Nonlinear Gap Analysis of an Airplane Wing Rib - OS-1140



Your Ad Here

In this tutorial, an existing finite element model of an aluminum wing rib model will be used to demonstrate how to perform nonlinear gap analysis using OptiStruct. HyperView will be used to post-process the stress and deformation characteristics of the rib.

image\wing_rib_model.gif

Wing rib model

There are four shell components in the model: the mounting flange, the web, the top and bottom flanges, and the lug. Gap elements have already been defined in the model and they connect the web to the lug. Coupling forces are applied to the lug and pressure loading has been defined on the top and bottom flanges of the rib joint. The mounting flange is constrained in all degrees of freedom at the four mounting hole locations and the lug is constrained for the z-displacements and rotations to prevent rigid body motion.

This tutorial will use the following steps to set up the structural model for a nonlinear gap analysis:

·      Create a cylindrical coordinate system and assign it to the gap elements

·      Create a gap property and assign it to the gap elements

·      Run a linear gap analysis

·       Post-process the results from the linear gap analysis using HyperView

·       Create a load collector to define nonlinear parameters

·       Update the subcases to include the nonlinear load collectors

·       Run a nonlinear gap static analysis

·       Post-process results using HyperView

To load the OptiStruct user profile and open the model file:

  1. Launch HyperMesh and choose the OptiStruct user profile in the User Profiles dialog.

User Profiles… can also be accessed from the Preferences pull-down menu on the toolbar.

  1. Click the Files panel toolbar button image\files_panel.gif.

  2. Select the hm file subpanel using the radio buttons on the left-hand side of the panel.

  3. Click retrieve….

An Open file… browser window pops up.

  1. Select the rib.hm file, located in <install_directory>/tutorials/os/.

  2. Click Open.

  3. The rib.hm database is loaded into the current HyperMesh session, replacing any existing data.

  4. Click return to go to the main menu.

To create a cylindrical coordinate system and assign it to the gap elements:

For gap elements with coincident nodes as is the case here, the gap coordinate system MUST be specified. For detailed information, please refer to the online help section on CGAP.

  1. Click the Collectors toolbar button image\collectors.gif.

  2. Click the collector type switch and choose system collectors.

  3. Click the card image switch and select no card image from the pop-up menu.

  4. Click on name = and type cylindrical.

  5. Click color and pick a color from the palette.

  6. Click return.

  7. Click the Collector Visibility toolbar button image\collector_visibility.gif.

  8. Make sure that the entity selection switch on the right side of the panel is set as comps.

  9. Select only the Lug component.

Right-click any component’s check box to deselect it, or click the green none button to deselect all, and then check the box beside the component to be selected.

  1. Click the entity selection switch and change from comps to loadcols.

  2. Click the green none button to deselect all.

  3. Click return.

  4. Press V on the keyboard to get view options and choose top.

  5. Press F4 and select three nodes using the radio buttons on the left.

  6. Pick any three nodes on the outer circumference of the top lug as shown in the following figure.

image\3_nodes.gif

Selection of any three nodes on the top of the Lug component to find circle center

  1. Click in circle’s center.

A temporary node at the center of the circle should be created.

  1. Click return.

  2. Go to the Analysis page and choose the systems panel.

  3. Select create CORD2 and pick the center node created in the last sequence.

  4. Click origin and pick the center node again, click x-axis pick any node on the circumference and for xy plane, pick any node on the plane of the lug as shown in the following figure:

image\cylindrical_nodes.gif

Nodes to select for creating cylindrical coordinate system

  1. Click the switch beside rectangular and choose cylindrical.

  2. Click create.

For cylindrical systems, the x-axis defines the radial direction (q= 0) and the xy plane defines the r-q plane.

  1. Repeat this process for the bottom lug (steps 3 through 5 of this sequence).

  2. Click return.

  3. Click the Collector Visibility toolbar button image\collector_visibility.gif.

  4. Click the entity selection switch and choose comps.

  5. Select only the gap component.

  6. Click return.

  7. Click the Card Editor toolbar button image\card_editor.gif.

  8. Click the switch on the top left and choose elems.

  9. Click elems and select by window from the pop-up menu.

  10. Select the gap elements that are connected to the top lug as shown by the selected window in the following figure.

image\wind.gif

Gap elements connected to top lug

  1. Click select entities.

  2. Click config= and select gap from the pop-up menu.

  3. Click edit.

  4. Click CID, and select the system that was created at the center of the top lug as shown below.

image\lug_center.gif

  1. Click return twice.

  2. Repeat this process for the gap elements that are connected to the bottom lug.

The gap elements have now been assigned with a cylindrical coordinate system.

To define a property card and assign it to the gap elements:

  1. Click the Collectors toolbar button image\collectors.gif.

  2. Click the collector type switch and select properties.

  3. Click card image = and select PGAP.

  4. Click name = and input gap_prop.

  5. Click color and choose a color from the palette.

  6. Click create/edit.

  7. Click on U0_opts and choose AUTO beneath it.

This way the initial gap opening is calculated automatically.

  1. Click on KA_opts and choose AUTO.

This determines the value of KA for each gap element using the stiffness of surrounding elements.

  1. Click return two times.

  2. Select the 1D page and choose the gaps panel.

  3. Choose the update subpanel.

  4. Click elems and choose by collector from the pop-up menu.

  5. Select gap by checking the box beside it.

  6. Click the green select button.

  7. Click property= and click on gap_prop.

  8. Click update.

  9. Check beside property.

  10. Click update.

The gap elements have now been updated to the new property collector.

  1. Click return.

To run a linear gap analysis:

A subcase has already been created in this HM model.

  1. From the Analysis page, select the OptiStruct panel.

  2. Click save as… following the input file: field.

A Save file… browser window pops up.

  1. Select the directory where you would like to write the file and enter the name rib_linear.fem in the File name: field.

  2. Click Save.

Note the name and location of the rib_linear.fem file displays in the input file: field.

  1. Set the memory options: toggle to memory default.

  2. Click the run options: switch and select analysis.

  3. Set the export options: toggle to all.

  4. Click OptiStruct.

This launches the OptiStruct job.

If the job was successful, new results files can be seen in the directory where the OptiStruct model file was written. The rib_linear.out file is a good place to look for error messages that will help to debug the input deck if any errors are present.

The default files written to the directory are:

rib_linear.html

HTML report of the analysis, giving a summary of the problem formulation and the results.

rib_linear.out

OptiStruct output file containing specific information on the file setup, the setup of the problem, estimates for the amount of RAM and disk space required for the run and compute time information. Review this file for warnings and errors that are flagged from processing the rib_linear.fem file.

rib_linear.h3d

HyperView binary results file

rib_linear.res

HyperMesh binary results file.

rib_linear.stat

Summary of analysis process, providing CPU information for each step during analysis process.

Post-process the results using HyperView:

  1. From the OptiStruct panel, click the HyperView button.

This will launch HyperView and load the rib_linear.h3d file, reading the model and results.

  1. Click the Entity attributes image\entity_att.gif toolbar button and undisplay all components except the Web component. You can do this by activating the Auto apply mode: check box, (activating Display off) and then clicking on the components that you want turned off in the GUI.

image\auto_apply.gif

  1. Go the Contour image\contour.gif panel and set the Result type: to Element Stresses (2D & 3D) and the type to vonMises.

  2. At the bottom right of the GUI, click in the portion circled below to activate the Load Case and Simulation Selection dialog.

image\lc_sim_dialog.gif

  1. Select Subcase 1 as listed under the Load Case list shown below and click OK.

image\sub1.gif

  1. Click Top in the view controls section from the bottom right corner of the HyperView panel to get a top view of the Web.

  2. Click Apply.

This should show the contour of stresses on the Web component under the coupled loading.

image\1140results.gif

Stress results on the Web from linear gap analysis

  1. Click File from the pull-down menu and click Exit to quit HyperView.

To create a load collector defining parameters for nonlinear static analysis:

  1. Click the Collectors toolbar button image\collectors.gif.

  2. Click the collector type switch and choose load collectors.

  3. Click card image = and select NLPARM from the pop-up menu.

  4. Click name = and enter nonlinear.

  5. Click color and pick a color from the palette.

  6. Click create/edit.

  7. Click on NINC and input 10.

NINC denotes the number of load sub-increments. If NINC is blank, then the entire loading is applied at once. An NINC of 10 signifies that the load will be sub-divided into 10 equal increments.

