SUMMARY
Certain element types have been hidden in the Mechanical interface to keep it cleaner, more user-friendly, and streamlined. This design choice helps users focus on physics-oriented simulations, emphasizing core project aspects like analyzing physical behaviors and phenomena. It prevents them from getting overwhelmed by the complexities of finite element procedures. Consequently, the interface is less cluttered and more intuitive, promoting a smoother and more efficient workflow for engineers.
Certain users require access to these element results for specific purposes such as validation or enhanced model comprehension. Therefore, this entry will explore the method to access hidden elements in Ansys Mechanical for post-processing purposes. This will involve creating an APDL snippet to select the relevant elements, with results extraction conducted using interface objects.
Process steps
As usual, an example is the best way to explain these concepts. But before that, let's list the two main steps of this process:
Example
One of the most common cases is during the use of beam connectors. Consider a model where you have created several connectors to simulate bolts and you want to extract results. Even if you can use tools to create bolt results automatically, they will be scoped just to one object. Or if you use User results you'll need to scope all of them.
Imagine now an intermediate scenario where you want to group the results somehow, say the upper line in one set and the lower line in a second one. This is the logic you need to include into the APDL snippet.
APDL Snippet
For this example the logic is simple, just selecting beam elements and then filter this selection by coordinates to separate the two line sets. After that, create a Component. Never forget to select everything again to solve the model correctly. This object must be included in the Analysis branch (Static Structural) because this location will allow the snippet to capture the full created mesh overcoming the limitation of creating a Named Selection directly.
The first ESEL command selects all the BEAM188 elements, and the second ESEL filters this initial selection using the centroid X coordinate keeping selected the elements located between 0 and 40 length units (mm). Then the CM command creates the new Component assigning the name 'UPPER_CONN', this the key name to be used later. Finally the ALLSEL command will select everything again to continue the solving.
Once the model is solved in the usual way, you can find the created Component 'UPPER_CONN' in Solution-> Worksheet->Solver Component Names.
If you want to plot them, just right click on it and 'Plot Item(s)'
Post-processing
To evaluate results you need to use a scoping based on 'Result File Item' and then choose 'Component Name', the component name need to be typed in the following field. This example shows a User Defined Result with the BEAM_BENDING_MY expression to evaluate bending moments.
Finally the desired post-processing contour is achieved:
Conclusions
You have the flexibility to develop highly intricate selection logic, which underscores the true strength of this methodology. This approach effectively eliminates the limitations associated with interface-based selection, allowing for a more tailored and precise analysis. By leveraging this advanced selection logic, users can isolate specific elements or groups of elements based on a variety of criteria such as geometric location, material properties, or loading conditions. This level of customization ensures that the results are not only accurate but also highly relevant to the specific engineering problem at hand. Consequently, engineers can achieve a deeper understanding of the physical behaviors and phenomena within their models, leading to more informed decision-making and optimized design solutions.