Utilizing Creative Routing Solutions with Tight Component Placement

November 5, 2018 Altium Designer

3D image of trace routing on a green PCB

 

When I was working in a research lab and designing PCBs for our homemade optical systems, my layouts were down and dirty. We didn’t worry about little things like packaging, limited board space, or compact routing. We were happy as long as we could get all of the required components to appear on the board and eventually the board became a printed circuit.

 

Once our microscope systems became more intricate, connecting our high speed, custom images devices to our microscopes meant that we now had to work within tight space constraints, lest we have giant PCBs with a mess of optical connections hanging off the side of an even more giant microscope. We were suddenly forced to figure out creative component layout and routing strategies just to get all our components to fit in tight spaces.

 

Unless you’re working with HDI boards, or you have some tight mechanical constraints in your device, you’re probably not worried about available real estate on your board. As component density increases and more connections are required, you’ll need to use some creative routing methods and layer stacks to make sure you can place all the required connections while operating within your design rules. The powerful CAD and routing tools in Altium Designer can help you place and route your components while conserving available board space.

Initial Schematic Capture and Layout

Working on a multilayer board with the ground plane located directly under the top signal layer can greatly improve your routing strategy. If costs or some other constraint prohibit the use of a board with four or more layers, you can still use a two-layer board with split power and ground planes, although your routing may not be as tight in all situations. Using a multilayer board allows you to place a ground plane directly below your signals, thereby reducing EMI susceptibility. You can also shorten or eliminate some connections using vias directly to the ground plane.

 

First, we want to define our layer stackup in Altium Designer. The board layers stackup, prepregs, cores, and surface material can be defined in the layer stack manager. Go to the “Design” pulldown menu and click on “Layer Stack Manager”. This dialog allows you to design your own stackup, or you can use a template in the “Presets” dropdown menu. The image below shows the four-layer stack created from a preset template.

 

Printed circuit board layer stackup in Altium Designer

Defining a four layer board in Altium Designer

 

 

This dialog lets you change a number of material properties in your board. This gives you a significant level of customizability as your real boards might use alternatives to FR-4 as the board substrate. You can also define drill pairs between layers, and you can add or remove layers from a present stackup. For now, we’ll stick with a four-layer board so that we can easily drop some of our signals to ground as needed.

 

By default, the board will only define a drill pair between the “Component Side” and “Solder Side” layers. Here we want to define drill pairs between the “Component Side” and “Ground Plane” layers, as well as a drill pair between the “Component Side” and “Power Plane” layers.

 

Screenshot of the drill pair dialog in Altium Designer

Defining a drill pairs in our four layer board

 

Altium Designer includes a number of interactive routing features that make it easy to get started routing your board, especially when you are working with high pin density components like FPGAs. Depending on your layer stack and drill pairs you defined for your board, Altium Designer will decide how best to route your connections while still conforming to your design rules.

Capturing the Schematic as a PCB Layout

Once you’ve defined your board stackup, you can capture you schematic as an initial layout and start arranging your components. The schematic we’ll be working with includes a buffer connected to 3 1-to-32 decoders. For brevity, we’ve enabled all the 1-to-8 sections in each decoder, but you could easily control enable/disable each 1-to-8 section using a second buffer or some other circuit.

 

Screenshot of a schematic with several ICs in Altium Designer

A schematic with several ICs in Altium Designer

 

Next, you’ll need to create a new PCB and open it. Go to the “Design” menu and select “Import Changes From…”. This will open up an ECO dialog that allows you to import all changes in the schematic into your blank printed circuit board. Once you click the “Execute Changes” button, Altium Designer will check for errors followed by placing the components in the blank PCB. Your newly created layout will look something like this:

 

Screenshot of Altium Designer’s design rules in impedance calculation

The routing width rule in Altium Designer’s design rules

 

Now we can start arranging components in the way we want them to appear on the board. You’ll have plenty of freedom to arrange components as you see fit, but we would like to arrange them as tight as possible. This will prevent a transition to transmission line behavior at higher signal switching speeds and eliminate the need for termination. One possible layout is shown below:

 

Screenshot of our initial layout before finalizing routing

Our initial IC layout before finalizing routing.

 

At this point, we should decide whether we want to proceed with routing automatically or manually. If you count up the number of connections that were already defined in the schematic, you will see that there are 103 connections that need to be defined in the layout. Laying all of these connections manually would take a significant amount of time. Instead, we can specify a routing strategy and allow Altium Designer to implement it while checking against our design rules.

 

Go to the “Route” menu, and select “Auto Route” and “All…”. This will bring up the Situs Routing Strategies dialog as shown in the next image. You’ll be able to review all the applicable design rules that apply to a number of different routing strategies. You can define your own strategy as well. Here, we will use the “Default Multi Layer Board” strategy.

 

Screenshot of the Situs Routing Strategies dialog in Altium Designer 

Situs Routing Strategies dialog in Altium Designer

 

 

Click the “Route All” button to begin routing. The tool will take some time to execute as it needs to evaluate each trace against the standard design rules for your project. Once the tool finishes, connections between components will appear on the top layer, and you can now define your board shape. In a real application, the board shape will need to be larger to accommodate other components, but we can get an idea of the amount of real estate this board occupies. If you measure the board, we see this board occupies about 5.6 sq. in.

 

Screenshot of the routed board in Altium Designer

Our routed circuit board

 

Notice that staggering each of the 1-to-32 decoders gives the Auto Route tool plenty of room to place vias where necessary and prevents several traces from overlapping more than is necessary.

An Alternative, Less Effective Strategy

If we only use the default settings for a two-layer board without power or ground planes, we can also try to route this board using the Auto Route tool. Try going back to the Layer Stack Manager shown above, selecting the default two-layer configuration, and create a new blank PCB. You can now create the same layout as before and use the Auto Route tool to place your connections. The Auto Route tool will generate the layout shown below:

 

Screenshot of the finalized layout on a two layer board 

Finalized routing on a two layer board

 

 

The area occupied by this layout is about 7.2 sq. in. Using a four layer stackup allows you to use about 24% less real estate than on a two layer board. Since the four layer board includes a ground plane directly below the top layer, it will be less susceptible to EMI than the simple two layer board. Obviously, creative component placement is not the only factor affecting your board layout; the layer stack plays a critical role.

 

In case you didn’t notice, using this two layer stackup will also require us to route additional traces to a power/ground buses or individual power/ground points. This can increase the required printed circuit space even further and won’t eliminate the EMI susceptibility that is inherent in this layout.

 

Working through the schematic capture to capturing the supply chain, Altium Designer’s user-friendly workflow management solution can make sure you know the path length to getting any project off the ground. The heavily rules-driven environment in Altium Designer gives you control over your routing strategy. Couple this with the advanced CAD tools and routing features, and you’ll be able to design modern PCBs with any routing requirements. The CAD tools and routing features in Altium Designer 18.1 have set a new standard in PCB design.

 

If you want to learn more about how Altium Designer can help you implement creative routing strategies, then talk to an Altium expert today.

 

About the Author

Altium Designer

PCB Design Tools for Electronics Design and DFM. Information for EDA Leaders.

Visit Website More Content by Altium Designer
Previous Article
How to Expand Input and Output for a Microcontroller
How to Expand Input and Output for a Microcontroller

Choosing a higher pin-count microcontroller can mean increased component costs. When your microcontroller r...

Next Article
When to Prefer a Longer Trace Over an Additional Via
When to Prefer a Longer Trace Over an Additional Via

If you need to choose between a longer trace or additional vias in your PCB, here are some things to consider.