Search In: Doc:Documentation: Altium Designer
Altium DesignerAltium 365Altium MCAD CoDesignerAltium CircuitMakerCompany DashboardAltium On-Prem Enterprise ServerAltium Infrastructure Server
Ver: Version: 16.1
2120.220.120.019.119.018.118.017.117.016.116.015.1
Close
Suche Search on Documentation
Documentation Altium Designer Documentation ... ((Dialog Reference))_AD Dialogs((A to F))_AD

Sch_Dlg-SchComponentPinsPropertiesFormComponent Pin Editor_AD

Created: Juli 28, 2015 | Updated: Juni 16, 2017 | Applies to versions: 15.1, 16.0, 16.1 and 17.0

The Component Pin Editor dialog.

Summary

This dialog presents 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 the designer 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 is accessible from both the Schematic Editor and the Schematic Library Editor:

  • Schematic Editor - double-click on the required placed component to access the Properties for Schematic Component dialog, then click the Edit Pins button at the bottom-left of the dialog.
  • Schematic Library Editor - double-click on the component's entry, in the Components region of the SCH Library panel, to access the Library Component Properties dialog, then click the Edit Pins button at the bottom-left of the dialog.

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 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. This entry corresponds to the Display Name property in the Pin Properties dialog.
    • Desc - the description for the pin. This entry corresponds to the Description property in the Pin Properties dialog.
    • Footprint Model Mapping - 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.
    • 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. This entry corresponds to the Electrical Type property in the Pin Properties dialog.
    • Owner - the parent part to which the pin is associated. For a single-part component, this entry will always be 1. It is really 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. This entry corresponds to the Part Number property in the Pin Properties dialog.
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, where their display would otherwise cause unnecessary clutter on the schematic sheet. This entry corresponds to the Hide property in the Pin Properties dialog.
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, respectively. Alternatively, in the Schematic Library Editor, the display of hidden pins can be toggled by clicking Tools | Options | , from the main menus.
  • Number - this option 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. This entry corresponds to the Visible property (associated with the Designator field) in the Pin Properties dialog.
  • Name - this option 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. This entry corresponds to the Visible property (associated with the Display Name field) in the Pin Properties dialog.
The following additional points relate to working with the Pin Grid:
  • With the exception of fields displaying mapping information for any models linked to the parent part, displayed fields for a pin are directly editable within the dialog. Click once on a field to focus it for editing and then type the value or select the option as required. Click away from the field or press Enter to effect 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 grid (with the exception of check box controls) to access the Pin Properties dialog directly.
  • 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 entry in the grid, from where all properties for the pin can be browsed and managed.

Right-Click Menu

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

  • Jump - use this command to jump to the currently selected pin, within the workspace (zoomed and centered (where possible)).
  • Add - use this command to add a new pin to the component (or part thereof).
  • Remove - use this command to remove the currently selected pin from the component. A confirmation dialog will appear, click Yes to proceed with the removal.
  • Edit - use this command to edit the currently selected pin, using the Pin Properties dialog.
  • Report - use this command to generate a report based on the information in the Pin Grid. The Report Preview dialog will open, from where you can browse the report, before printing, or exporting into one of various supported formats.

 

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

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.