As I noted in my series on nodal interactions in Mechanical, ANSYS has been exposing more capabilities to interact with the underlying finite element model over the past couple of versions. Additionally, Mechanical’s visual verification capabilities have improved as well, as it is now possible to view nodal connectors created by remote forces and displacements, weak springs, and MPC contact.
To demonstrate this, I’ve modeled a ball valve as shown below.
The model is set up with the following options and boundary conditions. (Don’t try to make real-life sense of these; I’m just demonstrating capabilities here.)
- Weak springs are turned On under Analysis Settings.
- The bonded contact between the handle and shaft is set to MPC behavior (the bonded contact between between the valve body and ball is kept as Program Controlled).
- A 50 lb remote load is applied just off the end of the handle and scoped to the end face of the handle (B in the figure above).
- A 5 degree Z-rotation is applied as a remote displacement and scoped to the front face of the valve body (C in the figure above).
Now, you won’t be able to view the “spider webs,” “bicycle spokes,” etc. generated by the nodal connections yet. The weak springs, MPCs, and beams are not created until the matrices are assembled. So, at this point you will want to solve the model.
When the solution is complete, highlight the Solution Information folder in the Model tree. You will see two tabs at the bottom of the graphics window: Graphics and Worksheet. Click on the Graphics tab.
You will now see all the nodal connections displayed for your finite element edification, and they are glorious. Note: Constraint equations (CEs) include multi-points constraints (MPCs).
Click the Show Mesh button for the full finite element display.
The “clumping” of the MPCs on the front face of the valve body might look a little odd, and it is—you’re not imagining it—but it deflects the way I expect it to, so I’m good with it.
Now right about now, you’re yelling at me through your monitor and I can hear what you’re saying. “Hey, Strain, I don’t have the luxury of working with these little Mickey Mouse sample models that you create for sales demos or training courses or Focus articles! The models I make are real-life models that take hours or days to solve. Do you really expect me to wait for hours or days before I can verify that my connectors are correct?” Fret not, dear ANSYS user; there is a simple workaround to this. When the Solution Status says “Solving the mathematical model,” simply click [Stop Solution] and continue to display the connectors as described above. Maybe give it a minute or two first, though, just to make sure the matrices have been assembled and the connectors generated.
The default is that you see everything, displayed as lines, but if you take a look at the Solution Information details, you’ll see that you have some additional display options under FE Connection Visibility.
By default, we see All FE Connectors, but we can switch the Display option to CE Based, Beam Based, or Weak Springs. (We can also change it to None, but that would defeat the purpose of this article.) Here is the same model with Display set to Weak Springs.
By default, the connections for all nodes are displayed, but you can isolate the display to a nodal named selection under the Draw Connections Attached To option. For example, here is the connector display for the front valve body face nodes, named “front face nodes.” (Note: I’ve turned all FE connectors back on.)
Finally, if you want a bit more visual clarity, you can change the Display Type to Points instead of Lines.
This is another example of direct finite element interaction being enabled in Mechanical. With this capability, the user will no longer need to export the model to Mechanical APDL for visual node connector verification. Expect even further finite element interaction capability in future versions; ANSYS is on a roll in this area.