PCB Layout

Video Tutorial

In the previous part of the bootcamp, you validated your schematic and are ready to move on to transferring your schematic onto an actual PCB drawing that can be sent to a manufacturer.

Let’s get started.

Creating a new PCB layout

Click File → New → PCB.

You should get a large black empty square on your screen. This is your empty PCB!

The next step is to define your board stack-up, or the various layers in your design.

Click Design → Layer Stack Manager.

A page similar to the one below should appear. This is where you define the layers of your board. As you can see, there is a top overlay for silkscreen, a top solder mask layer and then your copper and dielectric layers sandwiched between more solder mask and bottom overlay. This is a basic stack-up for a 2 layer board. Clicking Add will allow you to add more layers to your board. Keep in mind that adding more layers to your board increases cost and manufacturing time, so it is best to design a board using as few layers as possible.

Open

You can also change the layer thicknesses in the board stack manager. Typically you will want to check with your manufacturer (e.g. JLCPCB) what layer sizes they have and select based on their requirements, but for the purpose of this board its fine to leave the layers thicknesses are they are right now. It is up to you, however, to decide how many layers you will need.

There are two approaches for the next step. We can either decide our board shape right now, or we can place our components on the PCB and then define our board shape after. In industry, there is often a target board shape constraint delivered by a mechanical team, but in our case the board shape is not critical, so we can define our board shape after optimizing placement.

Next is component placement. The photo below is an arbitrary placement example, but you want to drag your components around on the board and place them in the exact configuration you want. Think about the electrical theory from earlier, and try to imagine the user experience of someone handling the completed board.

Open

At this point, you want to be considering critical placement of input capacitors and output capacitors in relation to your LDO IC. Where are you going to put your feedback resistors (if included)? Where should input and output connectors be placed for easiest access to them by a user? Am I going to have large current loops? All of these are questions that you should be asking as you place your components.

Open

Example of an optimized buck converter placement.

After you’ve finished placement, the next step is to connect your nets together with traces, polygons, and vias.

Types of connections

Open

Traces: Lines of copper that transmit signal or power to/from components

Open

Polygons: Shapes/geometries filled in with copper that are used to connect a large number of components or carry large amounts of power

Open

Vias: Conductive drill holes connecting polygons and traces across different layers

To route a trace that connects a component, select the Interactively Route Connections button at the top.

Open

This will allow you to click and start a trace to connect your footprints/pads/components.

Altium will not allow you to make a connection between two pads or pieces of copper if they are not assigned to the same net.

Open

Net name highlighted in the properties panel.

You can view the net name on the trace or use the properties panel to ensure the correct net has been set.

To create polygons, select the Place Polygon Plane on the top menu bar. This will allow you to draw out a shape that will be filled in with copper.

Open

Similarly to traces, it is important to define the net that the polygon is associated with. If you make any changes to the shape of the polygon or change a setting in the properties tab, the polygon will show a DRC (design rule check) error in the form of many green circles in a grid. Be sure to select Repour whenever you make a change to a polygon.

Open

Going to Tools → Polygon Pours → Polygon Manager reveals all the polygons in your board. In this menu that you can shelve polygons (temporarily remove them) and reorder the pour priority of each polygon.

In order to place your vias, select the Place Via button on the top menu bar. This will allow you to place vias anywhere you like on the board. Note that vias need a net to be selected in the same way as traces and polygons. Additionally, placing a via on an already poured polygon will require you to repour the polygon.

Open

One thing to be aware of is your via sizes. It is very important to define the Diameter and Hole Size in the Properties tab of the via. These parameters are usually limited by your manufacturer’s capabilities (e.g. JLCPCB), and by the aspect ratio of your via.

The last step is to define your board outline. This can be done by selecting a board outline (mechanical) layer and using the Place Line or Place Rectangle tool at the top menu to create a closed shape as shown below.

Try adding chamfered corners to your rectangle to give your board rounded edges.

Open

Next, select the lines of the shape you created, and select Design → Board Shape → Define Board Shape From Selected Objects.

Open

You should be left behind with a board in the shape you defined.

Example layout

A random example board is shown below. It uses a 2-layer stack-up, with the top layer in red and the bottom layer blue. You can see all the pads for each component and green arrows pointing to vias that are used to make connections across the two layers. Note that this is not a recommendation to create a design similar to this.

Open

Design Rule Checks

During the design process, you will run into design rule errors/violations. In Altium Designer, these constraints are set in the Design → Rules… window of the layout editor. When a rule is violated, the offending components and/or copper is highlighted in green circles with an X marked in them. This indicates that according to your project’s rules, the highlighted part of the design is not manufacturable.

Open

Example: Short-circuit violation between two traces on the Top layer.

In the example above, the green circles show which parts are affected, while the beige symbol and text show the type of constraint that was violated (Short-circuit constraint), and what that rule is currently set to (0.1mm minimum). To fix a DRC error, you may need to modify one of the trace’s nets, move one trace out of the way, or modify your rule.

3 - Final Review

At this point, you should have completed the WARG EE bootcamp! Your only deliverable is your LDO PCB that you will need to present to an electrical bootcamp reviewer or team lead in Discord. You will be asked about your design (schematic, layout) and the decisions made in your component selection.