This is the second entry in a thrilling saga about interacting with nodes in ANSYS Mechanical. In Part 1, I addressed the various methods for picking and querying nodes in a Mechanical model. In this entry, I discuss various methods for creating nodal Named Selections. Creating nodal Named Selections is a key step in executing the processes I’ll address in my next two entries: Applying nodal boundary conditions and scoping results to nodes.
I’ll start with the easy stuff. To create a Named Selection from picked nodes, simply pick the nodes you’re interested in as described in Part 1, right-click, and select Create Named Selection (or, in the Named Selection toolbar, click the Create Named Selection) and give it a name.
Note that the “Apply geometry items of same:” option does not work with nodes yet. However, there is another option: The Worksheet. The worksheet will allow you to define nodes based on location, node number, and attachment to solid model entities.
To activate the Worksheet mode, highlight the Named Selection branch (add it from the Model toolbar if necessary) and insert a new Named Selection. In the details window, change the Scoping Method from Geometry Selection to Worksheet.
The Selection worksheet appears.
To begin the selection process, right click on the first row and select Add Row.
The Add action is similar to selecting “from full” or “also select” in Mechanical APDL and is most likely the first action you will take in the selection process. Select Mesh Node from the pull-down menu under Entity Type.
For the criterion, select either Location X, Y, or Z or Node ID (node number).
Then select the appropriate Operator from the pull-down menu. Available options for both Location and Node ID are Equal, Not Equal, Less Than, Less Than or Equal, Greater Than, Greater Than or Equal, and Range. Options for Location additionally include Smallest and Largest.
Next, fill in the Value, Lower Bound, and/or Upper bound as appropriate. Also select the appropriate coordinate system when using one of the Location criteria.
When complete, click the Generate button to execute. The Geometry entry in the details will indicate the number of selected nodes. Click on the Graphics tab to verify the selection.
If desired, add additional selection actions. The Add action at this point behaves as “also select.” Remove behaves as “unselect.” Filter acts as a “reselect” operation. In this example, we will Filter the selection to nodes between Y = 0 and Y = 2.5 inches. (I also could’ve simply done Y > 0, but I wanted to show the Range Operator here.)
At this point, you’ve probably noticed that the Named Selection is named “Selection.” Simply rename it by right clicking on the Selection object and selecting Rename.
So now you know how to create nodal Named Selections based on location and node number, but how do you create a named selection from nodes attached to a face or some other solid model entity. That’s a little more complicated, but I’m here to take you through it. It’s not really difficult once you know the steps.
First, create a Named Selection from the geometric entities containing the nodes you want to select.
Then create a new Named Selection with the Worksheet scoping method. In the first row set Add as the Action. Set the entity type equal to the entity type the Named Selection was created from in the previous step. Set the Criterion to Named Selection and the Operator to Equal. Select the Named Selection created in the previous step from the pull-down menu under Value.
“Criminy, Strain! We’re just selecting the same Named Selection that we create in the previous step! What’s the point?! You’re wasting my time!” Read on; there’s another step here.
Add another row to the Worksheet. Set the Action to Convert to and the Entity Type to Mesh Node. Then click Generate and verify the selection in the graphics window. There, don’t you feel silly for getting so upset in the previous paragraph?
In these first couple of parts, we’ve spent a lot of time learning how to simply select the nodes. Now wouldn’t it be nice to actually do something with them? In the next two parts, we’ll do exactly that. First, we’ll see how to apply loads and constraints directly to nodes, and rotate them into different coordinate systems. For the last installment, we’ll discuss how to scope results to nodes.