Search In: Doc:Documentation: NEXUS Client
Altium DesignerAltium 365Altium MCAD CoDesignerAltium On-Prem Enterprise ServerAltium CircuitMakerAltium CircuitStudioCompany DashboardAltium Infrastructure Server
Ver: Version: 1.0
543.23.13.02.12.01.11.0
Close
Suche Search on Documentation
Documentation Altium NEXUS Documentation ... ((Dialog Reference))_AD Dialogs((A to F))_AD

Sch_Dlg-SchComponentPinsPropertiesFormComponent Pin Editor_AD

Created: Juli 10, 2017 | Updated: März 06, 2024 | Applies to version: 1.0

Nexus message

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 Component Pin Editor dialog
The Component Pin Editor dialog

Summary

The Component Pin Editor dialog displays all pins for either the component in the active schematic library document or a placed component (or part thereof) in the schematic editor. It provides a single, convenient location for you to modify certain properties of any pin associated to that component. In addition to providing a means of editing pin properties, the dialog also allows you to add new pins or delete existing ones.

Access

The Component Pin Editor dialog can be accessed from either the schematic editor or the schematic library editor by performing the following steps:

  1. Double-click on the desired placed component (or right-click then choose Properties from the context menu) to open the Properties panel in Component mode.
  2. On the Pins tab of the panel, click . 

Options/Controls

  • Pin Grid - this area presents all pins for the component. For each pin, the following information is displayed:
    • Designator - the numerical identifier of the pin. Each pin in a part must have a unique designator.
    • Name - the display name for the pin. Note that the pin name is optional, this field can be left blank if required. Alternatively, enter a string into the Name text field, then use the Name checkbox to display or hide the name.
    • Desc - the description for the pin. 
    • Footprint Model Mapping - the title of this is the pad of the indicated linked footprint model to which this pin of the schematic component is mapped. A separate field is presented for each linked footprint model.
The mapping of component pins to model pins can be updated in the Model Map dialog.
  • Type - 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.
  • Owner - the parent part to which the pin is associated. For a single-part component, this entry will always be 1; it is only meaningful for a multi-part component. 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, simply disable the Show option and set the Owner field to 0.
  • Show - reflects whether the pin is visible on the sheet (enabled) or hidden (disabled). The power pins of multi-part components are typically hidden when their display would otherwise cause unnecessary clutter on the schematic sheet. 
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. 
  • Number - this is used to determine whether the designator for the pin is displayed (enabled) or hidden (disabled) when the parent part is placed on a schematic sheet. 
  • Name - this is used 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. 
The following tips relate to working with the Pin Grid:
  • With the exception of fields displaying mapping information for any models linked to the parent part, all fields are editable. Click once on a field to select it then type the value or select the option as required. Click away from the field or press Enter to make the change.
  • Changes made to a pin in the grid will be reflected when accessing the Pin Propeerties dialog for that pin, and vice versa. Double-click on a field associated with a pin entry in the gridto access the Pin Properties dialog.
  • For a multi-part component, the pins for the active/selected part will be presented with a normal white background, with the pins of all other parts presented with a grey background.
  • Pins can be sorted by various fields using the column header in each case. Click once to sort in ascending order, click again to sort in descending order. Shift+click to sort by additional fields. Ctrl+click to remove sorting.
  • Add - click this button to add a new pin to the component. The new pin will be assigned the next available designator (which can be pin 0), and will have the following default properties:
    • Name - 0
    • Desc - blank
    • Mapping - all 0
    • Type - Passive
    • Owner - the number of the active/selected part.
    • Show/Number/Name - all enabled.
Upon clicking OK in the dialog, any newly added pins will be initially placed at the bottom-right of the component (or part thereof). Reposition as required.
  • Remove - click this button to remove the currently selected pin from the component. A confirmation dialog will appear - click Yes to proceed with the removal. If removing a pin from a placed component instance on a schematic, you may need to rewire any existing wiring that was connected to that pin.
  • Edit - click this button to access the Pin Properties dialog for the currently selected pin.

Right-Click Menu

The grid right-click menu offers the following commands:

  • Jump - use to jump to the currently selected pin within the workspace (zoomed and centered (where possible)).
  • Add - use to add a new pin to the component (or part thereof).
  • Remove - use to remove the currently selected pin from the component. A confirmation dialog will appear, click Yes to proceed with the removal.
  • Edit - use to open the Pin Properties dialog to edit the currently selected pin.
  • Report - click to open the Report Preview dialog to preview the report before printing it.

 

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