  1. Click on MAXITER and leave the default value of 25.

  2. The error tolerances EPSU, EPSP and EPSW can be left at their default values.

For details on these tolerances, please read the section Nonlinear Quasi-static Gap Analysis in the online help.

  1. Click return.

To update the loadsteps to include the nonlinear step:

  1. From the Analysis page, choose the subcase panel.

  2. Click review and select the Coup_Vert collector.

  3. Check the box next to NLPARM and a new area pops up.

  4. Click on = next to NLPARM and choose to the newly created nonlinear load collector.

  5. Click update.

  6. Repeat this process for the Pressure collector.

To run a nonlinear gap analysis:

  1. From the Analysis page, select the OptiStruct panel.

  2. Click save as… following the input file: field

A Save file… browser window pops up.

  1. Select the directory where you would like to write the file and enter the name for the rib_nonlinear.fem, in the File name: field.

  2. Click Save.

Note the name and location of the rib_nonlinear.fem file displays in the input file: field.

  1. Set the memory options: toggle to memory default.

  2. Click the run options: switch and select analysis.

  3. Set the export options: toggle to all.

  4. Click OptiStruct.

This launches the OptiStruct job.

If the job was successful, new results files can be seen in the directory where the rib_nonlinear.fem file was written. The rib_nonlinear.out file is a good place to look for error messages that will help to debug the input deck if any errors are present.

The default files written to the directory are:

rib_nonlinear.html

HTML report of the analysis, giving a summary of the problem formulation and the results.

rib_nonlinear.out

OptiStruct output file containing specific information on the file setup, the setup of the problem, estimates for the amount of RAM and disk space required for the run and compute time information. Review this file for warnings and errors that are flagged from processing the rib_linear.fem file.

rib_nonlinear.res

HyperMesh binary results file.

rib_nonlinear.h3d

HyperView binary results file

rib_nonlinear.stat

Summary of analysis process, providing CPU information for each step during analysis process.

To post-process results using HyperView:

  1. From the OptiStruct panel, click the HyperView button.

This will launch HyperView and load the rib_nonlinear.h3d file, reading the model and results.

  1. Go to the Entity attributes image\ent.gif panel and undisplay all the components except the Web component. You can do that by activating the Auto apply mode: to Display off and then clicking the components that you want turned off in the GUI.

image\auto_apply.gif

  1. Click the Contour panel toolbar button image\contour.gif and set the Result type: to Element Stresses (2D & 3D) and the type to vonMises.

  2. At the bottom right of the GUI, click in the portion circled below to activate the Load Case and Simulation Selection dialog.

image\sub_circled.gif

  1. Select Subcase 1 as listed under Load Case as shown below and click OK.

image\sub2.gif

  1. Click Top in the view controls section from the bottom right corner of the HyperView panel to get a top view of the Web.

  2. Click Apply.

This should show the contour of stresses on the Web component under the coupled loading.

image\1140results2.gif

Stress results on the Web from nonlinear gap analysis.

Analysis Review

Even though the deformation patterns are similar for both linear and nonlinear analyses, the stress patterns differ. Though the horizontal loads are in opposing directions in the lug, the stress distribution in the web for the linear run are the same around both the lug holes which is not correct. This happens as all the gaps are in a closed condition for the linear analysis. Nonlinear gap analysis gives more accurate representation. The gap status, open or closed, depending on loading condition can also be observed from the .out file (shown below):

ITERATION 0

NONLINEAR ITERATION SUMMARY Subcase 1 

 

LOAD FACTOR: 0.1000 

------------------------------------------------------------ 

Nonlinear Error Measures Gap Elem Status 

ITER EUI EPI EWI Open Closed

------------------------------------------------------------ 

1 9.9000E+01 1.1659E+00 1.1659E+00 23 25

2 2.9097E-02 2.5218E+02 1.1274E+01 23 25

3 8.4208E-05 1.9063E+01 1.9427E-02 22 26

4 1.4632E-06 0.0000E+00 0.0000E+00 22 26

Go To

OptiStruct Tutorials

Return to Altair HyperWorks Index