Search In: Doc:Documentation: Altium Designer
Altium DesignerAltium 365Altium MCAD CoDesignerAltium CircuitMakerCompany DashboardAltium On-Prem Enterprise ServerAltium Infrastructure Server
Ver: Version: 17.1
17.117.016.116.015.1
Close
Search Search on Documentation
Documentation Altium Designer Documentation ... Dialog Reference M to R

Port Properties

Created: June 08, 2017 | Updated: June 18, 2017 | Applies to version: 17.1

This document is no longer available beyond version 17.1. Information can now be found here: Port Properties for version 25

The Port Properties dialog.

Summary

This dialog allows the designer to specify the properties of a Port object. A port is an electrical design primitive. It is used to make an electrical connection between one schematic sheet and another, in a design using multiple sheets. The name of the port defines the connection (i.e. a port on a schematic sheet connects to ports with the same name on other sheets in the project).

For information on how a placed port object can be modified graphically, directly in the workspace, see Graphical Editing.

Access

The Port Properties dialog can be accessed prior to entering placement mode, from the Schematic – Default Primitives page of the Preferences dialog. This allows the default properties for the port object to be changed, which will be applied when placing subsequent ports.

During placement, the dialog can be accessed by pressing the Tab key.

While attributes can be modified during placement, bear in mind that these will become the default settings for further placement unless the Permanent option on the Schematic – Default Primitives page of the Preferences dialog is enabled. When this option is enabled, changes made will affect only the object being placed and subsequent objects placed during the same placement session.

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

  • Double-clicking on the placed port object.
  • Placing the cursor over the port object, right-clicking and choosing Properties from the context menu.
  • Using the Edit » Change command and clicking once over the placed port object.

Graphical Tab

Port Properties dialog - Graphical tab.

Use the dialog's Graphical tab to modify graphical properties of the port object.

Options/Controls

  • Height - the height of the port. Use this field to manually increase or decrease the port's height. If the Autosize option is enabled, this field will automatically adjust to accommodate changes in font size of the port's Name text.
With the Autosize option enabled, you can manually increase the height of the port by entering a larger value still, but you will not be able to enter a value lower than that determined by the autosizing feature.
  • Width - the width of the port. Use this field to manually increase or decrease the port's width. If the Autosize option is enabled, this field will automatically adjust to accommodate changes in length of the port's Name text.
With the Autosize option enabled, you can manually increase the width of the port by entering a larger value still, but you will not be able to enter a value lower than that determined by the autosizing feature.
  • Alignment - specifies the alignment of the port's Name text. Choose from Center, Left, and Right alignment.
  • Fill Color - click the color sample to change the fill color for the port, using the standard Choose Color dialog.
  • Text Color - click the color sample to change the color of the port's Name text, using the standard Choose Color dialog.
  • Border Color - click the color sample to change the border color for the port, using the standard Choose Color dialog.
  • Style - use this field to determine the graphical style of the port. Style options available are: None (Horizontal), Left, Right, Left & Right, None (Vertical), Top, Bottom, Top & Bottom.
  • Border Width - the thickness of the port's border. Choose from Smallest, Small, Medium, or Large.
  • Location X/Y - the current X (horizontal) and Y (vertical) coordinates for the left/bottom editing handle of the port (depending on whether the port is currently horizontal or vertical in its orientation). Edit these values to change the position of the port in the horizontal and/or vertical planes respectively.

Properties

  • Name - the name of the port. The entry in this field defines the connectivity of the port. Ports in a design are considered to be electrically connected if they have identical names. Enter the name directly, or use the field's drop-down list to choose a name from another existing port on the same sheet.
Should you need to negate (include a bar over the top of) the harness entry name, include a backslash character after each character in the name (e.g. E\N\A\B\L\E\). Alternatively, enable the Single '\' Negation option on the Schematic- Graphical Editing page of the Preferences dialog, then include one backslash character at the start of the name (e.g. \ENABLE).
  • I/O Type - defines the electrical properties of the port. Select an option from the drop-down list. Available options are: Unspecified, Output, Input, and Bidirectional.
The setting of this field does not influence the connectivity of the circuit, but is considered during the running of an electrical rules check, which can be set to detect incompatible port directions.
  • Harness Type - this field is used to provide the connectivity between the port and a defined signal harness system, allowing a collection of signals to be transferred between sheets. The Harness Type itself is defined either manually in the associated Harness Definition File, or as part of the properties of a Harness Connector. The associated drop-down lists all currently defined Harness Types detected across the source schematic documents of the active project.
When a defined Harness Type is entered in this field, the color of the port will automatically change to match that of the applicable Harness, and the port's I/O Type will change to Unspecified (and become read-only).
When the port is physically connected to a Harness Connector - either directly, or via a signal harness - it will automatically inherit that harness's type. The Harness Type field will populate with that harness's type, and become read-only.
  • Locked - enable this option to protect the port 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.
  • Unique Id - the current unique identifier for the port. The Unique ID (UID) is a system generated value that uniquely identifies this current port. A new UID value can be entered directly into this field.
    • Reset - click this button to have the system generate a new UID for the port.
  • Autosize - enable this option to have the port automatically adjust its Height and/or Width to accommodate a change to its Name text, in terms of its font sizing, or length.
The autosizing feature proves invaluable when picking up existing text for the port name from elsewhere on the sheet, using the inheritance feature. Simply ensure the Autosize option is enabled (on-the-fly during placement using the Tab key to access the Port Properties dialog). In placement mode, hover the cursor – with port attached – over the text required (a net label for example), and press the Insert key. The port will not only inherit the text, but resize to accommodate the length/height of that text.
  • Font - this control serves two purposes. Firstly, it reflects the currently chosen font – applied to the text for the associated port Name - in terms of Font Name, Font Size and Font Style. Secondly, when clicked it provides access to the standard Font dialog, from where to change the font as required.
By default, the font used for the port's Name follows the document-level font, set on the Sheet Options tab of the Document Options dialog (Design » Document Options). Use the Font field to override this.
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

Port Properties dialog - Parameters tab.

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

Adding a parameter (as a rule) to a port 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 Net associated with that port.

Options/Controls

  • Parameters Grid - the main region of the tab lists all of the parameters currently defined for the port, 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 can not 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, select and edit the parameter, and click the Edit Rules Button in the Parameter Properties dialog - this will give access to the Edit PCB Rule (From Schematic) dialog, from where 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 appear. Use this to define the parameter, especially its Name, Value, Type, and whether or not it's 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 modify the currently selected parameter. The Parameter Properties dialog will appear, with which to do so.
  • Add as Rule - click this button to add a new design rule directive parameter to the list. The Parameter Properties dialog will appear, but this time will contain the Edit Rule Values button, which in turn gives access to 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 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.

 

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.