Altium Designer Documentation
Analyzing Your PCB Design in Altium Designer
Analyzing Design Signal Integrity in Altium Designer
Signal Integrity Analysis (by Altium)
Altium Designer includes pre-layout and post-layout Signal Integrity analysis capabilities. Altium Designer's Signal Integrity Analyzer uses sophisticated transmission line calculations and I/O buffer macro-model information as input for simulations. Based on a fast reflection and crosstalk simulator model, the Signal Integrity Analyzer produces accurate simulations using industry-proven algorithms.
Preliminary impedance and reflection simulations can be run from your source schematics prior to final board layout and routing. This allows you to address potential Signal Integrity issues, such as mismatched net impedances, before committing to board layout.
Full impedance, signal reflection and crosstalk analysis can be run on your final board (or a partially routed board) to check the real-world performance of your design. Signal Integrity screening is built into the Altium Designer design rules system, allowing you to check for Signal Integrity violations as part of the normal board DRC (Design Rule Checking) process. When Signal Integrity issues are found, Altium Designer shows you the effects of various termination options, allowing you to find the best solution before modifying your design.
The Signal Integrity Analysis capabilities are available through an Altium Designer Signal Integrity Analysis system extension, which is not installed with Altium Designer by default. The extension can be installed/removed or updated from the Altium Designer Extensions and Updates page (select the Extensions and Updates option from the system User menu – 
). When not installed, the Signal Integrity Analysis extension is located within the Purchased tab. Hover the cursor over the extension and click the 
icon at the top-right of its entry.
See Extending & Updating Your Installation for more information on installing and managing Altium Designer extensions.
Running a Signal Integrity Analysis from a Schematic-Only Project
You can perform a Signal Integrity analysis on the design using only a schematic whenever there is no PCB as part of the project. The schematic must be part of a project, as analyses will not run on documents opened as Free Documents. There is no crosstalk analysis available because routed nets are required for this analysis.
When running in schematic only mode, default average track length and impedance can be defined using the Signal Integrity setup options. The Signal Integrity Analyzer also reads the PCB design rules from the schematic for the stimulus and supply nets. These rules can be added as PCB Layout directives or Parameter Set directives on nets in the schematic.
From the schematic editor, with the schematic open, select Tools » Signal Integrity from the menus. This will first allow you to setup any necessary signal integrity models and then show the Signal Integrity panel from where you can view initial results and perform further analysis.
Running a Signal Integrity Analysis from a PCB Project
When running a Signal Integrity analysis from a PCB document, the PCB must be part of a project along with the related schematics. Note that you could also run Signal Integrity from any of the schematic documents in the project and it will have the same effect as running it from the PCB. This will allow both reflection and crosstalk analysis to be performed.
From the PCB editor, select Tools » Signal Integrity which will proceed through the same process as that described above for the schematic only mode.
You can now have some (or none) of the schematic components in the PCB but any that have been placed must be linked with Component Links. This can be checked by selecting Project » Component Links. Note also that any unrouted nets will use the Manhattan length between pins to calculate a track length estimate for analysis purposes.
Refer to the following pages to learn more about performing Signal Integrity analysis in Altium Designer: