Altium Designer Documentation

Interfacing to the ANSYS Simulation Tools from Altium Designer

Created: October 3, 2022 | Updated: October 3, 2022
All Contents

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 Designer, 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 Designer.

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 Designer in order to complete the installation of the extension.

Exporting the Design from Altium Designer

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

After launching the command, a dialog will open in which to select the desired folder for export (by default this will be the parent folder for the project). Once chosen, the Ansys EDB Export Options dialog will open - used to configure what is to be included in the export.

Component Types

  • Resistors – enter the resistor component value that is mapped to the property for RLC components in the Ansys component model that you want to be included in the export process.
  • Capacitors – enter the capacitor component value that is mapped to the property for RLC components in the Ansys component model that you want to be included in the export process.
  • Inductors – enter the inductor component value that is mapped to the property for RLC components in the Ansys component model that you want to be included in the export process.
  • Integrated Circuits – enter the integrated circuit component value that is mapped to the property for RLC components in the Ansys component model that you want to be included in the export process.
  • Input/Output – enter the input/output component value that is mapped to the property for RLC components in the Ansys component model that you want to be included in the export process.
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. The component value is mapped to the R, L or C property for RLC components in the ANSYS component model. This can be accessed through the Model Info button in ANSYS.

Units

Select either Imperial or Metric to be used as the preferred unit of measurement during export.

Others

  • Merge Net Tie Nets – when enabled, if a design contains nets connected by Net-Tie components, these nets will report as distinguished single nets in the netlist.
  • Override Part Number With – when this option is enabled, specify which parameter should be used as a Local Part Name rather than using 'Comment' by default. Enable the option then use the associated drop-down to select the desired parameter or type the parameter name into the field.

    The option is available only if the Ansys EDB Exporter extension you have installed is version 1.0.12.180 or later.

With options defined, click OK to proceed with the export. The PCB document will be saved as an *.edb file and a dialog will open confirming that the save was successful. The exported data is written into a file in an automatically created EDB folder, named as follows:

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

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

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 Designer 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.
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: