This tutorial was completed using ANSYS 7.0 The purpose of the tutorial is to show the how to use substructuring in ANSYS. Substructuring is a procedure that condenses a group of finite elements into one super-element. This reduces the required computation time and also allows the solution of very large problems.

A simple example will be demonstrated to explain the steps required, however, please note that this model is not one which requires the use of substructuring. The example involves a block of wood (E =10 GPa v =0.29) connected to a block of silicone (E = 2.5 MPa, v = 0.41) which is rigidly attached to the ground. A force will be applied to the structure as shown in the following figure. For this example, substructuring will be used for the wood block.

The use of substructuring in ANSYS is a three stage process:

  1. Generation Pass
    Generate the super-element by condensing several elements together. Select the degrees of freedom to save (master DOFs) and to discard (slave DOFs). Apply loads to the super-element

  2. Use Pass
    Create the full model including the super-element created in the generation pass. Apply remaining loads to the model. The solution will consist of the reduced solution tor the super-element and the complete solution for the non-superelements.

  3. Expansion Pass
    Expand the reduced solution to obtain the solution at all DOFs for the super-element.

Note that a this method is a bottom-up substructuring (each super-element is created separately and then assembled in the Use Pass). Top-down substructuring is also possible in ANSYS (the entire model is built, then super-element are created by selecting the appropriate elements). This method is suitable for smaller models and has the advantage that the results for multiple super-elements can be assembled in postprocessing.


  1. Give Generation Pass a Jobname Utility Menu > File > Change Jobname ...

    Enter 'GEN' for the jobname

  2. Open preprocessor menu ANSYS Main Menu > Preprocessor
    /PREP7

  3. Create geometry of the super-element Preprocessor > Modeling > Create > Areas > Rectangle > By 2 Corners
    BLC4,XCORNER,YCORNER,WIDTH,HEIGHT

    Create a rectangle with the dimensions (all units in mm):

  4. Define the Type of Element
  5. Preprocessor > Element Type > Add/Edit/Delete...

    For this problem we will use PLANE42 (2D structural solid). This element has 4 nodes, each with 2 degrees of freedom (translation along the X and Y axes).

  6. Define Element Material Properties Preprocessor > Material Props > Material Models > Structural > Linear > Elastic > Isotropic

    In the window that appears, enter the following geometric properties for wood:

    1. Young's modulus EX: 10000 (MPa)
    2. Poisson's Ratio PRXY: 0.29

  7. Define Mesh Size Preprocessor > Meshing > Size Cntrls > Manual Size > Areas > All Areas ...

    For this example we will use an element edge length of 10mm.

  8. Mesh the block Preprocessor > Meshing > Mesh > Areas > Free > click 'Pick All'
    AMESH,1

  1. Define Analysis Type
  2. Solution > Analysis Type > New Analysis > Substructuring
    ANTYPE,SUBST

  3. Select Substructuring Analysis Options
  4. It is necessary to define the substructuring analysis options

  5. Select Master Degrees of Freedom
  6. Master DOFs must be defined at the interface between the super-element and other elements in addition to points where loads/constraints are applied.

  7. Apply Loads
  8. Solution > Define Loads > Apply > Structural > Force/Moment > On Nodes

    Place a load of 5N in the x direction on the top left hand node

    The model should now appear as shown in the figure below.

  9. Save the database
  10. Utility Menu > File > Save as Jobname.db
    SAVE

    Save the database to be used again in the expansion pass

  11. Solve the System
  12. Solution > Solve > Current LS
    SOLVE

The Use Pass is where we model the entire model, including the super-elements from the Generation Pass.

  1. Clear the existing database Utility Menu > File > Clear & Start New

  2. Give Use Pass a Jobname Utility Menu > File > Change Jobname ...
    FILNAME, USE

    Enter 'USE' for the jobname

  3. Open preprocessor menu ANSYS Main Menu > Preprocessor
    /PREP7

    Now we need to bring the Super-element into the model

  4. Define the Super-element Type
  5. Preprocessor > Element Type > Add/Edit/Delete...

    Select 'Super-element' (MATRIX50)

  6. Create geometry of the non-superelement (Silicone) Preprocessor > Modeling > Create > Areas > Rectangle > By 2 Corners
    BLC4,XCORNER,YCORNER,WIDTH,HEIGHT

    Create a rectangle with the dimensions (all units in mm):

  7. Define the Non-Superelement Type
  8. Preprocessor > Element Type > Add/Edit/Delete...

    We will again use PLANE42 (2D structural solid).

  9. Define Element Material Properties Preprocessor > Material Props > Material Models > Structural > Linear > Elastic > Isotropic

    In the window that appears, enter the following geometric properties for silicone:

    1. Young's modulus EX: 2.5 (MPa)
    2. Poisson's Ratio PRXY: 0.41

  10. Define Mesh Size Preprocessor > Meshing > Size Cntrls > Manual Size > Areas > All Areas ...

    For this block we will again use an element edge length of 10mm. Note that is is imperative that the nodes of the non-superelement match up with the super-element MDOFs.

  11. Mesh the block Preprocessor > Meshing > Mesh > Areas > Free > click 'Pick All'
    AMESH,1

  12. Offset Node Numbering
  13. Since both the super-element and the non-superelement were created independently, they contain similarly numbered nodes (ie both objects will have node #1 etc.). If we bring in the super-element with similar node numbers, the nodes will overwrite existing nodes from the non-superelements. Therefore, we need to offset the super-element nodes

  14. Couple Node Pairs at Interface of Super-element and Non-Superelements

  1. Define Analysis Type
  2. Solution > New Analysis > Static
    ANTYPE,0

  3. Apply Constraints
  4. Solution > Define Loads > Apply > Structural > Displacement > On Lines

    Fix the bottom line (ie all DOF constrained)

  5. Apply super-element load vectors
  6. Save the database
  7. Utility Menu > File > Save as Jobname.db
    SAVE

    Save the database to be used again in the expansion pass

  8. Solve the System
  9. Solution > Solve > Current LS
    SOLVE

  1. Show the Displacement Contour Plot General Postproc > Plot Results > Contour Plot > Nodal Solution ... > DOF solution, Translation USUM
    PLNSOL,U,SUM,0,1

    Note that only the deformation for the non-superelements is plotted. This results agree with what was found without using substructuring (see figure below).


To obtain the solution for all elements within the super-element you will need to perform an expansion pass.

  1. Clear the existing database Utility Menu > File > Clear & Start New

  2. Change the Jobname back to Generation pass Jobname Utility Menu > File > Change Jobname ...
    FILNAME, GEN

    Enter 'GEN' for the jobname

  3. Resume Generation Pass Database Utility Menu > File > Resume Jobname.db ...
    RESUME

  1. Activate Expansion Pass
  2. Enter the Super-element name to be Expanded
  3. Enter the Super-element name to be Expanded
  4. Solve the System
  5. Solution > Solve > Current LS
    SOLVE

  1. Show the Displacement Contour Plot General Postproc > Plot Results > (-Contour Plot-) Nodal Solution ... > DOF solution, Translation USUM
    PLNSOL,U,SUM,0,1

    Note that only the deformation for the super-elements is plotted (and that the contour intervals have been modified to begin at 0). This results agree with what was found without using substructuring (see figure below).


The above example was solved using a mixture of the Graphical User Interface (or GUI) and the command language interface of ANSYS. This problem has also been solved using the ANSYS command language interface that you may want to browse. Open the .HTML version, copy and paste the code into Notepad or a similar text editor and save it to your computer. Now go to 'File > Read input from...' and select the file. A .PDF version is also available for printing.