Adding Design Detail to Your Schematics with Parameters in Altium NEXUS

User-defined design attributes are added to your design using parameters. Parameters are general-purpose text strings that are child objects of a parent object that allow detailed information to be added to that parent object. For example, schematic components make extensive use of parameters. They are used to define the Designator and the Comment, as well as the general-purpose parameter strings that can be added to fully define it. General-purpose component parameters can be used for a variety of functions, including component detail, such as Wattage, Voltage, etc., supplier detail, including the supplier name and part number, library component design detail, such as the revision number of the symbol; and documentation detail, such as a URL that links to a component datasheet.

Parameters can also be defined at the schematic sheet (document) level and also the project level. Document-level parameters are ideal for defining fields such as the document title and number, and project-level parameters are ideal for defining fields such as the designer or the project name.

Altium NEXUS supports parameters at various levels of the project - project-level parameters, document-level parameters (defined for a schematic sheet), and variant-level parameters. They also have a hierarchy, which means you can create a parameter with the same name at different levels of the project, each having different values. Altium NEXUS resolves this with the following order of precedence: Variant (highest priority) ---> Schematic Document ---> Project (lowest priority). That means the parameter value defined in the schematic document overrides the value defined in the project options, and the value defined in the variant overrides the value defined in the schematic document. 

Project-level Parameters

Parameters are used to provide additional design information. Parameters defined at the project level are available for use across all schematic sheets in the project. Project-level parameters are defined in the Project Options dialog on the Parameters tab. Click here for detailed information about adding, deleting, and editing parameters on the Parameters tab.

You display the value of a parameter on a schematic sheet by placing a special string. A special string is nothing more than a standard schematic Text String containing the parameter name, preceded by an equals sign (when a string starts with the = symbol, it is called a special string).

For example, the image above shows four project parameters. To display the project name on a schematic you place the special string =Project. When the software detects the = symbol it then checks for a parameter (project, document, or variant) whose name is defined by that Text String, Project in this example. Instead of the string =Project being displayed on the schematic sheet, it displays the value of that parameter, KAME_FMU in this example.

► Learn more about Working with text Objects on a Schematic, and Special Strings.

► Learn more about the options that affect the display of Special Strings.

Server-side Parameters

Server-side project parameters are saved in the server with the project and can only be edited within the server. By contrast, design-side project parameters are saved in the project file (*.PrjPcb) and can be edited in Altium NEXUS. Server-side project-level parameters display on the Parameters tab of the Project Options dialog with a blue icon, while design-side project-level parameters display with an orange icon.

Document-level Parameters

Document-level parameters can be configured for each schematic document. The document parameters are defined in the Document Options mode of the Properties panel. This mode is accessed when no objects are selected in the schematic. The Parameters tab of the panel is where you add, edit or delete parameters for the schematic. Use the buttons above the list of parameters to display only parameters in the list, as shown in the image below.

Adding a parameter is done by clicking the Add button and then selecting Parameter as shown in the image below. A new parameter named Parameter n will appear in the list. Click on the name then enter the desired parameter name. Click in the Value column then enter the desired value of the parameter.

To edit a parameter's value, click the cell in the Value column then edit as needed.

To delete a parameter, select it in the list then click . Within the panel, you will be asked to confirm the deletion by clicking Yes to delete or No to cancel the deletion. You can select one or more parameters in the list to delete at one time.

Variant-level Parameters

Parameters for variants are displayed in the Variant Management dialog. Once a variant is added, using the Add Variant button in the dialog, you can add parameters by clicking in the Variant of <xxx> column then click the Edit Variant button.

The Edit Project Variant dialog opens in which all the parameters for the variant are listed. To add a new parameter, click the Add button. Use the Parameter Properties dialog that opens to enter the Name and set the Value of the new parameter then click OK. The new parameter is now displayed in the Edit Project Variant dialog.

Parameters can be deleted by selecting the parameter in the Edit Project Variant dialog then click Remove.

Component Parameters

Component parameters can be defined for schematic components from the Component mode of the Properties panel on the General tab in the Parameters region. The Component mode is accessed by double-clicking on a component in the schematic. Click the Parameters button at the top of the Parameters region to list only parameters in the region.

Component Comment Parameter

Comment parameters can only be edited (not added - see below information box) in the Parameter mode of the Properties panel. 

Component Designator Parameter

Designator parameters can only be edited (not added - see below information box) in the Parameter mode of the Properties panel. 

Preventing Component Parameter Updates

Component-level parameters can be prevented from being updated by clicking the lock icon () in the Component mode of the Properties panel (double-click a component to access) in the Parameters region. To unlock the parameter, click .

