Comsol Tutorial 1 – A simply supported
beam modeled in 3D
In this tutorial you will create a fully 3-dimensional beam model using Comsol’s drawing tools. You may
also import 3-D modeling files from Solidworks (IGES) .igs files.. For the projects of this course you may
use either Comsol or Solidworks to create the geometries, however you should use Comsol for
generating the mesh and you must use Comsol for the analyses.
Start Comsol 3.5a and open a New model > Comsol MultiPhysics > Structural Mechanics > Solid Stress
Strain > Static Analysis. Notice the dependent variables are now u, v, and w. A 3D drawing grid will
appear. Under Options, Preferences, Modeling, set the Default Unit System to IPS (inch Pound, Second).
In the left-hand drawing tool bar select the Block tool. Set the Corner Base-Point at 0,0,0 and the length
to 4.0, 0.75 , and 0.75. This creates a solid square beam. Create a second square beam with Base-Point
at 0,.75/4, .75/4. and length 4,.75/2, .75/2. In the graphics window, select both blocks then select the
Difference icon from the left-hand drawing window. This should create a hollow box beam with wall
The beam is still prismatic. Modify it by cutting holes along its length. Select the Cylinder tool from the
drawing bar. Choose R=.75/4, H=.75, and set the Axis Base Point to .5, 0, .75/2. Also set the Axis
Direction Vector to 0,1,0. Hit the XZ-Plane icon from the drawing tool bar for a better view. Next make
sure the cylinder is still selected then select the Array tool from the drawing toolbar. Set the
displacement to 1,0,0 and the Array Size to 4,1,1. This creates four pretty big cylinders. Using Edit>Select
All from the pull down, highlight everything, then select the Difference icon to cut holes in the beam.
Return to the isometric view.
Finally, we need to create a place to apply our load. Choose the Block icon and place a box at 2-
1/16,0,.75 with lengths 1/8,.75,.1.
Next set the boundary conditions. Under Physics>Subdomain set the material properties to Structural
Steel (you may need to Load the property library). Select Physics>Boundary Settings and highlight the
top of the loading section (boundary # 33) and apply 1000 psi downward. Next choose Physics>Edge
Settings (new to 3D) and set edge #2 to a Constraint of Rx=0, Rz=0 and hit Apply. Select edge # 144 and
set Rz=0; hit Apply. These edges are the contacts with the supports.
This recreates a pin condition on the left and roller on the right but leaves the y-direction free which is
not good. An unrestrained direction allows a Free Body Mode (i.e. translation). Correct this by
choosing points #1 and #81 and setting Ry=0 for both. Hit OK. This allows the beam to naturally contract
due to the Poisson effect in the y-direction on the boundary.
Choose the Equals Sign (Solve) from the top menu and go to Postprocessing. Under General select
Subdomain and Deformed Shape. Turn off Slice. Choose the Subdomain tab and examine the Sxx and
von Mises Stresses.
Next select Postprocessing and Boundary Integration . From the Predefined pulldown select Face Load in
Global z. Hit Apply and look for the “Value of Integral” in the information box at the bottom of the
window. Remember that we put 1000psi on 1/8 in. x 3/4in. which yields 93.75 pounds as expected.
Finally, from Postprocessing>Subdomain select the Max/Min tab. Turn the Marker On and select z-
displacement from the pulldown. Note that since there are no free points at the center line, there was
no way to select a point for the max/min as down in the 2D model.