Understanding the Difference Between Maximum Von Mises Stress and XY Plot Values

[yjun9911TMAVC]

Hello, I am currently trying to simulate a nonlinear static analysis of ABS plastic using Inventor Nastran. The solution was successful. However, as you can see in the images, the maximum von Mises stress is shown in various colors (33.69 MPa), but in the XY plot, it is only about 20 MPa. Why are these two values different? When I derived the results for the XY plot, I grouped the entire drawing elements together. Thank you.

[John_Holtz]

Hi @yjun9911TMAVC 

• The XY Plot uses the stress from the centroid of the chosen element. 
• The contour plot shows the stress from the corner of the elements by default. Since those are two different locations, there are two different results shown by the XY Plot and the contour plot.
• To get a similar display, you can edit the contour plot (from the ribbon, "Results > Options") and set "Data Type" to "Centroid", "Contour Type" to "Elemental", and check "No Averaging". See this article for more details. 
  How to Understand XY Plot of Element Along Selected Entity in Inventor Nastran (Not entirely related to your question, but the article does provide information about the stress plot in general and links to more details.)

Let us know if you have any questions.

John

[yjun9911TMAVC]

Thank you , John. However, is it not possible to show the stress at the corners in the XY plot?

I have more confidence in the contour plot and would like to compare it with the XY plot.

[yjun9911TMAVC]

Thank you , John. However, is it not possible to show the stress at the corners in the XY plot?

I have more confidence in the contour plot and would like to compare it with the XY plot.

[John_Holtz · Accepted solution]

Hi @yjun9911TMAVC 

Without making some changes to the model, the XY Plot will not graph the stress at a node. You can try a test model to see if this works. (Or re-run the real model if it does not take too long.)

1. Edit the Parameters. (Second to last branch in the Model Tree).
2. Search for GPSTRESS using the text box in the lower left corner. (This stands for grid point stress. It will output the averaged stress at the nodes.)
3. Set GPSTRESS to be on.
4. Run the analysis.
5. If I remember correctly, Inventor does not display the grid point stress result. But you may be able to graph it in the XY Plot.

Note that there will still be a difference shown in the XY Plot versus what Inventor shows! The difference is due to the method of calculating the results:

• The non-grid point stress results are an average of the result from each corner of each element attached to the node. If three elements are connected to a node, three von Mises results are averaged to determine the value for the contour plot. For example, the average von Mises stress (vM) shown in the contour plot = (vM1 + vM2 + vM3)/3. Each of the three von Mises stress values are calculated from the corresponding stress tensor values (X-Normal through ZX-Shear).
• For grid point stress results, the six stress tensor results are averaged first. For example, the X-Normal result X = (X1 + X2 + X3)/3, and likewise for Y-Normal, Z-Normal, XY-Shear, YZ-Shear, and ZX-Shear. The invariant stress results are then calculated from the averaged stress tensors. For von Mises, vM = Square Root[ {(X-Y)^2 + (Y-Z)^2 + (Z-X)^2 + 6*(XY^2 + YZ^2 + ZX^2)} /2} ].
• This difference between the two methods, average of the invariant stress or average of the stress tensors and then calculate the invariant stress, leads to the differences in the two sets. For a proper mesh, the difference should be small.

John

[yjun9911TMAVC]

Thank you for the detailed response, John. I solved this problem.

However, I am encountering a new problem.

I am conducting nonlinear compression analysis right now. I want to obtain stress-strain data for the entire object rather than specific points(elemet). So, I grouped the meshed object in the group items within the model tree. However, as shown in the attached picture, only the data results for elements 1 through 10 came out. I want to get data for the entire object (stress, strain) rather than specific points. What should I do?

[John_Holtz]

Hi @yjun9911TMAVC 

If I understand correctly, you want to create a graph with 1946 curves on it? What use would that be? (I am not sure if "the entire object" means all 1946 elements or just a portion of the entire model.)

The XY Plot is limited to 10 items. (Probably because trying to plot more than that just creates a mess.) You either need to create multiple plots, 10 items at a time, or use a third-party tool to extract the data to a text file. See tip 56 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks on the Inventor Nastran forum.

John