Search In: Doc:Documentation: NEXUS Client
Altium DesignerAltium 365Altium MCAD CoDesignerAltium CircuitMakerCompany DashboardAltium On-Prem Enterprise ServerAltium Infrastructure Server
Ver: Version: 3.2
543.23.13.02.12.01.11.0
Close
Suche Search on Documentation
Documentation Altium NEXUS Documentation ... ((Dialog Reference))_AD Dialogs((M to R))_AD

Sch_Dlg-PinPropertiesDialogPin Properties_AD

Created: Juli 10, 2017 | Updated: März 06, 2024 | Applies to versions: 1.0, 1.1, 2.0, 2.1, 3.0, 3.1, 3.2, 4 and 5
Now reading version 3.2. For the latest, read: Sch_Dlg-PinPropertiesDialog((Pin Properties))_AD for version 5

This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer and a connected Altium 365 Workspace. Check out the FAQs page for more information.

The Pin Properties dialog The Pin Properties dialog

Summary

This dialog allows you to specify the properties of a Pin object. A pin is an electrical design primitive and gives a component (part) its electrical properties and defines the connection points on the part for the incoming and outgoing signals.

Access

The Pin Properties dialog can be accessed by clicking the Edit button in the Component Pin Editor dialog.

Logical Tab

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

The Logical tab of the Pin Properties dialog The Logical tab of the Pin Properties dialog

Options/Controls

  • Display 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 quickly see for how the pin is being used. Note that while the pin name is optional, it is required when the pin is 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 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 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 the drop-down to set the electrical type of the pin. The electrical 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 to provide an optional description for the pin, perhaps a concise summary of its purpose.
  • Hide - enable to hide the pin. This is typically the case for power pins of multi-part components where their display would otherwise cause unnecessary clutter on the schematic sheet.
    • Connect To - use 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 option in the Pins region of the Properties panel. 
  • 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.
For a multi-part component, the power net connections should ideally be assigned through the 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 region to add additional symbols to the pin. These symbols can be used to visually enhance the component by showing, in a purely graphical way, the electrical characteristic of the pin.

  • Inside - use 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 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 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 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. 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.

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.
  • Length - use to specify the length of the pin in accordance with the currently defined units of measurement.
  • Orientation - specify the orientation of the pin, counterclockwise in relation to the horizontal. Options available are: 0 Degrees, 90 Degrees, 180 Degrees, and 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 - line, Display Name, 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 in the Designator Position and Font region.
  • Locked - enable this option to protect the pin from being edited graphically.
If attempting to graphically modify an object that has its Locked property enabled, a dialog will appear asking for confirmation to proceed with the edit. If the Protect Locked Objects option is enabled on the Schematic – Graphical Editing page of the Preferences dialog, and the Locked option for that design object is enabled as well, then that object cannot be selected or graphically edited. Double-click on the locked object directly and disable the Locked property or disable the Protect Locked Objects option to graphically edit the object.

Name Position and Font

  • Customize Position - enable to change from following the default settings for position of the pin's Display Name to an overriding, customized position.
    • Margin - use to enter the required margin (space) between the pin's Display Name text and the edge of the component symbol outline. The Customize Position option must be enabled to access this option.
    • Orientation - use to choose the orientation of the pin's Display Name text (0 Degrees or 90 Degrees). The Customize Position option must be enabled to access this option.
      • To - use 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 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 Font set in the General region of the Properties panel in Document Options mode. 
Effects are also displayed when enabled (Strikeout, Underline). If Regular is used for the font style, this will not be displayed visually in the control's string.

Designator Position and Font

  • Customize Position - enable to change from following the default settings for position of the pin's Designator to an overriding, customized position.
    • Margin - use to enter the required margin (space) between the pin's Designator text and the edge of the component symbol outline. The Customize Position option must be enabled to access this option.
    • Orientation - use to choose the orientation of the pin's Designator text (0 Degrees or 90 Degrees). The Customize Position option must be enabled to access this option.
      • To - use 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 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 Font set in the General region of the Properties panel in Document Options mode. 
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.

VHDL Parameters

  • Default Value - the default value of the parameter.
  • Formal Type - the formal type.
  • Unique Id - the ID of the type.
  • Reset - click to reset the parameters.

PCB Options

  • Pin/Pkg Length - enter the pin-package length. The unit will automatically be entered after you press Enter.

Parameters Tab

Use the 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.

The Parameters tab of the Pin Properties dialogThe Parameters tab of the Pin Properties dialog

Options/Controls

  • Parameters Grid - the main region of this tab lists all of the parameters currently defined for the pin in terms of:
    • Visible - use 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 Parameters region of the Properties panel in Component mode.
    • 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 uneditable. Its Value can only be edited by changing the constraints of the rule. To do this, double-click the parameter to select it, then double-click the rule in the Rules region of the Properties panel in Parameter Set mode. In the resulting Choose Design Rule Type dialog, double-click the desired rule. This opens the Edit PCB Rule (From Schematic) dialog from where the changes to the constraints can be made.
  • Add - click to open the Parameter Properties dialog to add a new parameter to the list and to define the parameter's Name, Value, Type, and whether or not its value is to be visible in the workspace.
  • Remove - click to delete the selected parameter(s) from the list of parameters.
  • Edit - click to open the Parameter Properties dialog to modify the currently selected parameter. 
  • Add as Rule - click open the Parameter Properties dialog to add a new design rule directive parameter to the list. The Parameter Properties dialog opens with an Edit Rule Values button, which in turn opens the Choose Design Rule Type dialog, from where you can choose, and subseqently define, the constraints of the required rule type.

Right-Click Menu

The grid right-click menu offers the following commands:

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

 

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.