Print this page

A Guideline to Submodeling in ANSYS

Submodeling is a finite element technique that allow users to obtain more accurate stress and strain results in a particular region of a model which is a small area of concern in comparison to whole model.

 

In too complex structures that fine mesh is required to produce good accuracy, submodeling approach will be useful to let users to utilize coarse elements in base models and solve it with less solution time that follows with employing fine mesh in a particular area of interest to get better stress distribution.

A finite element mesh may be too coarse to produce satisfactory results in a given region of interest. The results away from this region, however, may be satisfactory. In joint analysis specifically weld connections, it has more advantage to model welds with shell elements and then obtain accurate stress results from submodels.

The approach is very simple:

1.       Create the base or coarse model.

2.       Analyze the base or coarse model. (Use different jobname for coarse model and submodel)

3.       Create the submodel. (Only shell and solid elements are supported for submodeling)

4.       Perform cut-boundary interpolation. (It only projects master node displacements to slave nodes)

5.       Analyze the submodel.

6.       Verify that the distance between the cut boundaries and the stress concentration is adequate.

 

 

Here is an example for employing submodeling approach :

! Start with coarse model analysis:

/FILNAME,my_coarse

/PREP7

...

/SOLU

ANTYPE,...

...

SOLVE

SAVE

 

! Jobname = my_coarse

! Enter Preprocessor

! Generate coarse model

! Enter SOLUTION to solve coarse model

! Define analysis type and analysis options

! Define any loads and load step options

! Coarse model solution, Results are written on file coarse.rst

! Coarse model database file my_coarse.db

 

! Create submodel:

/CLEAR

/FILNAME,my_submod

/PREP7

...

 

! Clear the database (or exit program and re-enter)

! New jobname = my_submod

! Re-enter Preprocessor to generate fine mesh

! Generate submodel with fine and detail mesh

! Perform cut-boundary interpolation:

NSEL,... 

NWRITE

ALLSEL

SAVE

RESUME,my_coarse,db

/POST1

FILE,my_coarse,rst

SET,...

CBDOF

 

RESUME

/SOLU

ANTYPE,...

/INPUT,my_submod,cbdo

... 

SOLVE 

 

! Select nodes on cut boundaries

! Write those nodes to my_submod.node

! Restore full sets of all entities

! Save submodel database file my_submod.db

! Resume coarse model database (my_coarse.db)

! Enter Post processor

! Use coarse model results file

! Read in desired results data

! Reads cut-boundary nodes from my_submod.node

! and writes D commands to my_submod.cbdo

! Resume submodel database (my_submod.db)

! Enter SOLUTION

! Define analysis type and options

! Cut-boundary DOF specifications

! Define loads and load step options

! Submodel solution

/POST1

...

FINISH

! Enter Post processor

! Verify submodel results

! FINISH

Last modified on 10/09/2015

Share this article

Login to post comments