Node Interaction in Mechanical, Part 4: Scoping Results to Nodes

This article is the eagerly awaited fourth and final installment in my series on interacting with nodes in ANSYS Mechanical. To review, the previous three articles covered picking your nodes, creating named selections from nodes, and applying boundary conditions to nodes.  I know some of you were wondering why it took a while for this final article to come out. Well, I’d been sent to my home state of Indiana for business and decided to take a few extra days to visit relatives—living and not-so-living.

photo

Great-great-great-great-great grandpa!

Now on to business. Our discussions so far have centered on preprocessing and solution processing operations with nodes. Now we’ll conclude the series by covering postprocessing operations with nodes in Mechanical. Much the same way that you can scope boundary conditions to nodes, you can also scope results to nodes. There is one key difference however: whereas nodal boundary conditions can only be scoped to named selections, nodal results can be scope to geometry or named selections.

Scoping results to nodes based on geometry selection is accomplished using the same procedure as scoping results to any other geometry: simply select the nodes of interest, and insert results.

image

image

Likewise, for named selections, simply insert the results object of interest, set the Scoping Method to Named Selection and choose the appropriate named selection.

image

image

Does something appear a bit unusual about that last figure? Notice that the results are plotted as continuous contours, with the nodes emphasized, rather than just appearing as discrete points. When all of the nodes on an element are selected, such as in this example, the results are displayed as a continuous contour across the face. Here’s an example showing what happens when some element faces have all their nodes selected, and others have only a few.

image

image

Beyond the standard analysis results, you can perform some additional nodal orientation verification as well. Remember how in the third article in this series I sent the Mechanical modal over to Mechanical APDL and turned on the nodal coordinate systems there to verify their orientations? Now you do, because I linked you to it. Well, as it turns out, you can get the same information in Mechanical. Let’s see how.

As an example we’ll start with the same valve with a cylindrical coordinate coordinate system located at the center of the outlet flange. The nodes on the outlet flange face (Named Selection: Outlet Flange Nodes) have been rotated into this cylindrical coordinate system and a 0.01” displacement applied to them in the Y (theta) direction. The inlet flange is fixed.

image

After solving the model, highlight the Solution branch and click on the Coordinate Systems pulldown, way on over to the right of the Solution toolbar, next to the Command Snippet button.

image

Using this pulldown menu, you can display nodal coordinate triads and nodal rotation angles. The Nodal Triads pick displays the nodal coordinate systems, equivalent to executing /PSYMB,NDIR,1 in Mechanical APDL.

image

The Nodal Euler Angles display the amount of nodal rotation in each plane from the original position. Here’s a plot of the Nodal Euler XY Angles of the outlet flange nodes.

image

Wait a second. Don’t those contours seem a little “off” to you? They’re not lined up radially, and the zero and 180 degree rotation values aren’t quite located where I expect them to be. Wait, I think I know what the problem is. Let’s set the displacement scaling to 0.0 (Undeformed) and see what happens.

image

There, that’s better.

Note that you can also display element triads and Euler angles, for rotated element coordinate systems, but that’s a topic for another day.

This completes the nodal interaction series for R14.0 ANSYS Mechanical. We will be sure to keep you informed of further improvements to finite element interaction capabilities in Mechanical as future versions are released.