Parameter Properties (SCH)

Now reading version 20. For the latest, read: Parameter Properties (SCH) for version 18.0

The Parameter Properties dialog
The Parameter Properties dialog

Summary

This dialog allows you to specify the properties of a Parameter object. Parameters can be added in a variety of places to provide additional information. For example, parameters at the local document level can be used as the source for special string parametric data to be added to schematic sheets - most notably as part of the title block in a schematic template. Parameters can also be added to specific design objects, such as components, sheet symbols, ports, and pins. These can be both standard parameters that give additional useful information local to the object, or rule-based parameters. The latter enables design constraints to be specified on the schematic side, which will translate into PCB design rules with appropriate scope once the design is passed to the PCB document. 

Access

The Parameter Properties dialog can be accessed from the schematic editor by clicking the Add, Edit, or Add as Rule button on the Parameters tab of the Pin Properties dialog (click the Edit button in the Component Pin Editor dialog).

Options/Controls

Name

  • Name - use this field to give a standard (non-rule) parameter a meaningful name reflective of its purpose.
  • Visible - enable this option to have the parameter's name displayed on the schematic.
  • Lock - enable this option to prevent editing of the parameter's name.
Visibility only applies to port, pin, sheet symbol-based, and component parameters, and not to document-level parameters. For the latter, the Visible option is unavailable.
None of these options are editable for a parameter added as a rule - the Name field is set permanently to Rule, the Visible option is permanently disabled and the Lock option is permanently enabled.

Value

  • Value - use this field to give a standard (non-rule) parameter its value. For a rule-type parameter, this entry will initially be Undefined. The value can only be set/modified by defining the constraints of the chosen rule type. This is done by clicking the Edit Rule Values button.
  • Visible - enable this option to have the parameter's value displayed on the schematic.
  • Lock - enable this option to prevent editing of the parameter's value.
  • Edit Rule Values - this button is only available for a parameter that has been added as a rule. If the value for the parameter is currently Undefined, click this button to open the Choose Design Rule Type dialog. Choose the required rule then use the subsequent Edit PCB Rule (From Schematic) dialog to define its constraints. Once the rule is defined, subsequently clicking this button will access the latter dialog directly.
Visibility only applies to port, pin, sheet symbol-based, and component parameters, and not to document-level parameters. For the latter, the Visible option is unavailable.
On the sheet, the Value alone can be visible, or both the Name and the Value (appearing in the format <Name>:<Value>), but not the Name by itself.

Properties

  • Location X/Y - the current X (horizontal) and Y (vertical) coordinates for the bottom-left corner of the parameter's bounding rectangle. Edit these values to change the position of the parameter in the horizontal and/or vertical planes.
  • Color - click the color sample to change the color used for the parameter (both for its name and value) using the standard Choose Color dialog.
  • 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.
  • Font - this control serves two purposes: it reflects the currently chosen font – applied to the text for the parameter's name and value - in terms of Font Name, Font Size and Font Style, and when clicked, it provides access to the standard Font dialog, from where you can change the font as required.
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.
  • Locked - enable this option to protect the parameter 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 parameter. The Unique ID (UID) is a system-generated value that uniquely identifies this current parameter. 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 parameter.
When adding a parameter as a rule to an object, a unique ID is given to it. The same ID is given to the corresponding design rule that is created in the PCB. With this Unique ID, the constraints of the rule can be edited on either the schematic or PCB side and the changes pushed through upon synchronization.
  • Orientation - specify the orientation of the parameter, counterclockwise in relation to the horizontal. Options available are: 0 degrees, 90 degrees, 180 degrees, and 270 degrees.
  • Autoposition - this option is meaningful only for a component parameter. Enable it to have visible parameters positioned automatically every time the associated component is rotated. Disable this option to take manual control over parameter placement. The parameter will have a dot appear at its bottom-left corner to distinguish it as being a manual parameter.
  • Justification - use the two buttons associated with this field to specify how the parameter is to be vertically (left button) and horizontally (right button) justified. This will depend on its current Orientation and Location X/Y.
    • Vertical Justification - the following justification options are available, using a visible parameter with 0 degrees orientation as an example:
      • Top - the top edge of the parameter's bounding rectangle is against the Y = Location Y line.
      • Center - the parameter's bounding rectangle is centered across the Y = Location Y line.
      • Bottom - the bottom edge of the parameter's bounding rectangle is against the Y = Location Y line.
    • Horizontal Justification - the following justification options are available, using a visible parameter with 0 degrees orientation as an example:
      • Left - the left edge of the parameter's bounding rectangle is against the X = Location X line.
      • Center - the parameter's bounding rectangle is centered across the X = Location X line.
      • Right - the right edge of the parameter's bounding rectangle is against the X = Location X line.
  • Allow Synchronization With Database - this option is meaningful only for a component parameter. Enable it to maintain synchronicity with the parameter in the corresponding component record in the relevant linked database. If there is a change to the parameter in the database, an update of the schematics from that database will bring the change into the parameter of the placed component instance.
  • Allow Synchronization With Library - this option is meaningful only for a component parameter. Enable it to maintain synchronicity with the parameter in the corresponding component in the relevant source library. If there is a change to the parameter in the source, an update of the schematics from that source will bring the change into the parameter of the placed component instance.

 

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.