Home / Simulate / CAD-based FEA Tutorial, Part 2

CAD-based FEA Tutorial, Part 2

By Dimitrios Karamanlidis

Editor’s note: In his April 2012 article, the author provided an overview of the process described in step-by-step detail below. Please see that article here.

SpaceClaim 1: We start out with a thin-walled part created by another modeler and imported into SpaceClaim. For the sake of simplicity we assume that all undesired rounds, holes and cut-outs have already been removed, leaving us with the part shown below


SpaceClaim 2: Switch from Design to Prepare, click on Midsurfaces and select the box as shown below


SpaceClaim 3: With Midsurfaces still active, click on the Add/Remove Faces tool and add the three pipes to the selection. If what you see on your screen looks similar to the Figure below (left) click on the Complete tool to finalize the midsurface extraction. The result should look similar to the Figure below (right)

SpaceClaim SpaceClaim

SpaceClaim 4: Delete all 3D solids, that is, if you check the Structure tree, it should indicate that the part consists of four surfaces only, viz.


SpaceClaim 5: Export the part to a neutral geometry file, say IGES.

ANSYS 1: Now we are off to ANSYS. First, we import the geometry using the sequence

File > Import > IGES


ANSYS 2: Check to see if your model contains any volumes and if it does, just delete them using the sequence

Preprocessor > Modeling > Delete > Volumes Only

ANSYS 3: To make sure that the model has no gaps nor overlaps use the sequences

Preprocessor > Modeling > Operate > Boolean > Glue > Lines > Pick All

Preprocessor > Modeling > Operate > Boolean > Glue > Areas > Pick All

Preprocessor > Modeling > Operate > Boolean > Overlap > Lines > Pick All

Preprocessor > Modeling > Operate > Boolean > Overlap > Areas > Pick All

ANSYS 4: Choose a thin shell element from the library using the sequence

Preprocessor > Element Type > Add/Edit/Delete > Add > Shell > Elastic 4node 63

ANSYS 5: Define the shell element “real constants” using the sequence

Preprocessor > Real Constants > Add/Edit/Delete > Add > OK

That brings up the real constants window


In the simplest case scenario (shell with constant thickness) only one value need be entered in the first box. If the thicknesses of the box and the pipes are not all the same then we need to define more than one set and assign each one to the respective portion of the mesh.

ANSYS 6: Define the material properties using the sequence

Preprocessor > Material Props > Material Models

which will bring up a window titled Define Material Model Behavior


Expand the Favorites folder and click on Linear Isotropic to bring up the window


where the numerical values for the modulus of elasticity (EX) and Poisson’s ratio (PRXY) may be entered. We assumed the material to be structural steel and entered for EX=30000 (ksi), and for PRXY=0.3.

ANSYS 7: Use the sequence

Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > Picked Lines

in order to define size controls for the mesh generation (we used ten divisions per line) and then proceed to create the mesh using the sequence

Preprocessor > Meshing > Mesh > Areas > Pick All

The result is shown in the figure below.


Note that certain symmetries of the part geometry have not been preserved in the mesh which, in turn, may adversely affect the accuracy of the results obtained by the analysis.

A better mesh is obtained by splitting all faces in question into three- or four-sided regions. While it is outside the scope of this tutorial to get into too much detail about meshing it seems appropriate to briefly note the difference between a free and a mapped mesh. A free mesh may be applied to any region of arbitrary shape as shown in the figures below.


Whereas a mapped mesh may be applied only to three- or four-sided regions, viz.


Going now back to our thin-walled part, the splitting of the surfaces may be done either in ANSYS or in SpaceClaim. Personally, in terms of manipulating geometry I find the latter considerably easier to work with than the former.


The figures above show, respectively, the model exported from SpaceClaim (left) and the model imported into ANSYS (right). The obtained mesh in this case is shown in the figure below.


As a second example consider now the thin-walled part shown in the figure below


Proceeding as before, we extract all midsurfaces which leaves us with the solid shown below


Noticing that the fins are a) too long and b) not connected with the cone we take care of both issues in SpaceClaim using the Pool tool. The resulting surface solid along with its structure tree is shown below.


Importing the geometry into ANSYS and creating a mesh of SHELL63 elements leads to


Upon closer examination we realize that the above created mesh is basically useless due to improper connections between elements. The reason for that is that the entire cone is represented as a single surface. Hence, we go back to SpaceClaim and subdivide the cone accordingly


Depending on the kind of analysis we intend to perform it may be necessary/sufficient to use a coarse mesh,


a locally refined mesh,


or a fine mesh


About DE Editors

DE's editors contribute news and new product announcements to Digital Engineering. Press releases can be sent to them via DE-Editors@digitaleng.news.