Creating a User Defined Result Showing Tabular Loads with Multiple Variables in Ansys Mechanical

User defined results are a powerful tool. You can even use them to look at applied loads. We recently received a tech support call that was related to a post that Alex Grishin did on the blog, Using External Data in ANSYS Mechanical to Tabular Loads with Multiple Variables, Part 2. The question was, how do you view the tabular loads you applied. Doug Oatis created the following response to the question, showing how to use a user defined result, and we felt it was certainly blog worth.

Creating a User Defined Result Showing Applied Tabular Loads

First question…how to look at the actual values that were applied using tabular loads via command snippet.

I took Alex’s article and commands the user provided and created an example model (mainly making sure the x/y dimensions were correct and the time value was the same as defined via APDL). 

I created a single convection load on a face, specified that both convection and temperature were time-varying (need to do this otherwise the loading won’t have the appropriate _convvari and _loadvari tables defined):

I pulled the ID from the load object details window and replaced that ID for the ID used in the article:

And that all worked.  Now, to answer the question “how do you view the mapped values?” The way we do that is to get the actual values to display *after* solving. 

Let’s walk through the long way…

Click on the ‘solution’ branch, then go to the worksheet view, toggle the button to ‘material and element type information’, and then it’ll show you a list of all the different element types in the model.  ANSYS handles convection loads through SURF152 elements (it’s essentially a skin paved over the solid elements).  You’ll get one TYPE for each convection load, so if you have a lot of different convection loads realize that they’re all applied through SURF152s but they will have different TYPE numbers (see the option for ‘collapse consecutive IDs’ to break them out into individual lines).  If you’re trying to figure out which element is where, you can always right-mouse click, go to plot items, then switch to the geometry tab:

Which gives:

Now we know that SURF152s are in the model, that’s how the convection is defined, so how to get more information out of the SURF152s… We need to look up the SURF152 in the user manual.

If we look in the element table output for those elements we’ll see:

Going into the actual specific table definitions:

We see that HFILM is stored in the NMISC,5 table while the temperature is stored in NMISC,7

So we can put all that information together to create a user defined result in Ansys Mechanical:

Now this example works if I only have a single convection load applied, as I’m telling the solver to show me the output for ALL SURF152s.  If I wanted a specific type (as defined in the solution > worksheet view) you could toggle the scoping method for the user defined results to be by element TYPE rather than NAME:

Tech Support and Training for Users by Users

This is a slightly modified version of the type of response you can expect from PADT if you are one of our Ansys customers. Our deep product knowledge and understanding of how users run theses tools lets us create simple, to the point and effective tech support responses. It makes a difference and it is why so many companies choose PADT as their Ansys support provider. You get the same level of expertise if you leverage our team for training, mentoring, or consulting. Reach out, we would enjoy talking to you about how we can help you get the most out of your Ansys software investment.