Usually it is not convenient to draw very complex schematics in a single page but it is preferable to distribute the different sections in separate pages; this simplifies both the drawing of the schematic and its description and understanding. All documents belonging to the same project are considered parts of the same schematic, so the netlist (the list of existing connections between the pins of the components included in the schematic) is always generated at the project level and includes all the components present in all the graphic pages of the project. Multi-page schematics can be Flat or Hierarchical.
 Tip: |
|---|
You can exclude an entire document from the netlist by setting the property Ignore this document in the dialog box Document Properties or you can exclude a single page by setting the Ignore this page property in the Page properties dialog box. |
Multi-page Flat schematic
A project in which connections between pages are made horizontally is called flat because all the sheets of the schematic are on the same level. Connections between the pins of components belonging to different pages are made only with global connections or with ports. A flat design can be imagined as a design drawn on a single large sheet of paper that has subsequently been cut into smaller pages.
To use the multi-page flat design model
Open the Project Properties dialog box in one of the following ways:
Right-click on the project name in the Job panel to open the menu and choose Project Properties.
Select the Settings » Project Properties command.
Press the key combination CTRL+ALT+P.
Open the tab Schematics.
Set the parameters in the Compiling netlist » Connectivity in a Multi-Sheet Design to the following values:
The scope of the Net on Page.
The scope of the Port on Project.
Multi-page Hierarchical schematic
A project in which the connections between the pages are made vertically is called hierarchical because the entire project can be represented by a tree structure in which the different pages can be found on different levels. The names of the connections are local and the connections between the different sheets are made only by connecting the sheet entries with the ports having the same name and belonging to the associated child sheet.
Generally, in a hierarchical multi-page schematic, the upper level represents the block diagram of the entire circuit. Each block is represented by a Sheet object and presents the input and output lines represented by the Sheet entry objects. In the pages corresponding to the Sheet objects there is the schematic of each block that can contain other Sheet objects and so on.
To use the multi-page hierarchical design model
Open the Project Properties dialog box in one of the following ways:
Right-click on the project name in the Job panel to open the menu and choose Project Properties.
Select the Settings » Project Properties command.
Press the key combination CTRL+ALT+P.
Open the tab Schematics.
Set the parameters in the Compiling netlist » Connectivity in a Multi-Sheet Design to the following values:
The scope of the Net on Page.
The scope of the Port on Page.