Transferring the Deformed Geometry with Stresses

Transferring the Deformed Geometry with Stresses

By Dr. Therdthai Thienthong | Regional Technical Manager | CAD-IT 

Category: Tips & Tricks 

It can be very beneficial to use the deformed geometry with stresses in ANSYS Workbench for different applications. For example, you might want to start a new simulation with the deformed shape from a previous analysis to include imperfections or to evaluate the post-deformation behavior of the structure. This can help in avoiding convergence problems in nonlinear simulations or in measuring the effect of deformations on the performance of a component under additional loading conditions. This article will show you how to transfer deformed geometry with pre-stress from one analysis system (a structural analysis) to another analysis system.  

A screenshot of a computer

Description automatically generated

Figure 1Example of Project Schematic for transferring the deformed geometry with stresses

Figure 1 shows the project schematic for transferring the deformed geometry with stresses. We need 3 components. The analysis system A is the initial conditions for system B. The deformed geometry is transferred from A6 to B3 field, and the component C will be mapped the stresses from A (manual extracting from result plot of A) to system B. The instruction is listed below: 

  1. Check the option of export in Mechanical to ensure that “Include Node Numbers” and “Include Node Location” are setting to be “Yes”.:
    Tools >> Options… >> Mechanical/Export >> Include Node Number >> Yes.
    Tools >> Options… >> Mechanical/Export >> Include Node Location >> Yes.
    This will enable both node number and location to be exported to file.  

Figure 2 The UI of the export option in Ansys Mechanical

  1. Adding the system A to perform a structural analysis as usual. A screenshot of a computer

Description automatically generated

Figure 3 Adding Analysis System A

  1. From the first analysis system (A). We need to plot and extract the result of 6 stress components.: Normal stress in X, Y, Z and Shear stress in XY, YZ, XZ

Figure 4 Example of 6 stress components

  1. Export each stress components to a text file:
    Select parameter >> RMB >> Export >> Export Text File
    1. Example of file name:
      1. Normal stress in X 🡺 Sx.txt
      2. Normal stress in Y 🡺 Sy.txt
      3. Normal stress in Z 🡺 Sz.txt
      4. Shear Stress in XY 🡺 Sxy.txt
      5. Shear Stress in YZ 🡺 Syz.txt
      6. Shear Stress in XZ 🡺 Sxz.txt

Figure 5 Exporting to text files

  1. Adding the analysis system B into the project schematic. Then connect Engineering Data from [A2] to [B2] and connect solution [A6] to model [B3] as shown in Figure 6 and update. This process will allow you to transfer the deformed geometry from [A6] to [B3].
A screenshot of a computer

Description automatically generated

Figure 6 Connection between system A and B

  1. We can also identify which result set to be transfer by right click on the [A6] and select Properties:

Figure 7 Accessing properties for the solution [A6]

Then, you will see the properties panel of [A6] where you can select the solution time of exporting the deformed geometry with a scale factor.

Figure 8 Options of exporting deformed geometry in solution [A6]

  1. Load stress components into Ansys Workbench via “External Data” [C]

Figure 9 Adding External Data

  1. Edit the External Data by double clicking on [C2]
  2. Load 6 stress components files (Sx.txt , Sy.txt , …) into External Data
  3. Setup the configuration of the loaded file based on the

Figure 10 Import configuration of 6 stress components

  1. Connecting the setup [C2] to the setup [B4] and update
    A screenshot of a computer

Description automatically generated

Figure 11 Schematic

  1. Open Setup [B4] and import pre-stress data as initial stress. Right-mouse bottom on “imported load” >> “Insert” >> “Initial Stress” 

Figure 12 Adding initial stress

  1. Configure the imported initial stress setup. Figure 13 shows the setup option of the imported initial stress.

Figure 13 Imported Initial Stress Setup

  1. After setup the Initial Stress based on Figure 14Figure 13, Right-mouse bottom on “Import Initial Stress” and click “Import Load” 
A screenshot of a computer

Description automatically generated

Figure 14 Import Load

  1. The last step is to verify that the imported stress is the same with the original.A computer screen shot of a computer program

Description automatically generated

Figure 15 The result of the imported initial stress

In conclusion, this document described how to transfer the deformed geometry with pre-stress from one analysis system to another in Ansys Workbench and Mechanical. This can help with studying the behavior of a structure after deformation simulation. The method requires exporting stress components to text files, creating a new analysis system, and importing the stress data as initial stress. The last step is to check that the imported stress matches the original. 

Similar Posts

Leave a Reply

Your email address will not be published. Required fields are marked *