Editing Multiple Parameters Using the Parameter Manager
Contents
Figure 1. Choose which types of parameters to edit
User-defined design attributes are added to your design using parameters. Component parameters can be used to define anything from component ratings, to stock information, to PCB component class membership. You can even include links to component datasheets as a parameter. Parameter Sets containing PCB layout, NetClass and/or differential pair directives can be added to nets to specify PCB design requirements, or to include the net in a PCB net class for example. Document parameters can be used to define things like the title of the sheet, the designer's name, and so on.
Parameters can be added and edited individually, or you can use the Parameter Table Editor dialog to add and edit them 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 is launched by selecting Tools » Parameter Manager.
After selecting Parameter Manager from the menu, the Parameter Editor Options dialog appears first. In this dialog, you determine which type of parameters you want loaded into the Parameter Table Editor dialog.
If you were working on component parameters you would disable all options in the Include Parameters Owned By section, except for the Parts option. If you wanted to work on document parameters, you would only enable the Documents option. Note the Exclude System Parameters option – these include 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.
The following instructions and images are based on the 4 Port Serial Interface Reference Design example.
Renaming a Parameter
In Figure 2 below, you will notice that one of the existing parameters is called 'Text Field1'. This needs to be renamed. 'Component Type' would be a more suitable name.
Figure 2. Using the Parameter Table Editor to rename an existing parameter
Figure 3. The renamed parameter
To rename a parameter, right-click in any cell in that column and select Rename from the pop-up menu. The Rename dialog will open, so type in the new name and click OK. Note that the column heading will have changed and now has a small blue triangle next to the name (as shown in Figure 3). 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.
You will also notice in Figure 2 that some of the components do not have a Component Type parameter at all – this is indicated by the diagonal hatching. The next step is to add the Component Type parameter to the other components.
Adding a Parameter
To add a parameter to components that do not currently have it, select those cells in the editor using the SHIFT + Click or CTRL + Click key combinations. Then right-click and choose Add from the pop-up menu.
After selecting Add, you will notice that a small green plus symbol appears in each cell. This indicates that a new parameter has been added.
Figure 4. Adding parameters to selected components, before adding on the left, and after on the right
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. Use the cursor keys to 'walk' around the grid, press F2 to edit a cell, and press ENTER to apply the edit. Multiple cells can be edited in one go – select the cells, right click on the selection and choose Edit from the pop-up menu, type in the new value, and press ENTER to apply the edit to all selected cells.
Figure 5. Select the cells, right-click and Edit (left), type in new value (center) and press ENTER (right)
Applying the Parameter Changes
Figure 6. System applied changes are always done through the Engineering Change Order dialog
The parameter edits that have just been carried out are currently held in the Parameter Table Editor and they have not been applied to the components on the schematic sheets yet. To apply these changes to the components, you need to generate an ECO (Engineering Change Order) and then apply the ECO to the design.
When you are satisfied with your parameter edits, click the Accept Changes (Create ECO) button. The Parameter Editor Table dialog will close and the Engineering Change Order dialog will appear.
Click the Validate Changes button to check that the changes can be applied, then click Execute Changes to apply the parameter changes to the components. Once the changes have been applied, close the Engineering Change Order dialog.
Managing Multiple Component Models
Figure 7. The Schematic Library Editor, with the model editing region displayed at the bottom of the main window.
The schematic symbol represents the component on the schematic. The wiring then connects the component pins to create the connectivity. While this creates the schema, or the inter-connective structure of the design, other information is required to translate that into the final physical PCB.
The ability to translate the original schema into other forms, such as a PCB layout, or perhaps a circuit simulation description, is provided by the models that you attach to each component.
Different model kinds are supported, including PCB footprints, spice simulation models, signal integrity analysis models, and 3D models. While these can be defined on the schematic sheet, they are typically defined in the component library. For an individual component, it is straightforward to add a model to a component. You can add them in the model editing region at the bottom of the main schematic library editing window, as shown in Figure 7.
For more information on creating library components and attaching models, see Creating Library Components Tutorial
For a better understanding of component models, see Component, Model and Library Concepts
Figure 8. Use the Model Manager to manage the models across multiple components
To add or edit model settings across multiple components, the Library editor includes a Model Manager. To open the Model Manager for the current library, select Tools » Model Manager from the menus. The Model Manager dialog will open, displaying the components in the current library down the left, click to select a component and display a list of the models currently associated with that component.
Tasks that you can perform in the Model Manager include:
- Add a new model to one or more components
- Copy a model from one component, and paste it to one or more components
- Remove a model from one or more components
- Edit the model assigned to one or more components.
All of these commands can be executed from the right-click menu in the model list region of the dialog and some can also be performed using the buttons below the model list region.
Figure 8 shows the Model Manager with a PCB footprint model selected and about to be copied. Once it has been copied, it can be pasted to multiple components. To do this, use SHIFT + Click or CTRL + Click to select multiple components in the list. Once the required components are selected, right-click in the Model region and select Paste from the pop-up menu.