Parent page: Design Reuse
There is a strong incentive to re-use sections of circuitry from existing designs; the design is proven so the engineering is complete, it saves time, it can help reduce component inventory, and it frees up your design team to focus on the development of new concepts and products.
Designers are clever people - they already reuse existing designs all the time. It might be a proven circuit that they re-capture, or perhaps they copy and paste from an existing design, or they link an existing schematic sheet into a new design.
Device Sheets simplify the design process by providing modularized and consistent building blocks that can be reused between projects. Device Sheet Symbols are placed and referenced similarly to components. They are connected to and function in the same way as a sheet symbol that is referencing a standard schematic document, but are not explicitly added to a project.
Device Sheets are building blocks developed with the intent of being reused in different designs. They usually contain predefined circuits that are useful in multiple projects, for example, a power supply.
A Device Sheet is created and stored as a normal schematic document, in a declared Device Sheet Folder. Rather than being added as a document, they are placed and referenced in a project in a similar way as a component. Device Sheets are included in the project hierarchy and can be distinguished from standard schematic documents by a different document icon in the Projects Panel.
By default, Device Sheets are usually configured to be read-only. This gives all designers in the team confidence that they are complete and ready-for-use, and also ensures that no one in the design team can inadvertently modify them. Because they are configured to be read-only, the component designators cannot be changed, nor can the schematic sheet number.
The fundamental difference between a device sheet and a regular schematic sheet is that the software has additional features to handle component annotation and the schematic sheet numbering when the project includes Device Sheets.
Device Sheetswith sub-folders to suit your company's requirements, such as
Power, and so on.
A Device Sheet can be any normal schematic sheet, including a schematic that contains Sheet Symbols that reference other schematic sheets. It is the fact that they are placed as a Device Sheet from the Device Sheet folder that flags to the software that this schematic sheet is a Device Sheet, that the Device Sheet control options defined in the Preferences dialog must be applied, and the special annotation and sheet numbering commands obeyed.
By default, Device Sheets are usually configured to be read-only. The challenge of working with Device Sheets is not protecting that chunk of design from modification, it is dealing with the design finalization tasks that are carried out when the design is complete, namely schematic sheet numbering and component annotation.
There are some preparatory steps that should be taken before a schematic is copied or moved into the Device Sheet storage folder:
A Device Sheet is used in a project by placing the Sheet Symbol that represents it. To do this:
► Learn more about Creating Connectivity.
Once you have placed a Device Sheet Symbol, open the Device Sheet itself to view its graphical properties. The default setting in the software is for Device Sheets to be read-only as configured in the Options section of the Data Management - Device Sheets page of the Preferences dialog. Note that the Read-Only option is independent of the display of the Read Only Watermark across the sheet; check the Editor tab at the bottom of the editing window to see if a sheet is ReadOnly (as shown above).
You can edit Device Sheets in one of two ways: either directly in your project or from the source schematic documents in the Device Sheet folders.
To edit Device Sheets directly in your project:
To edit Device Sheets from your Device Sheet folders:
A Device Sheet may contain Device Sheet Symbols, although a Device Sheet cannot be the top sheet in a project due to hierarchical implications. There are no limitations to the depth of the hierarchical structure when using Device Sheets.
To prepare hierarchical Device Sheets:
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 refactor tools.
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 Subcircuit to Different Sheet command (also available via the right-click menu when there is a selection). The Choose Destination Document dialog will open. When you select the target sheet then click OK, that sheet will appear with the sub-circuit floating on the cursor, ready to position.
The refactoring commands support:
► Learn more about Design Refactoring.
To guarantee the integrity of the circuitry used in a Device Sheet, that sheet should not be edited during normal design use. That means the sheet number and designator assignments should not be modified on the sheet. So just how do you number all the sheets in the project and annotate all of the components?
These tasks are managed by two commands: sheets are numbered using the Annotate Compiled Sheets command and components are annotated using the Board Level Annotation command. Sheet number and designator assignments are stored in a separate file,
Main article: Numbering the Sheets
Complimenting the Board Level Annotation feature, the Tools » Annotation » Annotate Compiled Sheets command is used to uniquely number Device Sheets without modifying the source schematics. As with component annotations, the sheet numbers are stored in the
Notes about sheet numbering:
► Learn more about Annotating Compiled Sheets.
Main article: Annotating the Components
To allow the component designators to be uniquely assigned across the entire project, the software includes a feature called Board Level Annotation. This command does not edit the source schematic sheets. Instead, it stores mapping information, mapping each logical schematic designator to a physical PCB designator as they will appear on the PCB. These designator mappings are stored in a project file called
<ProjectName>*.annotation. There is a broad range of annotation options available in the Board Level Annotate dialog.
Notes about working with Board Level Annotation, referring to the image above:
► Learn more about Board Level Annotation.
If you open a project containing Device Sheets and the location of these Device Sheets has not been declared, you will see the following dialog with a list of the Device Sheets that cannot be found.
If you click Yes, the Device Sheet Folders section of the Data Management - Device Sheets page of the Preferences dialog will open. It might be that the Include Sub-Folders option has not been enabled, otherwise, add in the new path if the Device Sheets used in the project are stored in a different location.
Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.