Altium NEXUS Documentation

Component Pin Editor

Modified by Susan Riege on Jun 1, 2020
This documentation page references Altium Vault, which is no longer a supported product. Altium Vault and its component management features have migrated to Altium Concord Pro.


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, select a pin then 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 column 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 Mapping 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 the use of Part Zero. A pin is included in Part Zero by placing it, then setting the Part Number property to 0. Pins placed in Part Zero will appear on all parts.
  • The pins placed in Part Zero can also be hidden, if required. While this practice is not recommended, for each pin that is required to connect to a power net in this way disable the Show option in the Component Pin Editor dialog and enter the net name in the Hidden Net Name field in either the SCHLIB List panel or the SCH List panel.
  • 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.
  • 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.
  • Pin/Pkg Length - this is the pin-package length. 
  • 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.

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 - this command is non-functional.
  • Report - use to open the Report Preview dialog.

Properties Region

General Tab

  • Location
    • (X/Y)
      • X (first field) - the current X (horizontal) coordinate of the reference point of the object, relative to the current workspace 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. Choices are: 0 Degrees90 Degrees180 Degrees, and 270 Degrees.
  • Properties
    • ​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 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  or  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). Available types are: InputI/OOutputOpen CollectorPassiveHiZOpen Emitter, and Power.
    • 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.
    • 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.
  • A pin is included in Part Zero by placing it, then setting the Part Number property to 0. Pins placed in Part Zero will appear on all parts.
  • The pins placed in Part Zero can also be hidden, if required. While this practice is not recommended, for each pin that is required to connect to a power net in this way disable the Show option in the Component Pin Editor dialog and enter the net name in the Hidden Net Name field in either the SCHLIB List panel or the SCH List panel.
  • Preview Window - this area provides instant visual feedback as you change various options, enabling you to adjust the look and feel of the pin to meet design requirements.
  • 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
These symbols are purely graphical. The true electrical property of the pin is determined by the entry set for the pin's Electrical Type.
  • Inside - use to optionally add a symbol to the pin on the inside of the component graphic. Choose from: No SymbolPostponed OutputOpen CollectorHizHigh CurrentPulseSchmittOpen Collector Pull UpOpen EmitterOpen Emitter Pull UpShift 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 SymbolDotActive 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 SymbolRight Left Signal FlowAnalog Signal InNot Logic ConnectionDigital Signal InLeft Right Signal Flow, and Bidirectional Signal Flow.
  • 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.
  • Font Settings
    • 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- 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.
    • Allow Synchronization with Database - enable to synchronize with the database.
    • X/Y - enter the X and Y coordinates.
    • Rotation - use the drop-down to select the rotation. Choices are: 90°180°, and 270°.
    • Autoposition - check to enable auto-positioning.
  • Add - click to add a parameter. Use  to delete the currently selected parameter.

 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

You are reporting an issue with the following selected text
and/or image within the active document:
ALTIUM DESIGNER FREE TRIAL
Altium Designer Free Trial
Let’s get started. First off, are you or your organization already using Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

In that case, why do you need an evaluation license?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You actually don’t need an evaluation license for that.

Click the button below to download the latest Altium Designer installer.

Download Altium Designer Installer

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Please fill out the form below to get a quote for a new seat of Altium Designer.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

If you are on Altium Subscription, you don’t need an evaluation license.

If you are not an active Altium Subscription member, please fill out the form below to get your free trial.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Why are you looking to evaluate Altium Designer?

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

You came to the right place! Please fill out the form below to get your free trial started.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.

That’s great! Making things is awesome. We have the perfect program for you.

Upverter is a free community-driven platform designed specifically to meet the needs of makers like you.

Click here to give it a try!

If would like to speak with a representative, please contact your local Altium office.
Copyright © 2019 Altium Limited

Got it. You can download a free Altium Designer Viewer license which is valid for a 6 months.

Please fill out the form below to request one.

By clicking “Get Your Free Trial”, you are agreeing to our Privacy Policy.
You may receive communications from Altium and can change your notification preferences at any time.