OS-T: 1510 Follower Loads, Nonlinear Adaptive Criteria, and Nonlinear Intermediate Results

This tutorial demonstrates how to setup Follower Loads, and the usage of Nonlinear Adaptive Criteria (NLADAPT) and how intermediate results can be requested for Nonlinear runs.

Before you begin, copy the file(s) used in this tutorial to your working directory.
You will see how the activation of Follower Loads leads to a significant difference in model behavior and results, and how inaccurate results may be output if the follower load mechanism is not taken into account. You will look at activation of Follower Loads that are concentrated forces (Beam model) and of Follower Loads that are pressures (Rubber Disk model).

os_1510_models
Figure 1. Illustration of the Models: Follower Loads. Concentrated Forces - Beam (left), Pressures - Rubber Disk Model (Right)

Launch HyperMesh and Set the OptiStruct User Profile

  1. Launch HyperMesh.
    The User Profile dialog opens.
  2. Select OptiStruct and click OK.
    This loads the user profile. It includes the appropriate template, macro menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for OptiStruct.

Set Up the Beam Model

The beam model is a curved steel beam constructed with CHEXA elements. A Force of 100 N is applied to the top cross-section of the beam. The bottom of the beam is constrained by single point constraints (SPC).

Import the Model

  1. Click File > Import > Solver Deck.
    An Import tab is added to your tab menu.
  2. For the File type, select OptiStruct.
  3. Select the Files icon files_panel.
    A Select OptiStruct file browser opens.
  4. Select the beam_fllwer.fem file you saved to your working directory.
  5. Click Open.
  6. Click Import, then click Close to close the Import tab.

Submit the Job without Follower Loads Activation

The imported model already contains the material, the property, the boundary conditions, activation of large displacement, and the loadstep. In this step, you will run the model directly to generate results.
  1. From the Analysis page, enter the OptiStruct panel.

    OS_1000_13_17
    Figure 2. Accessing the OptiStruct Panel
  2. Click save as following the input file field.
    The Save As dialog opens.
  3. Select the directory where you would like to write the OptiStruct model file and enter the name for the model, beam_fllwer.fem, in the File name field.
    For OptiStruct input decks, .fem is the recommended extension.
  4. Click Save.
    The name and location of the beam_fllwer.fem file displays in the input file field.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct. This launches the OptiStruct job.
    If the job is successful, the new results files should be in the directory from which beam_fllwer.fem was selected. The beam_fllwer.out file is a good place to look for error messages that could help debug the input deck if any errors are present.

Set Up the Model

Activate Follower Loads

Follower loads for concentrated forces do not depend on the area of the element face to whose grids they are applied. Therefore, the results will remain the same for any activation option chosen on either the FLLWER Bulk Data Entry or the PARAM,FLLWER entry. Since you only have one subcase, select the parameter PARAM,FLLWER to activate follower loading for this model.
  1. In the Model Browser, Cards folder, click PARAM.
    The PARAM entry is displayed in the Entity Editor.
  2. Activate the Follower Loads.
    1. Check the box next to FLLWER.
    2. Set VALUE to 1.
    Options 1, 2, and 3 have the same effect for concentrated loads since element face areas are not involved. Using the parameter instead of the Bulk Entry activates follower loading for all subcases in a model. If you want to only activate follower loads for specific subcases, you can use FLLWER Bulk Data and Subcase Entries.

    os_1510_fllwer
    Figure 3.

Activate Nonlinear Adaptive Criteria

Parameters that allow you to define Nonlinear Adaptive Criteria are available via the NLADAPT Bulk Data and Subcase Entries. You can typically specify time-stepping and convergence criteria for Nonlinear Analysis if you run into convergence issues. Refer to the NCUTS parameter in this exercise. Similarly, you can define the DTMIN and DTMAX parameters, some of the other parameters like NOPCL and NSTSL are intended for models with contacts.
  1. Create a load step input.
    1. In the Model Browser, right-click and select Create > Load Step Inputs.
    2. For Name, enter NLADAPT.
    3. For Config type, select Time step Parameters.
      Default type is NLADAPT
    4. Check the box next to NCUTS and enter 5 (default) in the VALUE field.
      This indicates to OptiStruct that the maximum number of cutbacks allowed to reduce the time increment is 5. OptiStruct will error out if a greater number of cutbacks is required for a particular time increment for iterative convergence.

      os_1510_ee_nladapt
      Figure 4.
  2. Edit the Nonlinear Static load step.
    1. Click the Nonlinear Static Load Step to open in the Entity Editor.
    2. Click on the field next to NLADAPT and click LoadstepInputs.


