Tutorial - Creating and Configuring the PCB Document in Altium Designer

Parent page: Tutorial - A Complete Design Walkthrough with Altium Designer

Creating a New PCB

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.

The blank PCB has been added to the project and saved, and the project has been saved locally.

Configuring the Board Shape and Location

There are a number of attributes of this blank board that need to be changed before transferring the design from the schematic editor, including:

The board size has been defined, and the units, origin and grid have been set. The required layers will be configured shortly.

Configuring the Defaults

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

1. 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.
2. Default settings – if an applicable design rule does not exist or does not apply, the properties of the object 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, the software 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.

Transferring the Design

Main page: Managing Design Changes between the Schematic & the PCB

The design is transferred directly between the schematic editor and the PCB editor; there is no intermediate netlist file created. From the schematic editor, select Design » Update PCB Document Multivibrator.PcbDoc, or from the PCB editor, select Design » Import Changes from Multivibrator.PrjPcb.

When you run either of these commands, a set of Engineering Change Orders is created, which:

• List all components used in the design and the footprint required for each. When the ECOs are executed, the software will attempt to locate each footprint and place each into the PCB design space. If the footprint is not available, an error will occur. For this tutorial, all of the components have been acquired to the connected Workspace from the Manufacturer Part Search panel, so the software can reference back to the Workspace and retrieve each footprint.
• A list of all nets (connected component pins) is created. When the ECOs are executed, the software will add each net to the PCB then attempt 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 was 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.

  
  Once the ECOs have been executed, the components are placed outside the board shape and the nets are created. Note that the default Designator (and Comment) fonts have been changed.

Configuring the Display of Layers

Once all of the ECOs have been executed, the components and nets will appear in the PCB design space to the right of the board outline, as shown in the image above. Before you start positioning the components on the board, you need to configure certain PCB design space and board settings, such as the layers, the grid, and the design rules.

Your view of your board is a bird's-eye view – 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.

You design the board looking down into a stack of layers; hover the cursor over the image to show the same board in 3D, stretched in the Z-axis.

As well as the layers used to fabricate the board, which include: signal, power plane, mask, and silkscreen layers, the PCB Editor also supports numerous other non-electrical layers. The layers are often grouped in the following way:

• Electrical Layers – includes the 32 signal layers and 16 internal power plane layers.
• Component Layers – layers used in the design of the components including Overlay (silkscreen), Solder, and Paste layers. If an object is placed in a component footprint on one of these layers in the library editor, when the component is flipped from the top side to the bottom side of the board, all objects detected on a Component layer are flipped to their partner Component layer. This includes objects on user-defined Component Layer Pairs (paired mechanical layers).
• Mechanical Layers – the software supports unlimited general-purpose mechanical layers, which are used for design tasks such as dimensions, fabrication details, assembly instructions, and so on. These layers can be selectively included in print and Gerber output generation if required. Mechanical layers can also be paired; when they are paired, they behave as Component Layers. Paired Component Layers are used for tasks such as 3D body placement, glue dots, and selective gold plating on edge connectors.
• Other Layers – these include the Keep-Out layer (used to define keepouts that apply on all copper layers), the multi-layer (used for objects present on all signal layers, such as pads and vias), the Drill Drawing layer (used to place drilling information, such as a drill table), and the Drill Guide layer (used to display markers that indicate drill locations and sizes).

The copper layers are added and removed from the design in the Layer Stack, which is discussed shortly. All other layers are enabled and configured in the View Configuration panel.

Displaying Layers – View Configuration

Panel page: View Configuration

The display attributes of all layers are configured in the View Configuration panel. To open the panel:

• Click the button at the bottom right of the application window then select View Configuration from the menu, or
• Select the View » Panels » View Configuration menu entry, or
• Press the L shortcut, or
• Click the current layer color icon at the bottom-left of the design space.

