Adding a Preprocessing Feature in ANSYS AIM Structural

This section discusses customization of ANSYS AIM for the native exposure of a preprocessing feature—specifically, how to add a custom load to a structural analysis. The example used in the discussion is defined in the extension CustomPressure, which was written to create a custom pressure as a load. This example is for demonstration purposes only.

The XML extension definition file and IronPython script are addressed separately.

Custom Load Definition in the XML Extension Definition File

The XML extension definition file CustomPressure.xml follows. This code adds the custom pressure load to the project.

<extension version="1" name="CustomPressure">
  <guid shortid="CustomPressure">314bd00a-2f64-4b62-8196-bab9206c2c6b</guid>
  <script src="main.py" />

  <simdata context="Study">
    <load name="CustomPressure" version="1" caption="CustomPressure" icon="tload" issupport="false" 
    isload="true" color="#0000FF" >

      <callbacks>
        <getsolvecommands order="1">writeNodeId</getsolvecommands>
      </callbacks>

        <property name="Geometry" caption="Geometry" control="scoping">
          <attributes selection_filter="face" />
        </property>
        <property name="Expression" caption="Expression" datatype="double" control="float" 
        unit="Pressure" isparameter="true"></property>

    </load>
  </simdata>
</extension>

As in previous examples, this file first defines the extension using the attributes version and name. The <script> block specifies the IronPython script main.py.

The <simdata> block encapsulates the definition of the load. The attribute context is set to Study to indicate that the extension is for AIM. The attributes in the <load> block provide the name, version, caption, icon, support status, and color that apply to this load. The attribute color is defined in a hexadecimal format. This color is used to contrast the load when it is displayed on the model. The <callbacks> block encapsulates the function <getsolvecommands>. This IronPython function is called when the solver input file is generated by AIM. Consequently, the related IronPython function is responsible for generating the commands that describe the load within the ANSYS input file.

In the callback definition, the properties to apply to the actual definition of the load are specified. These properties are displayed in the specific ACT object created by the extension, where the user provides the necessary values to complete the load definition.

Neither of these properties requires you to define a callback.

  • The first property, Geometry, uses a scoping control type and has the attribute selection_filter set to face. This property allows the user to select the face of the geometry to which to apply the custom pressure.

  • The second property, Expression, uses a float control type, which provides the property with access to AIM expressions functionality. Consequently, you can enter an expression into the Expression field and expect a float. Setting datatype to double introduces a physical quantity dependency with the unit option, which is set to Pressure. This combination specifies that this property is consistent with a pressure. Finally, setting isparameter to true specifies that this expression can be parameterized.

Custom Load Definition in the IronPython Script

The IronPython script main.py for the extension CustomPressure follows.

def writeNodeId(load, stream):
    ExtAPI.Log.WriteMessage("writeNodeId...")
    stream.WriteLine("/com, GetSolveCommands")

    property_expression = load.PropertyByName("Expression")
    expression = property_expression.Value
    ExtAPI.Log.WriteMessage(expression.ToString())
    if expression=="": 
        return None

    property_geometry = load.PropertyByName("Geometry")
    refIds = property_geometry.Value.Ids
    ExtAPI.Log.WriteMessage(refIds.ToString())
    mesh = ExtAPI.DataModel.MeshDataByName("Mesh 1")
    for refId in refIds:
        meshRegion = mesh.MeshRegionById(refId)
        ExtAPI.Log.WriteMessage(meshRegion.ToString())
        nodeIds = meshRegion.NodeIds
        for nodeId in nodeIds:
            node = mesh.NodeById(nodeId)

            stream.WriteLine("F,"+nodeId.ToString()+", FX,"+expression.ToString()+"\n")

The script main.py defines the function writeNodeId, which writes the value of the property Expression on the geometry nodes scoped for the load.

The following figure shows how the load CustomPressure that you created in ACT is now available as a boundary condition in AIM.

 

The following figure shows the status of the load once all of the properties are defined.

 


Release 18.2 - © ANSYS, Inc. All rights reserved.