickly disable the Visible option for all currently selected parameters in the list.
  • Add - use this command to add a new standard (non-rule) parameter to the list.
  • Remove - use this command to remove the currently selected parameter(s) in the list.
  • Edit - use this command to edit the currently selected parameter in the list.
  • Select All - use this command to quickly select all parameters in the list.
  • Select None - use this command to quickly deselect all parameters in the list.

 

You are reporting an issue with the following selected text and/or image within the active document: