Impedance Calculation and Cross Section Features in PCB Layout

October 22, 2018 Altium Designer

 Image of 3D PCB trace routing in impedance calculation

 

 

When I first started laying out printed circuit boards, there wasn’t a lot of concern about controlled impedance routing. At that time most everything was low speed and we were using larger traces and thru-hole vias for the simple four layer boards that we were working with. That changed very quickly though as those boards grew in complexity and speed. These changes demanded that we become more involved with how the boards were stacked up and what kind of trace widths we were using. At first we relied on board constraint information from different sources and personnel that we worked with, and eventually, we started using impedance calculators ourselves to set up our board stacks and design rules.

 

Fortunately, the next step in CAD tools is now here, and it is a pleasure to work with. Instead of doing the impedance calculations ourselves and manually setting up the design rules, the calculators are embedded within the PCB design tools and their information is passed on directly on to the design rules. Altium Designer is a great example of a PCB layout system where this information is fed directly into the design rules from the layer stack. If this sounds like something that would be helpful to your workflow, read on and I’ll show you how it works.

Creating the PCB Layer Stack in the Layout Tools

Altium Designer has been built to do its impedance calculations automatically. You don’t have to start the calculator from a menu or engage it somehow. It takes its information from the board layer stackup, performs the calculations, and then feeds the results directly to the design rules. This saves you a lot of time and effort in searching for an online calculator to use or finding one that you can run as an app on your phone, and then manually entering the data and retrieving the results.

 

In order for Altium Designer to correctly calculate the impedance, you must first make sure that it has the necessary data to work with. To do this you will work with the layer stack manager to configure the circuit board layer stack and input the board material widths (both copper and dielectric) as well as the dielectric constant. The impedance calculator will then use this information along with the target impedance values to make its trace width calculations.

 

To configure the board layers and input the material widths, go to the “Design” pulldown menu and click on “Layer Stack Manager”. You can build your own board layer stack or you can choose to work with one of the layer templates available in the “Presets” button. Below is a picture of the eight layer stack created from the presets.

 

Screenshot of Altium Designer’s layer stack manager in impedance calculation

Setting up your layers in Altium Designer

 

As you can see above, the layer stack manager gives you the ability to change the following board layer attributes:

  • Layer Name
  • Type
  • Material
  • Thickness
  • Dielectric Material
  • Dielectric Constant

The layer stack manager also gives you control over many other functions such as adding and deleting layers as well as defining drill pairs. You can also see the button for making changes to the impedance calculator, but we will talk more about that later.

 

Altium Designer will base its impedance calculations on the configuration of the layers in your design. For a signal layer that has a plane layer next to it only on one side, such as the top or bottom layers of the board, the calculator will use an industry standard microstrip formula. For those signal layers that have planes on both sides, such as an internal signal layer, the calculator will use an industry standard stripline formula. The calculator works with either the microstrip or stripline configurations and does not support an offset stripline configuration.

Direct from the Impedance Calculator and Into the Design Rules

Although the impedance calculator will function automatically, you do have to configure the design rules to accept the automatic values. To do that you need to close the layer stack manager by clicking OK, then go to “Design” pulldown menu and select “Rules”. Scroll down the list of rules and click on the “Width” rule as shown in the picture below. In your designs you may have many width rules, this is just an example.

 

Screenshot of Altium Designer’s design rules in impedance calculation

The routing width rule in Altium Designer’s design rules

 

In the rule shown in the picture above we have enabled the impedance calculator to set our trace width by clicking on “Characteristic Impedance Driven Width”. We have also kept the default impedance value for the trace at 50 ohms. You change this value, which we will do later, but for now, we will leave it at the default. You can see that the trace widths have very specific values because of these settings with a preferred size of 16.881 mils for the top layer.

 

To demonstrate how the calculator works, we will close the rule by clicking OK, and then re-open the layer stack manager. In the picture of the layer stack manager below you can see that we have approximately doubled the thickness value for each layer. Obviously, this wouldn’t happen in real life as this is just for demonstration purposes.

 

Screenshot of Altium Designer’s layer stack manager with changed values in impedance calculation

Changing the material thicknesses in Altium Designer’s layer stack manager

 

Once we have finished with our new layer width values, as shown above, we will close the layer stack manager by clicking OK again. With the new layer width values now in place, we will re-open the design rules and look at our width rule again. As you can see in the picture below our trace width values have all changed. We used to have a preferred size of 16.881 mils for the top layer trace width, and now it is 31.737 mils.

 

Screenshot of Altium Designer’s changed width rule in impedance calculation

The effect of the changed material thicknesses on Altium Designer’s width rule

 

 

As we have shown, you can change the trace width of your routing rules by changing the thickness of your board materials. You can also make changes in your trace widths by adjusting the impedance of the trace that you are routing. In the picture below you can see that we’ve changed the impedance of the trace from 50 ohms down to 40 ohms. The trace widths have adjusted once again, and now you can see that the preferred trace width on the top layer is 45.321 mils.

 

 Screenshot of Altium Designer’s changed width rule after changing the impedance calculation

The effect of changing the trace impedance on Altium Designer’s width rule

 

Working with the Tools to Change the Impedance Calculations

The formulas that Altium Designer’s impedance calculator uses by default are industry standard formulas for calculating microstrip and stripline trace widths. You can change these calculations if you wish however by going into the impedance formula editor. This is found by clicking on the Impedance Calculator button in the layer stack manager dialog. Once in the editor, you can make changes to the string of text that makes up the “Calculated Impedance” and “Calculated Trace Width” formulas. Below is a picture of the editor and the formulas used for calculating stripline impedance and trace routing widths.

 

Screenshot of Altium Designer’s formula editor in impedance calculation

Altium Designer’s formula for stripline trace width calculations

 

Altium Designer also gives you some help with the impedance formula editor by clicking on the “Helper” buttons to the right of the formulas. This will open up Altium Designer’s standard “Query Helper” dialog as shown below. You can use this tool to help with different function keywords and operators as well as the “Check Syntax” feature to check your work for errors.

 

Screenshot of Altium Designer’s query helper in impedance calculation

Altium Designer’s query helper for changing the impedance calculation formula

 

With the impedance calculator in Altium Designer, you can drive your design rules and trace widths instead of trying to guesstimate the rules in yourself. Along with the high speed design rules and the other analyzers and simulators in Altium Designer, you have a powerful set of PCB design tools to help you route your board the way it needs to be done.

 

When trying to work through input impedance and output impedance, voltage and resistance, inductance and capacitance, current flow and other signal integrity equations, you’ll want to make sure you have the PCB design software you can trust. Especially when working with a conductor or capacitor, avoiding a short circuit, or managing complex impedance. Otherwise, voltage resistance might not be the only resistance your designs face.

 

Altium Designer is advanced PCB design software that has been created specifically to help you with your controlled impedance routing and all other aspects of designing your printed circuit boards. To find out more how Altium can help you today, talk to an expert at Altium.

 

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
Easily Placed Surface Mount Technology with 3D Viewing Software
Easily Placed Surface Mount Technology with 3D Viewing Software

With 3D viewing software in your PCB design tools, you will have a better perspective of your surface mount...

Next Article
HDI PCB Designs and the CAD Tools Behind Them
HDI PCB Designs and the CAD Tools Behind Them

Printed circuit boards manufactured with high density interconnect technology is here to stay. See what kin...