Object-level Parameters

Parameters for several schematic objects can be added, edited and deleted in the corresponding mode of the Properties panel. This section is a list of the schematic objects that allow parameters to be added or edited. The page with detailed information about that object's parameters can be accessed by clicking the gold link within the text.  

Harness Connector Type

Harness Connector Type parameters can only be edited (not added - see below information box) in the Parameter mode of the Properties panel. 

Pin

Pin parameters can be placed and edited from the Component Pin Editor dialog and the Pin mode of the Properties panel. 

Port

Port parameters can be placed and edited from the Parameters tab of the Port mode of the Properties panel.

Sheet Symbol

Sheet Symbol parameters can be placed and edited on the Parameters tab of the Sheet Symbol mode of the Properties panel.

Sheet Symbol Designator

Sheet Symbol Designator parameters can only be edited (not added - see below information box) in the Parameter mode of the Properties panel.

Sheet Symbol Filename

Sheet Symbol Filename parameters can only be edited (not added - see below information box) in the Parameter mode of the Properties panel.

Indirection

Parameters for certain objects are added as a property of the parent object and are not placed independently. To view/edit these types of parameters, select the object to open the Properties panel then click the parameter you want to view or edit in the Parameter mode of the Properties panel. These object parameters are described in the above sections and include:

• Comment
• Designator
• Harness Connector Type
• Sheet Symbol Designator
• Sheet Symbol Filename

Parameter Sets

A parameter set is a design directive that allows design specifications to be associated to a net-type object within a schematic design. For example, use a parameter set to declare two nets to be members of a differential pair. It is the presence of specifically named parameters in the parameter set that the software uses to determine which design directive you are placing.

Using the Parameter Manager

Parameters can be added and edited individually, or you can use the Parameter Table Editor dialog (Parameter Manager) to add and edit parameters across the entire design or across an entire library. When you open the dialog, it gathers all parameter data for the entire design and presents it in a table-like grid. The Parameter Table Editor dialog is launched from a schematic by selecting Tools » Parameter Manager from the main menus. After running the command, the Parameter Editor Options dialog opens. In this dialog, select the type of parameters you want to be loaded into the Parameter Table Editor dialog. As an example, if you are working on component parameters, disable all options in the Include Parameters Owned By region except for Parts. Another example is if you are working on document parameters, enable only the Documents option. Note that the Exclude System Parameters option includes things like component model settings, document parameters that were defined in the template, and so on. Explore this option when you are more familiar with managing parameters.

After selecting the options needed, click OK to open the Parameter Table Editor dialog (Parameter Manager). 

Use this dialog to edit and update parameters across the entire project. The dialog can be used to directly edit existing parameters in the project or to configure parameter updates from a linked database (linked via a DbLink, DbLib or SvnDbLib file). Note that these database library link type files include options that control if a parameter is to be updated or not.

Renaming a Parameter

To rename a parameter, right-click in a cell in the column you want to rename then select Rename Column from the drop-down menu. The Rename Existing Parameter dialog opens. Enter the new name then click OK. Note that the column heading will have changed and now has a small blue triangle next to the name. This icon indicates that the value of this cell has changed. For complete details on the various icons used in this editor, press F1 when the cursor is anywhere over the dialog.

Adding a Parameter

To add a parameter to components, select the cells in the Parameter Table Editor dialog editor using Shift+Click or Ctrl+Click key combinations, right-click then choose Add from the drop-down menu. After selecting Add, a small green plus symbol appears in each cell. This indicates that a new parameter has been added.

Now that the parameter has been added, you can define the component type for each component. The Parameter Table Editor dialog supports standard table editing shortcuts. You can press F2 to edit a cell then press Enter to apply the edit. Multiple cells can be edited by selecting the cells then right-click and choose Edit from the menu. Enter the new value then press Enter to apply the edit to all selected cells.

Applying the Parameter Changes

The parameter edits that have just been completed are currently held in the Parameter Table Editor dialog and have not been applied to the components on the schematic sheets. To apply these changes to the components, you need to generate an Engineering Change Order (ECO) then apply the ECO to the design. In the Parameter Table Editor dialog, click the Accept Changes (Create ECO) button. The Parameter Editor Table dialog will close and the Engineering Change Order dialog will open.

Click the Validate Changes button to check that the changes can be applied. If the changes are valid, a green check displays in the Check column.

Click Execute Changes to apply the parameter changes to the components. Once the changes have been applied, close the Engineering Change Order dialog.