Loads from File

Note: The information in this section applies to all analysis categories with the exception of mass transfer; since linear, nonlinear, thermal, fluid flow, and electrostatic analyses all accept loads from other files.

Sometimes, you have loads from a source other than the software – or from the results of a prior analysis – that you want to apply to the model. You can use Loads from File to do so.

Loads from File transfers loads from a text file – or from a prior analysis results file – to the model. The command facilitates various multiphysics scenarios and is also useful when you find it easier to calculate the load in a spreadsheet or other in-house program. In such cases, import the load – rather than entering it one-by-one through the interface. For example, you used an in-house program to calculate the temperature distribution of a model due to laser light passing through the components, and you want to apply those temperature results to a stress analysis model.

Tip: You can also import reaction forces from an electrostatic or fluid model, or temperatures from a heat transfer model, using the Loads from File dialog box.

The procedure to apply a load from another file, whether an Autodesk Simulation results file or a text file, is as follows:

  1. Select SetupLoadsLoads from File from the ribbon, or, with nothing selected, right-click in the display area of the FEA Editor and choose the Loads from File .
  2. Press the browse button in theResults File column. A dialog appears which allows you to select the results file. Use the Files of type: pull-down to select the appropriate type of file to read for the loads. See the details below for each file type.
  3. Select the file and click the Open button.
  4. Only the loads from a single load case in the selected file can be applied to a specific index (row of the spreadsheet). Select the load case in the Load Case column. In some cases, it is appropriate to import multiple sets of loads into a single model by pressing the Add Row button. The loads assigned to the other rows of the spreadsheet can be from different load cases (or time steps) in a single file, or the loads can be from different files.
  5. The loads will be placed in a specific load case or load curve in the analysis. Enter the load case/load curve in the Structural Load Case field. (Note: the name of the column may change with the analysis type.)
  6. For the loads to be multiplied by a constant value before being applied to the model, specify the constant value in the Multiplier column.
  7. Click OK.

The imported loads do not appear in the FEA Editor. They appear in the Results environment after doing a Check Model or performing the analysis.

Note:
  • Some loads, such as nodal forces, support multiple loads at the same node. For example, applying one nodal force of [0,100,0] and another nodal force of [0, 50,50] will result in 150 in the Y direction and 50 in the Z direction.
  • Other loads, such as initial nodal temperatures, support only one load at the same node. If multiple initial temperatures are loaded on the same node, the processor will use only one of the temperatures.

Unless indicated otherwise, the results in the selected file are converted from the Model Units of the results model to the Model Units of the current model. If the Model Units of the results model cannot be determined, then it is assumed that no conversion is required.

Importing Fluid Reaction Forces File or Electrostatic Reaction Forces File:

The reaction forces from a fluid flow analysis or electrostatic analysis can be imported into a stress analysis using the Loads from File command. Refer to the page, Setting Up and Performing the Analysis: General Information (Common to Multiple Analysis Types): Loads and Constraints: Force, for details on these two types of load transfer:

Importing Temperature Results File:

The temperatures from a steady state or transient heat transfer analysis can be imported into various stress analyses or transient heat transfer analyses using the Loads from File command. Refer to the page, Setting Up and Performing the Analysis: General Information (Common to Multiple Analysis Types): Loads and Constraints: Temperature, for details on transferring temperature results to a structural analysis. For more information regarding transferring temperatures to a transient heat transfer analysis, see the page, Setting Up and Performing the Analysis: Analysis-Specific Information: Thermal Analyses: Analyses Parameters: Transient Heat Transfer.

Note: There are two methods that can be used to transfer temperatures into a structural or thermal analysis—one via the Analysis Parameters dialog box and one vie the Loads from File command. Both methods are discussed within the above-referenced pages.

Importing ASCII XYZ Results File:

Selecting a file type of ASCII XYZ Results File will import nodal-based loads specified by X,Y,Z coordinate and apply the loads to the nodes in the model with the same coordinate. The tolerance used for the comparison is 1E-6. (If more than one node has the same coordinate, the load is applied to the first node.) The file to import must have an extension of .xyz to be recognized.

Any type of nodal load supported can be defined in the ASCII file.

The format of this file must be as follows. Other than the addition of the X, Y, Z coordinate of the load, the format of the file must be identical to the nodal condition table (nodecond.dbf located in the modelname.ds_data\design scenario\ds.mod folder). Each item needs to be on the same row of the file and separated by a comma.

  • Nodal condition Type
  • X coordinate of the load
  • Y coordinate of the load
  • Z coordinate of the load
  • X value of the load
  • Y value of the load
  • Z value of the load
  • Load case number for the load. Remember: only load case numbers in the file that match the load case number selected in the user interface are transferred.
  • Property Identification of the load. This is an ID number which points to AnalysisTypeMaster.Loading.Prop(Prop_ID) which enables the user to add an arbitrary number of additional properties to this load. Normally this value is 0.
Note: The result or value of the load in the ASCII file must be in the same units as the current Model Units. The values will not be converted when imported.

Importing ASCII Nodal Condition Data File:

Selecting a file type of ASCII Nodal Condition Data File will import nodal-based loads and apply them to the specified node. The file to import must have an extension of .nod to be recognized.

Any type of nodal load supported can be defined in the ASCII file. The format of this file must be identical to the nodal condition table (nodecond.dbf located in the modelname.ds_data\designscenario\ds.mod folder).

Note: The value of the load in the ASCII file must be in the same units as the current Model Units. The values will not be converted when imported.

Importing ASCII Element Condition Data File:

Selecting a file type of ASCII Element Condition Data File will import element-based loads and apply them to the specified element. The file to import must have an extension of .ele to be recognized.

Any type of element load supported can be defined in the ASCII file. The format of this file must be identical to the element condition table (elemcond.dbf located in the modelname.ds_data\designscenario\ds.mod folder).

Note:
  • The value of the load in the ASCII file must be in the same units as the current Model Units. The values will not be converted when imported.
  • When importing the loads from an ASCII file, additional input may be required in the model to utilize the loads. For example:
    • Certain types of loads, such as pressure (stress analysis) and convection (thermal analysis) use a global multiplier to activate the load. Be sure that the global multiplier is set on the Analysis Parameters screen.
    • Don't forget to define the number of load cases or to define the load curves as necessary for the imported loads. For example, if the linear stress model is set up for 2 load cases and a load imported from an ASCII file is assigned to load case 5, the load on load case 5 will not exist: the model has only 2 load cases! To create the additional load cases in this example, add three rows on the Multipliers tab of the Analysis Parameters screen.
    • Some loads may require input in the model table (model.dbf) or other tables to fully define the load.

Parent topic: Loads and Constraints