      Figure 5.
    3. In the Select LoadstepInputs dialog, select NLADAPT and click OK.

      os_1510_dialog_loadcol
      Figure 6.

Activate Nonlinear Intermediate Results

Parameters that allow you to activate Nonlinear Intermediate Results are available via the NLOUT Bulk Data and Subcase entries. The number of intervals at which intermediate results are output is controlled by the NINT parameter. The SVNONCNV parameter can be used to activate/deactivate the output of results for non-convergent solutions. This is currently turned on by default (set to YES).
  1. Create a load step input.
    1. In the Model Browser, right-click and select Create > Load Step Inputs.
    2. For Name, enter NLOUT.
    3. For Config type, select Output parameters.
      Default type is NLOUT.
    4. Check the box next to NINT, then enter 10 (default) in the VALUE field.
      This indicates to OptiStruct that the maximum number of intervals at which intermediate results are requested is 10. If the load increment from any load "n" to load "n+1" is greater than 1/NINT (in this case, 1/10 is 0.1), then the results corresponding to load level "n+1" are saved for output; otherwise, the results are not saved.
      Note: This parameter has no control over the adaptive load size selection during the incremental-iterative solution process. It only specifies the number of intervals when results are saved for output during the solution process.
  2. Edit the Nonlinear Static load step.
    1. Click the Nonlinear Static load step to open in the Entity Editor.
    2. Click on the field next to NLOUT, and click LoadstepInputs.


      Figure 7.
    3. In the Select LoadstepInputs dialog, select NLOUT and click OK.

      os_1510_dialog_nlout
      Figure 8.

Submit the Job with Follower Loads Activation

The model now consists of loads which have been identified as follower loads. Additionally, you have learned how to activate adaptive criteria for nonlinear analysis, and request results at intermediate increments.
  1. From the Analysis page, enter the OptiStruct panel.

    OS_1000_13_17
    Figure 9. Accessing the OptiStruct Panel
  2. Click save as following the input file field.
    The Save As dialog opens.
  3. Select the directory where you would like to write the OptiStruct model file and enter the name for the model, beam_fllwer_ON.fem, in the File name field.
    For OptiStruct input decks, .fem is the recommended extension.
  4. Click Save.
    The name and location of the beam_fllwer_ON.fem file displays in the input file field.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct. This launches the OptiStruct job.
    If the job is successful, the new results files should be in the directory from which beam_fllwer_ON.fem was selected. The beam_fllwer_ON.out file is a good place to look for error messages that could help debug the input deck if any errors are present.

View the Results

Displacements and Element Stresses are calculated by default and can be plotted using the Contour panel in HyperView.

Compare the displacement results between models without Follower Load activation.

  1. Launch HyperView.
  2. Click pageLayout2Vertical-24 to split the page into two windows.
  3. Load the result files by clicking fileImportModel-24 and navigating to your working directory.
    1. In the first window, load the beam_fllwer.h3d file.
    2. In the second window, load the beam_fllwer_ON.h3d file.
  4. Setup contouring for each window.
    1. Click the window to activate it, then click resultsContour-16 on the toolbar.
    2. Set Result type to Displacement (v).
    3. Click Apply.
    Note: Since you have requested results for intermediate iterations via NLOUT, you will see results for all intermediate iterations.
  5. In the Results Browser, click Load Factor and select the final increment Load Factor = 1.000000E+00.

    os_1510_load_factor
    Figure 10.
The Displacement contour results display. You can see that the activation of follower forces has modified the displacement profile significantly.

os_1510_contour_plot
Figure 11.

