Using Altium's PDN Analyzer and Incorporating Simulation-Driven Workflow

If you’ve ever placed your hand near the vent on your computer, you can get a sense for the heat being created by the motherboard. Fans are designed to remove heat generated by the components on your motherboard, particularly by your CPU and GPU. The same effects occur in PCBs, even if they do not include components that consume a large amount of power. Power is consumed as it is delivered from the power source to the components, and power drops reduce the voltage supplied to downstream components.

Many boards don’t include a CPU or GPU, and these two components are infamous for the heat they generate during operation. There are plenty of other components and design features that can generate significant heat due to voltage drop. Once your board is manufactured and placed in operation, you won’t have time to accurately test each connection with a multimeter or measure the temperature of every component with a thermometer. This is where simulation tools become critical, allowing you to diagnose potential power delivery problems before your board enters service.

Once you have diagnosed power signal problems in your PCB, you can take steps to redesign your PCB to prevent any resulting thermal problems. The PDN Analyzer^™ feature in Altium Designer^® can help you diagnose large voltage drops and hot spots in your PCB before you move to production. Implementing this critical simulation tool into your workflow is an iterative process that can save you testing time and help prevent failed production runs.

Simulation and Workflow

When working in a CAD tool, having security and confidence in producing the board correctly is paramount. Working through simulation software and engineering simulation, though, you can make this process a reality. Engineers trying to maintain workflow management will find easy-to-translate data to be among their best allies in working through capabilities and optimization along with product development.

What simulation technology can do is improve the capabilities for computer-aided engineering designs and devices to be understood by any level of individual interacting with them. The implications to your workflow simulation can have can be as simple as quickening translation speed to increasing process simulation for materials through additive manufacturing and beyond.

Setting Up Your Simulation

Once you’ve designed your schematic, captured it as a layout, and routed connections to your liking, you can begin setting up your simulation for power density analysis. Note that you do not need to have reference designators added to every component in your schematic. Reference designators and full component identifiers will appear in the PDNA interface in Altium  , allowing you to define nominal voltage/current levels and tolerances in each net in your PCB.

Here, we’ll be analyzing a PCB for the Mini PC WiFi module that comes prepackaged with Altium . This board includes a serial-to-WiFi module that communicates over 802.11 b/g/n, and it includes a power management system. This board runs at 3.3 V, and we would like to ensure that power is adequately reaching all of the system. A screenshot of the PCB layout for this board is shown in the figure below.

Example layout of a WiFi module in Altium

We have a single power plane that supplied power to various components in parallel. Normally, when analyzing a typical circuit diagram, this use of a power plane and a ground plane with finite conductivity between connections is ignored, so it becomes important to know whether power extending throughout this plane and its reference ground plane has an appreciably low voltage drop. This is important for preventing signal integrity and noise problems particularly ground loops.

To set up the simulation, go to the “Tools” menu and select “ ”. This will bring up the “ ” window as a non-modal interface. If you have a second monitor, you can move this window to your other monitor so that it does not cover the main design interface. First, you’ll need to click the “DC Nets” button in the upper left corner of the window and select the power nets you want to use in your simulation, as shown in the figure below.

Here, you’ll notice that we only have two DC nets: our 3.3 V power net and a ground net. We want to select both of these and click the “Add Selected” button. We can now use these nets in a new simulation to define the power network we want to simulate. In more complicated PCBs, which might have multiple power and ground nets for different groups of components, you’ll see many more options.

DC nets in the Mini PC WiFi module

For now, you can click on the “File” button and click “New Simulation”. A box will appear in the center of the screen that says “Network”, and an entry in the list on the left-hand side of the screen will appear with the same name. This is the network that we’ll be simulating, and now we need to define our sources and loads to this network. If you click on this entry, a network editor will appear in the top portion of the window.

