プロジェクトと回路図ドキュメントの作成

In Altium Designer, a PCB design project is the set of documents (files) required to specify and manufacture a printed circuit board. The project file (*.PrjPCB) is an ASCII file that lists the documents in the project as well as other project-level settings, such as the required electrical rule checks.

Creating a New PCB Project

Main page: Creating Projects and Documents

A new design project is created using the Create Project dialog.

1. Select the File » New » Project command from the main menus.

   

2. The Create Project dialog will open. In this dialog:

   1. Select the connected Workspace in the list of Locations. In the image below, the Workspace is named Company Workspace.

   2. In the Project Type region of the dialog, select <Empty> under the PCB entry.

   3. Enter a suitable name in the Project Name field, e.g., Multivibrator.

   4. Enter a suitable description in the Description field, e.g., Simple multivibrator design for the tutorial.

   5. When connected to an Altium 365 Workspace, ensure the Version Control option is enabled.

      When connected to an Enterprise Server Workspace, the Version Control option is not available in the Create Project dialog. In this case, the option is effectively checked.

   6. Enable the Constraint Management option.

      If the Constraint Management option is not available in the Create Project dialog, the design rule system will be used for the project. Depending on whether the Constraint Manager or the design rule system is used, this tutorial will provide relevant guides to complete the design.

   7. Click the Advanced control. The Folder field defines the name of the folder in the Workspace where your project will be stored. The default is to have a Projects folder in the Workspace.

   8. In the Local Storage field, select a suitable location to store the working copy of the project. A folder of the same name as the project will automatically be created in this location, and the working copy of the project file will be saved in it.

   

3. Click the  button at the bottom right of the dialog to close it and create the project. This will take a few moments, as the project is created in the working folder and in the Workspace.

An entry for the new project, Multivibrator.PrjPCB, will appear in the Projects panel. A small green check () will be displayed next to the project entry. This indicates that the version of the document opened in Altium Designer is the same as the version of the document stored in the Workspace (they are synchronized).

To provide a quick visual summary of document states, document entries in the Projects panel are accompanied by icons that indicate their open/modified status and their status in relation to the version control system (VCS). Some document icons that you might encounter when working on this tutorial project and their meanings are listed below.

	Open	The document is open.
	Open and locally modified	The document is open and has been modified (yet to be saved locally).
	No modification	The local copy of the document matches the document in the Workspace and is up to date.
	Modified	The local copy of the document has been modified and saved locally but is not yet saved to the Workspace.

To learn more about document status indication, refer to Indicating Document Status.

Adding a Schematic Document to the Project

Main page: Creating Projects and Documents

The next step is to add a new schematic document to the project.

1. Right-click on the project entry in the Projects panel then select the Add New to Project » Schematic command from the context menu. A blank schematic sheet named Sheet1.SchDoc will open in the design space and an entry for this schematic will appear linked to the project in the Projects panel under the Source Documents entry.

   When connected to the Enterprise Server Workspace, the Select configuration item dialog will open after selecting Add New to Project » Schematic. Select a schematic template from those stored in your Workspace (e.g., ANSI B Landscape) and click the OK button ().

   When the blank schematic sheet opens, you will notice that the design space changes. The main menu bar includes new items, and a bar with buttons becomes visible at the top of the design space – you are now in the Schematic editor. Each editor presents its own set of menus and panels and supports its own set of shortcut keys.

   ❯ ❮ Javascript ID: Tutorial_AddNewSchematic_AD25

2. To save the new schematic document locally, select the Save As command from the right-click menu of the document entry in the Projects panel. The Save As dialog will open, ready to save the schematic in the same location as the project file. Type the name Multivibrator in the File name field and click the Save button.

   There is no need to type in the file extension as it will be added automatically.

   

3. Because a new document was added to the project, the project file has changed. Right-click on the project entry in the Projects panel then select Save from the context menu to save the project locally. The VCS status of the project file will change to Modified indicated by the  icon.

   

4. Save the new schematic and the modified project file to the Workspace. To do this:

   1. Click the Save to Server control next to the project entry in the Projects panel.

      

   2. The Save to Server dialog will open. Enter a meaningful comment that describes the change into the Comment field (e.g., A new blank schematic sheet added), then click the OK button. When saving is complete, the VCS status of the project file and the schematic document will change to No modification indicated by the  icon.

      

Configuring Schematic Document Options

Main page: Setting Up a Schematic Document

Before you start capturing the circuit, it is good to set up the schematic document options as required, including the sheet size, as well as the snap and visible grids. The properties of most entities, including the schematic sheet, are configured in the interactive Properties panel. The panel displays the properties of the selected object, or if no object is selected, it displays the properties of the schematic sheet.

1. Make the Properties panel visible by clicking the button at the bottom right of the design space and selecting Properties from the menu that opens.

   

2. Select a template for the schematic sheet from those that are stored in your Workspace.

   When connected to the Enterprise Server Workspace, skip this step because the required template was already selected when you created the schematic document.

   To do this:

   1. In the Page Options region of the General tab, select Template for the Formatting and Size option, then select the ANSI B Landscape template under the entry of your connected Workspace in the Template drop-down.

      

   2. The Update Template dialog will open. Select Just this document for the Choose Document Scope option and Add new parameters that exist in the template only for the Choose Parameter Actions option, then click the OK button. In the information dialog that opens, click the OK button.

      

3. In the General region of the General tab, set the 100mil value for the Visible Grid and Snap Grid.

   

4. To make the document fill the design space, select the View » Fit Document command from the main menus.

   

5. Save the schematic document locally by right-clicking its entry in the Projects panel and selecting Save from the context menu.