Search In: Doc:Documentation: NEXUS Client
Altium DesignerAltium 365Altium MCAD CoDesignerAltium CircuitMakerCompany DashboardAltium On-Prem Enterprise ServerAltium Infrastructure Server
Ver: Version: 5
543.23.13.02.12.01.11.0
Close
搜索 Search on Documentation

多图纸和多通道设计

Created: 一月 12, 2022 | Updated: 四月 25, 2022 | Applies to version: 5

This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer and a connected Altium 365 Workspace. Check out the FAQs page for more information.

 

Parent page: Capturing Your Design Idea as a Schematic

When schematics were originally captured on paper, it was often on a single sheet of paper large enough to fill a big drafting table, which was reproduced on a dedicated, large-format copier. Times have changed, now schematics are captured on a desktop PC, stored on a server, and printed on a small-format laser printer.

This change means that even a simple design can be more easily displayed and understood if it is presented on multiple schematic sheets. Even when the design is not particularly complicated, there can be advantages in organizing it across multiple sheets.

For example, the design may include various modular elements. Maintaining these modules as individual documents allows several designers to work on a project at the same time. Breaking the design into logical modules greatly enhances the readability of the design too, an important consideration for those that need to read and interpret the schematic later in the life of that product. Another advantage is that when a design is structured over a number of sheets with fewer components on each, small format printing, such as laser printers, can be used.

There are two decisions to make if you plan to spread your design over multiple sheets:

  • the structural relationship of the sheets, and
  • the method employed for electrical connectivity between the circuitry on those sheets.

Your choice will vary according to the size and type of each project, and your personal preferences.

This article focuses on the structural relationships between the sheets, how it works, and the tools and techniques available to create a multi-sheet design. To learn more about how connectivity is created, refer to the Creating Connectivity article.

Flat or Hierarchical Design

As mentioned, as the designer you need to decide how the schematic sheets are organized, and how the connectivity is established between those sheets. These are not separate decisions though, as you choose the structure you will also need to choose how the connections between those sheets are going to be created.

There are two approaches to structuring a multi-sheet design: either flat or hierarchical.

The technique used to connect a child sheet to the parent sheet is the same for both flat and hierarchical designs - it is how the connectivity is created that determines if it is a flat or hierarchical design.

Flat Design

You can think of a flat design as if a large schematic sheet has been cut up into a number of smaller sheets - in a flat design all sheets exist on the same level. The connectivity in a flat design is created directly from any sheet to any other sheet - this type of connectivity is referred to as horizontal connectivity.

The use of a top sheet is optional in a flat design. If one is included, it will have a sheet symbol for each of the sheets in the design, but cannot include any wiring. There can be any number of sheets in a flat design.

First image - the flat design has no top sheet; second image - the same design has a top sheet. Note that the top sheet has no wiring. It simply shows the sheets in the design. 
First image - the flat design has no top sheet; second image - the same design has a top sheet. Note that the top sheet has no wiring. It simply shows the sheets in the design.

Both of the images above show a flat design, the version on the left does not have a top sheet, the version on the right does. For a small design that only has two or three schematic sheets in it, you might decide that a top sheet does not add any value. Once the sheet count gets higher, a top sheet can help the reader understand the functionality of the circuit design from the way that the logical blocks (Sheet Symbols) are arranged on the sheet. All sheets in the design appear at the same level in the Projects panel because there is no hierarchy.

Hierarchical Design

It is important to remember that for hierarchical designs, a project can contain only one top sheet. All other source documents must be referenced by sheet symbols. When performing a design validation, the Multiple Top Level Documents violation check can be used to flag if this is not the case. In addition, no sheet symbol may reference the sheet it's on or any sheet higher up the ladder, as this will create an irresolvable loop in the structure.

A hierarchical design is one that has Sheet Symbols to create the parent-child type relationships between the sheets, and, the connectivity is through the Sheet Entries in those Sheet Symbols - not directly from the Ports on one sheet to the Ports on another sheet.

As in a flat design, the child sheet is identified by defining its filename in the sheet symbol. In a hierarchical design, that child sheet can also include sheet symbols, referencing lower-level sheets, thus creating another level in the hierarchy. The image below shows a hierarchical design, with 3 levels in the hierarchy.