   
The two tabs of the View Configuration panel

As well as the layer display state and color settings, the View Configuration panel also gives access to other display settings including:

• Color and visibility of System Colors, such as the Selection color, or if Connection Lines are visible.
• How each type of object is displayed (solid or draft), and its transparency (Object Visibility section).
• Various view options, such as if the Origin Marker, Pad Net names, and Pad Numbers are to be displayed (Additional Options section).
• The amount the display is faded when objects are dimmed or masked (Mask and Dim Settings section).
• The creation of Layer Sets, which provide a quick way of switching which layers are currently visible, using the control (Layers section).
• The creation and selection of View Configurations, which are used to pre-configure all of the layer properties, such as color, visibility, object transparency, and so on (General Settings section).

Physical Layers and the Layer Stack Manager

Main page: Defining the Layer Stack

The definition of the PCB layer stack is a critical element of successful printed circuit board design. No longer just a series of simple copper connections that transfer electrical energy, the routing of many modern PCBs is designed as a series of circuit elements, or transmission lines.

There are also numerous other design considerations that come into play when designing a modern, high-speed PCB, including: layer-pairing, careful via design, possible back drilling requirements, rigid/flex requirements, copper balancing, layer stack symmetry, and material compliance.

These layer stack requirements are configured in the Layer Stack Manager, select Design » Layer Stack Manager to open it.

The Layer Stack Manager is used to:

• Add, remove and order the signal, plane, and dielectric layers.
• Select the Material properties from the Materials Library, or configure them manually.
• Add additional user-defined fields to the Layer Stack.
• Configure the allowed Via Types, defining which layers each Via Type spans.
• Configure the Impedance profiles, when controlled impedance routing is being used.
• Configure advanced features, including rigid-flex design, printed electronics, and back drilling.

This tutorial PCB is a simple design and can be routed as a single-sided board, or a double-sided board with thru-hole vias. In the image below, the Material for each layer has been selected.

The properties of the physical layers are defined in the Layer Stack Manager. To configure the allowed via types, click the Via Types tab at the bottom of the Layer Stack Manager.

Configuring the Grid

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

Imperial or Metric Grid?

Traditionally, the grid was selected to suit the component pin pitch and the routing technology that you planned to use for the board, i.e. how wide do the tracks need to be, and what clearance is needed between tracks. The basic idea is to have both the tracks and clearances as wide as possible to lower the fabrication costs and improve reliability. Of course, the selection of track/clearance is ultimately driven by what can be achieved on each design, which comes down to how tightly the components and routing must be packed to get the board placed and routed.

Over time, components and their pins have dramatically shrunk in size, as has the spacing of their pins. The component dimensions and the spacing of their pins have moved from being predominantly imperial with thru-hole pins to more-often being metric dimensions with surface mount pins. If you are starting a new board design, unless there is a strong reason, such as designing a replacement board to fit into an existing (imperial) product, you are better off working in metric. Why? Because the older, imperial components have big pins with lots of room between them. On the other hand, the small, surface mount devices are built using metric measurements – they are the ones that need a high level of accuracy to ensure that the fabricated/assembled/functional product works and is reliable. Also, the PCB editor can easily handle routing to off-grid pins, so working with imperial components on a metric board is not onerous.

Suitable Grid Settings

For a design such as this simple tutorial circuit, practical grid and design rule settings should be:

While it might be tempting to select a very fine routing grid so that routing can effectively be placed anywhere, this is not a good approach. Why? Because the point of setting the grid to be equal to or a fraction of the track+clearance is to ensure that the tracks are placed so that they do not waste potential routing space, which can happen if a very fine grid is used.

Setting the Snap Grid

Related pages: Grid Manager, Cartesian Grid Editor, Polar Grid Editor

The value of the snap grid you need for this tutorial can be configured by pressing:

• G to display the Snap Grid menu, where you can select an imperial or metric value (note the shortcuts shown in the menu).
• Ctrl+Shift+G to open the Snap Grid dialog, where you can type in a new grid value.
• Ctrl+G to open the Cartesian Grid Editor dialog, where you can enter the grid value, as well as configure how the grid is displayed (shown below).
• Editing the grid in the Grid Manager section of the Properties panel.

Set the Snap Grid to 1 mm, ready to position the components.