3. Board Layout Pt. I

Introduction

After you complete a schematic, the next step in the PCB design process is to conduct the layout for your board. In doing so, you're translating the theoretical arrangement of your circuit design onto a physical board that will have to operate in the real world.

During the layout process, you'll typically follow the steps below:

Board & Stackup: Outlining layers and arranging the via stack-up.
Design Rules: Configuring the constraints of the layout to your design requirements.
Component Placement: Arranging components on the board and maximizing functionality.
Routing: Connecting components together, sometimes between multiple layers.
Design Rule Check (DRC): Verifying that your layout confines to the requirements outlined in the Design Rules.

Remember, there are many solutions for a design's board layout. It's your job to determine the best viable solution!

Layout Set-Up

Before you begin, keep in mind this tutorial is a continuation of the previous module's schematic.

If you haven't already, please create the appropriate schematic by referring to 2. Creating a Schematic

To start, open the PCB document for the SPI-CAN Breakout Board project you created earlier. You should have a window similar to below:

If you zoom out of the page slightly, you'll notice an odd cross-hair on the bottom left of the window. This is the Origin, the reference point for your layout's dimensions. When placing down components at specific measurements, it's nice to have the origin level with your board.

To place the origin in the correct spot, navigate to the top-left tool bar. Then, select Edit --> select Origin --> then select Set.

Now, a green cross should appear with your cursor. Place the green cross on the bottom left corner of your board border. Once your cursor is at the desired spot, use left-click to set the origin.

Note: You can use Ctrl + Mouse Scroll Wheel to zoom in on the corner!

After zooming out, your layout should now look like what's seen below:

Now, since we only have about 15 components, we want to make our board smaller to save space and reduce manufacturing costs. To do this, we need to redefine the board shape.

In the top left tool-bar select View --> then select Board Planning Mode.

Your layout should now be in Board Planning mode, so your screen should look like this:

In the top left tool-bar, navigate to Design --> then select Edit Board Shape.

A white outline should appear around your board shape.

You'll want to change the board shape such that you have the following parameters:

Length = 2000 mils
Width = 1500 mils

To change the board lengths, pick a side (top or right, move toward the origin) and select the center of the edge. Then, click and drag the edge until your board is the correct size.

Use the legend on the top left to determine when your side is the correct size. Remember, you can zoom in to get a more precise placement.

Once you're done, your board should be a much smaller shape.

Navigate back to 2D Layout Mode (toggle View in the toolbar) until you have something that looks like this:

Layer Stack-Up

With your board size ready, we can check our layer stack-up manager. For PCB design, it's important to consider how many layers or "planes" you want on your board.

To view this, go to Design --> then select Layer Stack Manager.

You should get a new window that looks like below:

In PCB Design, you can add more than two layers to a board. For our purposes, we'll leave the the design at two layers. If you wanted to add more layers, this is where you can add them.

Design Rules

For the Design Rule Check, it's important to ensure the constraints we're applying to our layout are realistic and meet the requirements of our components. For our design, we want to modify the rules due to component pad sizes.

To start, navigate to the top left tool-bar and select Design --> then select Rules

You'll be greeted by a new window with a ton of different constraints you can apply to your design.

For our design, we want to modify the following rules:

Trace Width Constraint
Hole Size Constraint
Polygon Connect
Silk to Solder Mask Clearance

Trace Width Constraint

Open the drop-down options on the left side of the window until you reach the following page (Routing --> Width --> Width).

Modify the parameters under constraints to the following values:

Min Width: 6 mil
Preferred Width: 8 mil
Max Width: 16 mil

Hole Size Constraint

Next, navigate to the Routing Vias Page (Routing --> Routing Via Style --> RoutingVias)

Modify the parameters under the Constraints tab until you have the following values:

	Via Diameter:	Via Hole Size
Minimum	20mil	10mil
Maximum	50mil	20mil
Preferred	25mil	12mil

Next, navigate to the HoleSize module (Manufacturing --> Hole Size --> HoleSize).

Modify the Maximum parameter to 300mil.

Polygon Connect

Now, we need to change the polygon connect rules. For our power and ground Vias, we want to ensure they have easy access to their respective signals going in and out of their connected planes.

To do this, navigate to the Polygon Connect module (Plane -> Polygon ConnectStyle --> PolygonConnect).

Under Constraints, toggle on the Advanced option.

You should have a view of the full page.

Now, under Via Connection, change the Connect Style to Direct Connect.

Your page should now look like what's seen below:

Silk to Solder Mask Clearance

Finally, we need to modify the clearance constraint between the silk and solder mask. Navigate to the window below (Manufacturing --> Silk To Solder Mask Clearance --> SilkToSolderMaskClearance).

Change the Silkscreen to Object Minimum Clearance parameter to 4mil.

Finalizing Design Rules

Once you have all the rule constraints set to your needs, select the Apply option on the bottom right of the window. Then select OK.

This concludes our section on the layout set-up. To continue to the next part of the layout tutorial, navigate to this page: 4. Layout Pt. II