In a hierarchical design, the structure shown in the tree is determined by the parent-to-child relationships created by the sheet symbols.
In a hierarchical design, the structure shown in the tree is determined by the parent-to-child relationships created by the sheet symbols.

In a hierarchical design, a signal on a child sheet leaves the sheet via a Port, which connects upward to a matching Sheet Entry on the parent sheet. The parent sheet includes wiring that carries the child signal across to a Sheet Entry in another Sheet Symbol, it then travels down to a matching Port on the second child sheet, as shown in the image below.

The connectivity is from a Port on the child sheet up to a matching Sheet Entry in the Sheet Symbol on the parent sheet

This parent-child sheet structure can be defined to any depth, and there can be any number of sheets in a hierarchical design.

The connectivity between the sheets is determined by the Net Identifier Scope. This is set in the Options tab of the Options for Project dialog. To learn more about creating connectivity, read the Creating Connectivity article. Note that the Net Identifier Scope includes an Automatic option, unless you have unusual connectivity requirements, this option is a good choice.

Another advantage of a hierarchical design is that it provides the platform for the delivery of a sophisticated design reuse system. This system is delivered in two ways, depending on how the data is stored, either: file-based or server-based.

  • The file-based system is called Device Sheets, where you place an existing schematic from a library of Device Sheets directly into the design being created. To learn more about Device Sheets, refer to the Device Sheets article.
  • The server-based system is called Managed Sheets, where you place an existing schematic from a managed content server directly into the design being created. To learn more about Managed Sheets, refer to the Managed Sheets article.

Creating a Multi-Sheet Design

As soon as you add a second schematic sheet to your project, you've created a multi-sheet design. If you are planning on creating a flat design without a top sheet, you simply keep adding schematic sheets to the project, and confirm that the Net Identifier Scope is set correctly.

If you want to use sheet symbols to reference lower-level sheets, you can either place the sheet symbol and manually edit it to correctly refer to the lower-level sheet, or you can use the various built-in commands to help, as described below.

Referencing the Child Sheet

It is the Filename property of the Sheet Symbol that references the lower-level sheet. Note that this field should only include the schematic filename, not the path to that file's location (this location data is actually stored in the Project file).

The Filename property links this sheet symbol to the child schematic sheet.
The Filename property links this sheet symbol to the child schematic sheet.

Note that the child schematic does not have to be stored in the same folder as the parent schematic. If the file is stored in a folder below the parent's storage folder then relative file referencing is used. If the file is stored in another location, then absolute file referencing is used. Take care when relocating files in such a project, or use the Project Packager to ZIP the files, as it will resolve file paths as it ZIPs the project.

Creating Hierarchy

The software includes a number of commands that allow you to build your multi-document, hierarchical structure quickly and efficiently. The commands you use will depend on your personal design methodology - which can be broadly classified as top-down, or bottom-up. These commands will be more efficient than creating the hierarchy manually, as they handle all the elements that are needed in the process, such as adding Sheet Entries, creating new schematic sheets, placing Ports, and so on.

Use this command to build the hierarchy in a top-down fashion:

  • Design » Create Sheet From Sheet Symbol – use this command to create a new schematic sheet below the nominated sheet symbol. Ports are added to the child sheet to match any Sheet Entries found in the Sheet Symbol. Don't worry if you have not included all of the Sheet Entries in the Sheet Symbol yet, if more are added over time you can re-synchronize the Sheet Entries and Ports, as discussed below.

Use this command to build the hierarchy in a bottom-up fashion:

  • Design » Create Sheet Symbol From Sheet – use this command to create a symbol from the nominated schematic sheet. To use this command, first switch to the sheet that will hold the new Sheet Symbol, then launch the command. The Sheet Symbol will include a Sheet Entry to match each Port it finds. If Ports or Sheet Entries are added or removed at a later stage they can be re-synchronized, as discussed below.

Use this command to reorganize how the circuity is placed in the design:

  • Edit » Refactor » Move Selected Sub-circuit to Different Sheet - use this command to move the selected components and wiring to a different sheet in the project. The Choose Destination Document dialog will open, allowing you to choose any existing schematic in the project. This command is described in more detail below.