Set Up the Rubber Disk Model

The rubber disk model a rubber disk constructed with MATHE elements. A pressure load of 1 N/mm2 is applied to the rubber disk. The circumference of the disk is constrained via single point constraints (SPC).

Import the Model

  1. Click File > Import > Solver Deck.
    An Import tab is added to your tab menu.
  2. For the File type, select OptiStruct.
  3. Select the Files icon files_panel.
    A Select OptiStruct file browser opens.
  4. Select the disk_fllwer.fem file you saved to your working directory.
  5. Click Open.
  6. Click Import, then click Close to close the Import tab.

Set Up the Model

Create Follower Load Bulk Data Entries

In the Beam model, the follower loads for concentrated forces do not depend on the area of the element face to whose grids they are applied. Therefore, the results will remain the same for any activation option chosen on either the FLLWER Bulk Data Entry or the PARAM,FLLWER entry. Additionally, since you only had one subcase, select the parameter PARAM,FLLWER to activate follower loading for this model.

In this disk model, the loads are pressure loads which may depend on the area of the element faces to whom they are applied. Additionally, you have multiple subcases to showcase the effect of different FLLWER options. In the FLLWER Bulk Data Entry in the OptiStruct help, you will see the OPT parameter which contains the following options for the calculation of Follower Loads:
= -1, 0
Follower force calculation is not activated.
= 1 (default)
Follower effect is activated. For pressure load, both element surface area and load direction are updated during the solution. For concentrated force, only the force direction is updated.
= 2
Follower effect is activated. For pressure load, only element surface area is updated (load direction is not updated) during the solution. For concentrated force, only the force direction is involved, which is the same as OPT = 1.
= 3
Follower effect is activated. For pressure load, only load direction is updated (element surface area is not updated). For concentrated force, only the force direction is updated, which is the same as OPT = 1.
  1. In the Model Browser, right-click and select Create > Load Collector.
    A default load collector template displays in the Entity Editor.
  2. For Name, enter FLLWER_1.
  3. Set Card Image to FLLWER.
  4. Set OPT to 1.

    os_1510_ee_fllwer_1
    Figure 12.
  5. Create two more load collectors named FLLWER_2 and FLLWER_3.
    1. Set Card Image to FLLWER.
    2. Set OPT to 2 for FLLWER_2, and set OPT to 3 for FLLWER_3.

Reference the FLLWER Bulk Entries

The created FLLWER Bulk Data Entries should now be selected in the Subcase section.

  1. Edit the fllwer_1 load step.
    1. In the Model Browser, Load Steps folder, click fllwer_1.
      The load step is displayed in the Entity Editor.
    2. Check the box next to FLLWER.
    3. For ID, click Unspecified > Loadcol. In the Select Loadcol dialog, select FLLWER_1 and click OK.

      os_1510_dialog_loadcol_fllwer_1
      Figure 13.
  2. Edit the fllwer_2 load step.
    1. In the Model Browser, Load Steps folder, click fllwer_2.
      The load step is displayed in the Entity Editor.
    2. Check the box next to FLLWER.
    3. For ID, click Unspecified > Loadcol. In the Select Loadcol dialog, select FLLWER_2 and click OK.
  3. Edit the fllwer_3 load step.
    1. In the Model Browser, Load Steps folder, click fllwer_3.
      The load step is displayed in the Entity Editor.
    2. Check the box next to FLLWER.
    3. For ID, click Unspecified > Loadcol. In the Select Loadcol dialog, select FLLWER_3 and click OK.

Activate Nonlinear Intermediate Results

Parameters that allow you to activate Nonlinear Intermediate Results are available via the NLOUT Bulk Data and Subcase Entries.

The number of intervals at which intermediate results are output is controlled by the NINT parameter. The SVNONCNV parameter can be used to activate/deactivate the output of results for non-convergent solutions. This is currently turned on by default (set to YES).

