Вы просматриваете версию 20.0. Для самой новой информации, перейдите на страницу для версии 21
The Parameter tab of the Project Options dialog.
This tab of the Project Optionsdialog enables you to manage parameters defined for the project, often referred to as project-level parameters. Parameters defined at the project level are available for use across all schematic sheets and PCB documents in the project through the use of special strings (=<ProjectParameterName> on a schematic and .<ProjectParameterName> on a PCB). Parameters can be used to provide additional design information. Project-level parameters, for example, can be used in global fashion as the source for special string parametric data to be added to schematic sheets and/or the PCB document - the latter of which does not support localized parameters.
Server-side project parameters are saved in the Workspace with the project and can only be edited within the Workspace. By contrast, design-side project parameters are saved in the project file (*.PrjPcb), and can be edited in Altium Designer. Server-side project parameters appear in the Parameters tab of the Project Options dialog with a blue icon, while design-side project parameters appear with an orange icon.
When using the Project Parameter with a Schematic Template (*.SchDot), place the parameter as a Special String in the TitleBlock "=[ParameterName]" of the template.
Altium Designer 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 Designer 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. (Note that schematic-level parameters are not available on the PCB or in the BOM; for these types of outputs you should use project or variant parameters.)
For information about linking components to your company database, click here.
This is one of multiple tabs available when configuring the options for a project – accessed from within the Project Options dialog. This dialog is accessed by:
From the PCB or schematic editor click Project » Project Options.
Right-click on the project name on the Projects panel then click Project Options from the context menu.
Parameters Grid - the main region of the tab lists all of the parameters currently defined for the project, in terms of:
Name - the name of the parameter.
Value - the value of the parameter.
A parameter can be modified with respect to either of these attributes directly in the grid.
Add - click to open the Parameter Properties dialog, where you may add a parameter and specify the properties of a parameter when attached at the project or variant level.
Remove - click to delete the selected parameter(s) from the list of parameters. This option is unavailable for server-side project parameters due to the fact that they may only be removed or edited in the Workspace.
Edit - click to open the Parameter Properties dialog, where you may modify the contents of the currently selected parameter. This option is unavailable for server-side project parameters due to the fact that they may only be removed or edited in the Workspace.
Refresh - click to revert the last changes made to the design-side project parameter. For server-side project parameters, click to ensure you contain the latest version of the parameter. Changes made to server-side project parameters within the Workspace will not be reflected in this dialog until this option is used.
Set To Installation Defaults - click to set all options to the installation defaults.
The following commands are available on the right-click menu:
Edit - use this command to modify the currently selected parameter in the Parameter Properties dialog.
Add - use this command to add a new parameter to the list in the Parameter Properties dialog.
Remove - use this command to delete the selected parameter(s) from the list.
Copy - use this command to copy the selected parameter(s) to the Windows clipboard.
Paste - use this command to paste parameter(s) on the Windows clipboard into the parameters list.
The Copy and Paste commands support the ability to define a set of parameters in an external spreadsheet (such as Microsoft Excel) and paste them into the tab. If a parameter being pasted has the same name as an existing parameter in the list, the value for the existing parameter will be overwritten with the one being pasted.