Altium NEXUS Documentation

Interfacing to the ANSYS Simulation Tools from Altium NEXUS

Created: March 27, 2020 | Updated: March 27, 2020
Applies to Altium NEXUS Client versions: 3.1, 3.2, 4 and 5
This documentation page references Altium NEXUS/NEXUS Client (part of the deployed NEXUS solution), which has been discontinued. All your PCB design, data management and collaboration needs can now be delivered by Altium Designer (with Altium Designer Enterprise Subscription) and a connected Altium 365 Workspace. Check out the FAQs page for more information.

ANSYS® Engineering Simulation Software

ANSYS develops engineering simulation software for use in a range of engineering disciplines, including electronic design. ANSYS brings together a broad range of analysis and simulation tools into a single interface, called ANSYS® Electronics Desktop™. Using ANSYS Electronics Desktop, engineers can integrate rigorous 2D and 3D physics analyses with system and circuit simulations, all inside a single framework.

ANSYS SIwave is a design platform for power integrity, signal integrity and EMI analysis, that can be used for both printed circuit boards and IC design.

ECAD software, such as Altium NEXUS, can interface to ANSYS Electronics Desktop by exporting the PCB layout as an EDB file.

Learn more about ANSYS® SIwave™

Interfacing to ANSYS® Electronics Desktop™ 

The PCB layout is transferred to ANSYS Electronics Desktop by exporting it as an EDB file. The exported file is generated by the Ansys EDB extension.

Installing the EDB Extension

To export an ANSYS EDB file, the Ansys EDB Exporter extension must be installed in Altium NEXUS.

To install the extension, click  at the top right of the application then select Extensions and Updates to access the Extensions & Updates page. Locate the Ansys EDB Exporter extension on the Purchased tab.

Hover the cursor over the icon then click  to download the extension. You will be prompted to restart Altium NEXUS in order to complete the installation of the extension.

Exporting the Design from Altium NEXUS

To export the PCB layout, along with the components and connectivity, select File » Export » Ansys EDB from the PCB editor menus.

The exported data is written into a file in an automatically created EDB folder, named as follows:

\[Project folder]\[Project name].edb\edb.def

Exported Data

The following PCB objects are exported:

  • Copper objects (tracks, arcs, fills, regions, polygons, pads)
  • Vias
  • Components
  • Board layers, including the following supported layer material properties (defined in the Layer Stack Manager):
    • Permittivity (note that the Permittivity (dielectric constant) is set only for dielectric layers).
    • Permeability
    • Conductivity (the default value of 5.8e7 is set for electric layers).
    • DielectricLossTangent
    • MagneticLossTangent
  • Board outline, from the Altium NEXUS board shape (irregular board shapes are supported, board cutouts are not supported).
No custom properties are currently supported. Also note that the following predefined software material names (as defined in ANSYS software) are used: solder, solderMask, FR4_epoxy (for dielectrics), copper (for electrical layers). ANSYS software recognizes material by its name.

Exported Component Data

For each component, the following component data is exported:

  • ComponentType - mapped to the Part Type property in ANSYS.
    The component type (resistor, capacitor, inductor) is deduced from the component's designator prefix, R - resistor, L - inductor, C- capacitor. Components with any other designator prefix are assigned the Part Type property value of Other in ANSYS.
  • Component Value - mapped to the R, L or C property for RLC components in the ANSYS component model (accessed through the Model Info button in ANSYS).
    The EDB exporter checks for the component value in:
    • a named parameter - Resistance, Capacitance or Inductance, or
    • a parameter called Value, or
    • the Comment parameter
    • if not detected, a default value is used (resistance - 50Ohm, capacitance - 1nF, inductance - 1pH). These defaults are recommended by ANSYS.
  • Footprint - the footprint name is mapped to the Part property in ANSYS.

Importing the Design into ANSYS

Once the PCB design has been exported as an EDB.def file, it can be imported into any ANSYS tool that supports EDB Import.

In ANSYS, this is done via the File » Import » EDB command.


Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: