在Altium Designer中创建并配置PCB文档

You are now ready to create a PCB.

Adding a PCB Document to the Project

Before you transfer the design from the Schematic editor to the PCB editor, you need to create the blank PCB, then name and save it as part of the project.

1. Right-click on the project entry in the Projects panel then select the Add New to Project » PCB command from the context menu. A new PCB document will open and an entry for it will appear linked to the project in the Projects panel under the Source Documents entry.

   ❯ ❮ Javascript ID: Tutorial_AddNewPCB_AD25_0

2. Right-click the PCB document entry in the Projects panel and select the Save As command. The Save As dialog will open, ready to save the document in the same location as the project file. Type the name Multivibrator in the File name field and click the Save button.

3. Adding the PCB has changed the project, so save the project locally by right-clicking the project entry in the Projects panel and selecting Save.

Before transferring the design from the Schematic editor, we will also change some attributes of the new PCB.

Setting the Origin and the Measurement Units

Main page: Working with the Cursor-Snap System

The PCB editor has two origins: the absolute origin, which is the lower left of the design space, and the user-definable relative origin, which is used to determine the current design space location. The coordinates of objects in a PCB document are defined relative to the relative origin. The coordinates shown on the Status Bar are also relative to this origin. A common approach is to set the relative origin to the bottom-left corner of the board shape.

1. Zoom in to the lower left of the current board shape to easily see both the coarse and fine grids as shown in the images below.

2. To set the relative origin, select the Edit » Origin » Set command from the main menus, then position the cursor over the bottom-left corner of the board shape and click.

   

3. Select the View » Toggle Units command from the main menus to switch the measurement units of the PCB document from mils to millimeters.

   Look at the coordinates and the grid in the Status Bar to quickly check the measurement units currently in use.

   

Editing the Board Shape

Main pages: Defining the Board Shape

The default board shape is 6 x 4 inches. For this tutorial, you will change the board size to 30 x 30 mm.

1. Select a suitable snap grid. During the course of the design process, it is quite common to change grids, for example, you might use a coarse grid during component placement and a finer grid for routing. Select the View » Grids » Set Global Snap Grid command from the main menus and enter 5 in the field of the Snap Grid dialog that opens, then click OK to close the dialog.

   

2. Zoom out to show all of the board, including its edges.

3. Changing the board shape is done in board planning mode. Select the View » Board Planning Mode command from the main menus to switch to this mode (shortcut: 1). The display will change, and the board area will now be shown in green.

   

4. When in board planning mode, the PCB editor provides several commands for changing the board shape. For a simple square or rectangle, it is more efficient to edit the existing board shape. The coarse visible grid is 25 mm (5x the snap grid), and the fine visible grid is 5 mm; these can be used as a guide.

   1. Select Design » Edit Board Shape from the main menus.

   2. Editing handles will appear at each corner and the center of each edge, as shown in the video below.

      Note that clicking anywhere other than on an editing handle or an edge of the shape will drop you out of board shape editing mode.

   3. You can slide the upper edge down and slide the right edge to the left to create the correct size. To slide the upper edge down, position the cursor over the edge (but not over a handle). When the cursor changes to a double-headed arrow, click and hold, then drag the edge to the new location so that the Y cursor location is 30mm on the Status Bar, as shown in the video below.

   4. Repeat the process to move the right-hand edge in, positioning it when the X cursor location is 30mm on the Status Bar.

   5. Click anywhere in the design space to drop out of board shape editing mode.

5. Select the View » 2D Layout Mode command from the main menus to return to 2D Layout Mode (shortcut: 2).

6. Now that the shape has been defined, you can set the grid (View » Grids » Set Global Snap Grid) to a value suitable for component placement, for example, 1 mm.

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

The board size has been defined, and the units, origin, and grid have been set.

Configuring the PCB Object Defaults

When you place an object in the PCB editor design space, Altium Designer will define the shape and properties of the object based on:

• An applicable design rule – if there is a rule defined that applies to that object, the properties object are defined from the rule. For example, during a layer change when you are interactively routing, a via is automatically added with its size and hole size properties taken from the applicable Routing Via Style design rule.

• Default settings – if an applicable design rule does not exist or does not apply, the object properties are defined from the default settings configured in the PCB Editor – Defaults page of the Preferences dialog. For example, if you run the Place » Via command, Altium Designer does not know if that via will be part of a net, so it will present a via at the size defined in the defaults.

As part of this tutorial, you will configure the default properties of component designators and comments. These properties will be applied to these component strings when the components are placed on the PCB.

1. Click the  button at the top of the design space to open the Preferences dialog and then expand the PCB Editor category in the left tree and select the Defaults entry in this category to open the PCB Editor – Defaults page.

   

2. Select Designator in the Primitive List to display the default properties of this object. Confirm that the options are set as follows:

   • The Autoposition option is set to Left-Above. This is the default location in which this string is held when the component is rotated. The string can be interactively relocated at any time during the design process.

   • The Text Height value is set to 1.5mm.

   • The Font Type option is set to TrueType, and the Font is set to Arial.

   

3. Select Comment in the Primitive List and confirm that the comment visibility is set to hidden (the button at the right of the Value field is shown as ). This is a common default. Component comment strings can be selectively displayed during the design process if required.

   

4. Click OK to save the changes and close the Preferences dialog.

Transferring the Design from Schematic Capture to PCB Layout

Main page: Keeping the Schematics & PCB Synchronized

The design is transferred directly between the Schematic editor and the PCB editor; there is no intermediate netlist file created. This can be done by selecting the Design » Update PCB Document <PCBDocumentName> command from the main menus of the Schematic editor. When you run this command, a set of Engineering Change Orders (ECO) is created, which:

• List all components used in the design and the footprint required for each. When the ECOs are executed, Altium Designer attempts to locate each footprint and place each into the PCB design space.

• A list of all nets (connected component pins) is created. When the ECOs are executed, Altium Designer adds each net to the PCB and then attempts to add the pins that belong to each net. If a pin cannot be added, an error will occur. This most often happens when the footprint is not found or the pads on the footprint do not map to the pins on the symbol.

• Additional design data is then transferred, such as net and component classes.

In other words, an ECO is created for each change that needs to be made to the PCB so that it matches the schematic.

1. Click the schematic document tab at the top of the design space to make it the active document.

2. Select the Design » Update PCB Document Multivibrator.PcbDoc command from the main menus to open the Engineering Change Order dialog.

   

3. Click the  button at the bottom left of the dialog. If all changes are validated, a green check will appear next to each change in the Status – Check column of the dialog.

   

   If the changes are not validated, close the dialog, check the Messages panel, and resolve any errors.

4. If all changes are validated, click the  button to send the changes to the PCB editor. As each change is performed, a check will appear in the Status – Done column of the dialog.

   

5. When all changes have been completed, the PCB will open behind the Engineering Change Order dialog. You can close the dialog now.

6. The components are positioned outside of the board and ready for placement. Also, note that component pads of the same net are connected to each other with connection lines. 

   

There are a few steps to complete before starting the component placement process, such as configuring the placement grid and layers.

Configuring the Display of Layers

Main page: Your View of the PCB

Your view of your board is a bird's-eye view, i.e., looking down the Z-axis into the board from above. The PCB editor is a layered design environment; the objects you place on signal layers become copper when the board is fabricated, the strings you place on the overlay layers are silkscreened onto the board surface, and the notes you place onto mechanical layers become instructions on the assembly drawing that you print.

You design the board looking down into this stack of layers, placing components on the top and bottom sides of the board (Top Layer / Bottom Layer), and other design objects on the copper, overlay, mask, and mechanical layers as you build up the design. Layer display attributes and other layers are configured in the View Configuration panel.

1. Open the View Configuration panel. To do this, click the  button at the bottom right of the design space and select View Configuration from the menu.

2. In the Layers region of the panel's Layers and Colors tab, confirm that the Top Layer and Bottom Layer signal layers are visible (the visibility control at the left of layer entries is shown as ).

   

3. To have less visual "clutter" during placement and routing, disable the display of the Component Layer Pairs (except for Overlay layers), Mechanical Layers, and the Drill Guide and Drill Drawing layers.

   

4. In the Additional Options region of the panel's View Options tab, confirm that the Pad Nets and Pad Numbers options are enabled.

   

Configuring the Board Layer Stack

Main page: Defining the Layer Stack

Physical layers of a PCB (signal, plane, and dielectric layers) and other aspects related to the physical structure of the PCB such as via types and impedance profiles, are configured in the Layer Stack Manager.

This tutorial PCB is a simple design that can be routed as a double-sided board with thru-hole vias.

1. Open the Layer Stack Manager. To do this, select the Design » Layer Stack Manager command from the main menus of the PCB editor. For a new board, the default stack comprises a dielectric core, two copper layers, and the top and bottom solder mask and overlay (silkscreen) layers.

   

2. To simplify the management of layers, make sure that the Stack Symmetry option is enabled in the Board region of the Properties panel (if the panel is not visible, click the  button at the bottom right of the design space and select Properties from the menu). With this option enabled, layers are added in matching pairs, centered around the mid-dielectric layer.

   

3. To use a material for a specific layer (or pair of layers if symmetry is enabled), click the  button in the Material cell for the required layer to open the Select Material dialog.

   

   Select layer materials as follows:

   • Solder mask layers (Top Solder and Bottom Solder) – SM-001

   • Signal layers (Top Layer and Bottom Layer) – CF-004

   • Dielectric layer (Dielectric 1) – Core-043

   

4. Click on the Via Types tab at the bottom of the Layer Stack Manager and confirm that there is a Thru 1:2 type defined.

   

5. Save changes made in the Layer Stack Manager by selecting the File » Save to PCB command from the main menus.

6. Close the Layer Stack Manager by right-clicking its tab at the top of the design space and selecting the Close Multivibrator.PcbDoc [Stackup] command from the context menu.

Configuring the Snap Grid

Main page: Working with Grids & Guides

The next step is to select a suitable grid for placing the components. All the objects are placed in the PCB design space on the current snap grid.

1. If the Properties panel is not already visible, make it visible by clicking the  button at the bottom right of the design space and selecting Properties from the menu that opens. The panel displays the properties of the selected object, or if no object is selected, it displays the properties of the PCB document.

2. In the Grid Manager region of the panel's General tab, select the Global Board Snap Grid entry and click the  button. The Cartesian Grid Editor dialog will open.

   

3. In the Cartesian Grid Editor dialog:

   1. Make sure that the Step X field has the value 1mm. Because the X and Y fields are linked, there is no need to define the Step Y value.

   2. Click the color swatch for the Fine grid and select a lighter color using the Choose Color dialog that opens (e.g., select the color in row 34 on the Basic tab – ).

   3. For the Coarse grid, select Lines from the drop-down and click the Darker control to automatically set its color to a shade darker than the current fine grid color. This will make it easier to distinguish between the fine and coarse grids.

   4. Make sure that the Multiplier is set to 5x Grid Step. This will make the grid visible at lower zoom levels.

   

4. Click OK to close the dialog. The display of the grid will be updated in the design space. 

   

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