Next, click on the “<Power Net>” box in the upper portion of the window and click “Edit Net”. A window will appear that allows you to select the “3V3” net. Doing the same for the “<Ground Net>” box allows you to choose the “GND” net option. Now we’re ready to add our sources and loads to this network.

Adding sources and loads to your network allows you to run the simulator on specific portions of your PCB. These sources and their corresponding loads are listed by their reference designators, which can be found in the schematic for this board. Here, we’ll use U1 as a source with U1 and U2 as our loads. Here, we’ll set the input current to 0, which the interprets as “don’t care”. The current in each of the three loads will be set to 100 mA, although the actual current will be different during operation.

Once you’ve defined your network, you’re ready to run the simulation. Click the “Analyze” button. Once the simulation is finished, you’ll be able to see any issues as messages. Once you click over to the “Visual” tab, you’ll be able to add different layers to the output in the main PCB window. This network and the information on the “Visual” tab is shown below:

output in Altium

Inspecting Your Power Distribution

Now that the simulation is finished, we can analyze the power distribution in the power and ground layers, allowing us to identify any large voltage drops in the power and ground planes that could create noise problems, as well as the power dissipation in signal lines that could lead to thermal problems. If you examine the window, you’ll see a “Net” and “Layer” list. These lists allow you to visualize different layers and nets in your PCB, giving you a finer view of power distribution in your device.

There are also two options on the left side of the window, where you can choose to display voltage or current density throughout your device. To begin, let’s look at the current density and voltage in the signal layers. Make sure that only the “3V3” net and the “TopLayer” and “BottomLayer” layer options are selected. You’ll see slightly different windows showing power distribution in your PCB: one for voltage and another for current.

Current density (left) and voltage (right) in signal lines

If you look at the current density distribution (left), you’ll see that the copper pad in the lower right corner of the board has high current. The voltage distribution (right) also shows that this pad and its via connections have the highest voltage of anywhere in the PCB. It also connects directly to the ground plane through vias, so the voltage drop across this element is about 3.3 V. This point on the device could become a hot spot as it dissipates about 16 W of power within a 2 mm2. Other lines in this network can be examined in the same manner.

Aside from redesigning this pad, some solutions to this potential overheating problem include the use of passive elements like thermal relief pads, thermal vias connected to a landing, or a good old-fashioned fan with a heat sink. If we were looking at an IC that generated a large amount of heat, it would be best to place this IC in the center of the board in order to allow heat to conduct to the edges of the board.

Note that we confined our attention to the signal layers because the uses a color scale to visualize the power distribution in the PCB. If we include the power and ground planes, we lose the granularity that is present in the above windows. The voltage drop between the power and ground planes is 3.3 V, making it difficult visualize smaller variations in a single layer.

Instead, we can examine the potential for ground loops or other noise problems if we look at the power distribution in the ground plane. Switch the view over to voltage mode, and then select the “GND” net and the “int2_gnd” layer. When you switch back to the PCB view, you will see a power distribution that looks like the following image.

Power distribution in the ground plane

If you take a look at the voltage scale, you’ll see that the maximum voltage difference across the ground plane is only 11.3 uV. In particular, if you examine the voltage drop between any two neighboring vias, you’ll find that the voltage drop between them is on the order of nanovolts. This is a very low voltage that will not cause ground loops or create serious noise problems.

Once you’re comfortable running a PDNA simulation and you have an understanding of how the visualization helps you diagnose problem spots, you can go back to your schematic or layout, make changes to your board, and re-run the simulator to validate your design changes. This iterative process is a standard method for incorporating simulations into your design workflow. Be careful not to split existing nets into new nets, as this will require that you redesign the simulation to match your design changes.

The PDN package in Altium gives you a full view of power consumption and thermal demands in your next PCB. Combine this with the ultra-accurate CAD tools and component libraries, and you can easily modify your designs to alleviate power delivery issues in your next PCB. Altium has set a new standard in PCB design.

If you want to learn more about how Altium can help you, then talk to an Altium expert today.