ANSYS - Semi-monocoque shell - Step 8

Step 8: Postprocess the results

Plot Deformed Shape

The Results Viewer provides a convenient way to review results.

Main Menu > General Postproc > Results Viewer

The title bar for the Results Viewer indicates that the results are being read from the shell.rst file. Rearrange the windows slightly so that you can access the Results Viewer, ANSYS GUI and tutorial simultaneously.

Under Choose a result item, select Nodal Solution > DOF Solution > Displaced structure. Click on the Plot Results icon.

Hold down the Ctrl key and use the mouse to manipulate the model view;check that the BC's and loads have been imposed correctly. The snapshot below shows one view that is useful in checking the BC's. Are the symmetry and clamped conditions satisfied at the corresponding edges for the facesheet as well as the stiffeners? Is the model deformation as you'd expect for a uniform pressure on the facesheet in the +z direction?

The maximum displacement DMX=3.88 mm. Where do you think this occurs? We'll check this in a minute.

Animate the defromation and obsessively recheck the BC's:

Results Viewer > Animate Results > Deformed Shape > OK > Def + undef edge > OK

Select Forward Only in the Animation Controller.

Plot w Displacement

In the Results Viewer, in place of Displaced structure, choose Nodal Solution > DOF Solution > Z-Component of displacement. Click on the Plot Results icon.

The location of maximum deflection w_max is labeled MX. This occurs not at the facesheet center but on the edge x=0, at approximately y=L1/3. As expected, the deflection is zero along the clamped edges.

To save a copy of this plot, select Results Viewer > Image Capture > Capture to file > OK.

For filename, enter w_contours. This creates the file _w_contours.png_ in your working directory. Check that you can open this file using your pet image viewer.

Deflection at Facesheet Center

To query the value of the deflection at the center of the facesheet, select the Query Results icon in the Results Viewer.

Pick the node at X=0, Y=0. The coordinates of the picked node and the corresponding value of UZ (i.e. w displacement) are displayed in the Query Subgrid Results menu. The deflection at the center of the facesheet is 3.8 mm.

Cancel the Query Subgrid Results menu.

σ_xx for Facesheet

For clarity, let's first plot σ_xx for just the facesheet. Select the elements for the facesheet in two steps:

1. Select areas corresponding to the facesheet.
2. Select elements attached to these previously selected areas. Close the Results Viewer.

Utility Menu > Plot > Elements

Utility Menu > Select > Entities

Select Entities menu: Select Areas, By Location and Z coordinates. Under Min,Max, enter 0. Make sure From Full is selected. Click Apply.

Following this, select Elements, Attached to, Areas and From Full. Click Apply and then Replot. You should see that only elements for the facesheet are currently selected.

Main Menu > General Postproc > Results Viewer > Nodal Solution > Stress > X-Component of stress

Click Plot Results icon.

Shell theory provides the stresses through the thickness of the shell. This is illustrated in the help page for SHELL93 element. If, like me, you are looking at the top of the facesheet, then the contours values correspond to σ_xx values for the top face. Check the σ_xx value for the top face at the facesheet center:

Results Viewer > Query Results

Pick the node at X=0, Y=0. I get σ_xx=51 MPa at the center-top of the facesheet.

Hold down the Ctrl key and flip the model over so that you are looking at the bottom of the facesheet as in the snapshot below. Now the contours values correspond to σ_xx values for the facesheet bottom. Use Query Results to determine σ_xx at the center-bottom of the facesheet. I get -56 MPa. What do you get? The negative sign indicates compression.

(For an enlarged view, click and maximize the browser window)

Thus, at the facesheet center, σ_xx varies from a tensile stress of 51 MPa at the top to a compressive stress of 56 MPa at the bottom.

Using Query Results, I get σ_xx=116 MPa at the edge point x=W1, y=0 for the bottom of the facesheet (see snapshot above). What's the value you finagled out of ANSYS?

Do these values look plausible? We'll investigate this in Step 9 when we compare the center and edge stress values to plate theory.

Cancel the Query Subgrid Results menu.

σ_yy for Facesheet

Results Viewer > Nodal Solution > Stress > Y-Component of stress

Click Plot Results icon. The snapshot below shows the σ_yy contours.

Using Query Results, I get the following values for the bottom of the facesheet (see snapshot above):

1. At the center, σ_yy= -28 MPa.
2. At the clamped edge location (x=0, y=L1), σ_yy= 77 MPa. What are your corresponding values?

σ_xx for Stiffeners

Currently, the facesheet is selected and the stiffeners are unselected. To plot stress contours for the stiffeners, we'll unselect the facesheet and select the stiffeners i.e. reverse the selection. This can be done using the Invert operation:

Select Entities menu> Invert

Select Entities menu> Replot

(In MS-Windows, you can cycle through windows on the desktop by holding down the Alt key and repeatedly pressing the Tab key. In case the Select Entities menu has disappeared, exit the Results Viewer, bring up the Select Entities menu and re-enter the Results Viewer.)

Results Viewer > Nodal Solution > Stress > X-Component of stress

Click Plot Results icon.

Manipulate the view so that you are looking down on the top of the stiffeners as in the snapshot below. You might have to flip the model over.

The σ_xx values for the stiffeners in the y-direction is virtually zero; confirm this using Query Results. This means that, as expected, the load in the x-direction is carried by the stiffeners in that direction.

Let's determine σ_xx values at the top of the x-stiffener closest to the center; we'll compare these values to plate theory in Step 9. Using Query Results, I get the following values at the top of this stiffener (see snapshot above):

1. At (x=0, y=L₁/6), σ_xx= 312 MPa.
2. At the clamped edge location (x=W₁, y=L₁/6), σ_xx= -653 MPa. What are your corresponding values?

σ_yy for Stiffeners

Results Viewer > Nodal Solution > Stress > Y-Component of stress

Click Plot Results icon.

The σ_yy values for the stiffeners in the x-direction is virtually zero; confirm this using Query Results. This means that, as expected, the load in the y-direction is carried by the stiffeners in that direction.

Let's determine σ_yy values at the top of the y-stiffener closest to the center which we'll compare to plate theory in Step 9. Using Query Results, I get the following values at the top of the stiffener (see snapshot above):

1. At (x=W₁/4, y=0), σ_yy= 38 MPa.
2. At the clamped edge location (x=W₁/4, y=L₁), σ_yy= -300 MPa. What are your corresponding values?

Save: Toolbar > SAVE_DB

Go to Step 9:Validate the Results

See and rate the complete Learning Module

Go to all ANSYS Learning Modules