  1. Create a load step input.
    1. In the Model Browser, right-click and select Create > Load Step Inputs.
    2. For Name, enter NLOUT.
    3. For Config type, select Output Parameters.
      Default type is NLOUT.
    4. Check the box next to NINT, enter 10 (Default) in the VALUE field.
      This indicates to OptiStruct that the maximum number of intervals at which intermediate results are requested is 10. If the load increment from any load "n" to load "n+1" is greater than 1/NINT (in this case, 1/10 is 0.1), then the results corresponding to load level "n+1" are saved for output; otherwise, the results are not saved.
      Note: This parameter has no control over the adaptive load size selection during the incremental-iterative solution process. It only specifies the number of intervals when results are saved for output during the solution process.

      os_1510_ee_nlout
      Figure 14.
  2. Edit the fllwer_1 load step.
    1. In the Model Browser, Load Steps folder, click fllwer_1.
    2. For NLOUT, click Unspecified > Load step inputs.
    3. In the Select LoadstepInputs dialog, select NLOUT and click OK.

      os_1510_dialog_nlout2
      Figure 15.
  3. Edit the fllwer_2, fllwer_3, and NO_fllwer load steps.
    1. In the Model Browser, Load Steps folder, click the load step to edit.
      The load step is displayed in the Entity Editor.
    2. For NLOUT, click Unspecified > Load step inputs.
    3. In the Select LoadstepInputs dialog, select NLOUT and click OK.

Submit the Job with the Disk Model

The model now consists of loads which have been identified as follower loads. Additionally, you have learned how to request results at intermediate increments.
  1. From the Analysis page, enter the OptiStruct panel.

    OS_1000_13_17
    Figure 16. Accessing the OptiStruct Panel
  2. Click save as following the input file field.
    The Save As dialog opens.
  3. Select the directory where you would like to write the OptiStruct model file and enter the name for the model, disk_fllwer.fem, in the File name field.
    For OptiStruct input decks, .fem is the recommended extension.
  4. Click Save.
    The name and location of the disk_fllwer.fem file displays in the input file field.
  5. Set the export options toggle to all.
  6. Set the run options toggle to analysis.
  7. Set the memory options toggle to memory default.
  8. Click OptiStruct. This launches the OptiStruct job.
    If the job is successful, the new results files should be in the directory from which disk_fllwer.fem was selected. The disk_fllwer_ON.out file is a good place to look for error messages that could help debug the input deck if any errors are present.

View the Results

Displacements and element stresses are calculated by default and can be plotted using the Contour panel in HyperView.

Compare the displacement results between models with and without Follower Load activation.

  1. Launch HyperView.
  2. Click pageLayout2Vertical-24 to split the page into two windows.
  3. Load results from Subcase 1 to the first window.
    1. Click the first window to activate it.
    2. Load the results file by clicking fileImportModel-24. In the panel area, load the disk_fllwer_ON.h3d result file and click Apply.
    3. In the Results Browser, select Subcase 1 (fllwer_1) and Load Factor = 1.000000E+00.

      os_1510_results_hv
      Figure 17.
  4. Load results from the remaining subcases.
    1. Activate the second window and load the disk_fllwer_ON.h3d result file. In the Results Browser, select Subcase 2 (fllwer_2).
    2. Activate the third window and load the disk_fllwer_ON.h3d result file. In the Results Browser, select Subcase 2 (fllwer_3).
    3. Activate the fourth window and load the disk_fllwer_ON.h3d result file. In the Results Browser, select Subcase 2 (NO_fllwer).
  5. Setup contouring for each window.
    1. Click the window to activate it, then click resultsContour-16 on the toolbar.
    2. Set Result type to Displacement (v).
    3. Click Apply.
    Note: Since you have requested results for intermediate iterations via NLOUT, you will see results for all intermediate iterations.
The Displacement contour results display. You can see that the activation of follower forces has modified the displacement profile significantly. Additionally, you can see that since subcase 3 (OPT=3) updates the load direction but not the area, the force (Pressure*Area) distribution at the grid points is low for Subcase 3 and the Displacement results reflect this when compared to OPT=1 and 2.

os_1510_contour_plot2
Figure 18.