In case you're wondering why there are dedicated commands for moving components from one sheet to another, these are provided because the standard Cut & Copy commands automatically reset the Unique Identifier in each component. The UID ties the schematic component to the PCB component, if a schematic component's UID has been reset you will be prompted to attempt to match via designators whenever the design is synchronized (when the Design » Update command is used). UIDs can be re-synchronized if required, using the Project » Component Links command from within the PCB editor.

► Learn more about Design Synchronization

Restructuring the Design

Main article: Design Refactoring

The process of design is often unstructured and organic, the designer could be formulating ideas for multiple parts of the design at the same time, capturing sections as their ideas evolve. That means that what started out as a well-organized, neatly laid out set of schematics can become crowded and poorly organized. While you can Cut, Copy and Paste to reorganize the schematic design, this is not always the best approach.

Why not cut and copy? Because as each component is placed it is assigned a unique identifier, and this identifier is automatically reset whenever a component is Cut/Copied and Pasted. This UID management is done to ensure that there is only one instance of each UID used in the design, as it is the key field that links the schematic component to the PCB component. The Cut/Copy/Paste approach is fine if the design has not been transferred to the PCB editor, but if it has, then it is better to use the refactoring tools.

Moving a Sub-circuit to Another Sheet

The easiest way to move a section of circuitry from one sheet to another is to select it, then run the Edit » Refactor » Move Selected Sub-circuit to Different Sheet command. The Choose Destination Document dialog will open, after you select the target sheet and click OK that sheet will appear, with the sub-circuit floating on the cursor, ready to position.

A selected section of circuitry can easily be moved to a different sheet in the project using the Move Selected Subcircuit to Different Sheet command.
A selected section of circuitry can easily be moved to a different sheet in the project using the Move Selected Subcircuit to Different Sheet command.

► Learn more about Design Refactoring.

Synchronizing the Ports and Sheet Entries

If you have moved components and wiring as part of restructuring the design, then you may also need to re-synchronize the child sheet to its Sheet Symbol, so that each Port has a matching Sheet Entry. This is done using the Synchronize Sheet Entries and Ports command, which you can use for:

  • A specific Sheet Symbol - right-click on the Sheet Symbol to display the context menu and select the Sheet Symbol Actions » Synchronize Sheet Entries and Ports command to analyze only the Sheet Symbol under the cursor.
  • All Sheet Symbols in the design - select the Design » Synchronize Sheet Entries and Ports command to analyze all of the Sheet Symbols in the entire design, the dialog will include a tab for each Sheet Symbol in the design, in accordance with the Only Show unmatched sheet symbols option at the bottom of the dialog.

For both of these commands, the Synchronize Ports to Sheet Entries dialog will open. It will list the already matched Ports/Sheet Entries on the right side of the dialog, with the unmatched Ports and Sheet Entries listed in two columns on the left side of the dialog.

The Synchronize Ports to Sheet Entries dialog is used to check and correct any mismatches between Ports and Sheet Entries
The Synchronize Ports to Sheet Entries dialog is used to ensure that the Sheet Entries match with the Ports on the child sheet.
Note the two tabs, which means there are two Sheet Symbols that have Sheet Entry / Port mismatches in this design.

Focusing on the mismatches displayed on the left of the dialog, the idea is to select the Sheet Entry in the first column, then the correct Port in the second column, then click the required button in the middle of the dialog to update one of them so they are synchronized (and move to the list on the right of the dialog).

The buttons function as follows:

  • Button, update the Port to Match the Sheet Entry - use the Sheet Entry properties, and push them to the selected Port.
  • Button, update the Sheet Entry to Match the Port - use the Port properties, and push them to the selected Sheet Entry.

If multiple Sheet Entries are selected in the left-hand column, the software will synchronize each Sheet Entry with the adjacent Port in the second column. If there is no adjacent Port (or Sheet Entry), a new one is created.

If the command adds new Sheet Entries or Ports, they will need to be correctly positioned on the schematic sheet when it has finished.

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Content