Stress Probe; location of Vertex

  • Last Post 12 October 2018
jonsys posted this 08 October 2018

Hello Community,

I want to get the stress results over time at the Vertex shown in the picture, therefore I used a Stress Probe. I want the stress results of the lower layer, but I get the results from the middle layer.

How can I select which of the layers I want the stress output from?



Order By: Standard | Newest | Votes
peteroznewman posted this 08 October 2018

Hello Jon,

The following plots are made with 0 deformation so I don't lose track of which element is being plotted.
Below is the Normal Stress in the 3 layer sandwich where I have a very coarse mesh.

I created two named selections, but I picked the fourth element back from the end to get a larger difference.

I will be interested to read other member's posts.


  • Liked by
  • jonsys
SandeepMedikonda posted this 08 October 2018

Is there contact between the 2 parts?

If yes, you have 2 nodes sharing the same space and it would just display the values from one of the nodes.

Now, if you are just dealing with node sharing or generally in FEA and I hope I am understanding the question clearly, Nodal Value Stresses in Gauss points are extrapolated to element nodes. Most often, one node is shared by several elements, and each element reports different stresses at the shared node. Reported values from all adjacent elements are then averaged to obtain a single value. This method of stress averaging produces averaged (or nodal) stress results. Element values Alternately, the stress values from all Gaussian points within each element can be averaged to report a single elemental stress. Although these stresses are averaged between Gauss points, they are called non-averaged stresses (or element stresses) because the averaging is done internally within the same element only. Maybe the below picture will help understand this better:

This is often a question that FEA engineers struggle while using FEA whether to use nodal or elemental values and there is no correct answer here and is subjective.

Best Practices to post on the Student Community

  • Liked by
  • jonsys
jonsys posted this 11 October 2018

Hello peter,

thank you. That is a very good alternative way and would do the work if nobody else suggests something for the exact location stress output.


jonsys posted this 11 October 2018

Hello Sandeep,

that is a very interesting thing that you shared.

In the case I mentioned in the question, there is no contact defined between two bodies, they are under the same part.

In a previous question answered by you, I was trying to implement a path from which I would get the stress output throughout the path at a specific time. In this one, I want to get the stress-time graph (values) at a vertex. The problem at the output from the vertex shown in the first picture, is the one you mentioned 

Mechanical calculates the results from the body with the highest identifier (typically the latest one in the geometry tree).

Now together with the initial question, I am curious to know something regarding the figures you posted:

  • If request the stress output at the node shared by 4 elements, I would get the stress of the body with the highest identifier (let's suppose 3); how do I request to get the averaged value (i.e. 3.5)?


SandeepMedikonda posted this 11 October 2018


  That case was for the Construction Path, if I remember it correctly?

  Here I am talking about generic FEA approach. In a scenario such as yours, using stress probes will always either give you the max. or the min of the values extrapolated from the 2 elements connecting to that body. For simplicity, let's say that this node is being shared by only 2 elements and assume that they have different materials.

when your node is being shared by different parts and you want the average of those 2. Note that you can't scope to a vertex, but only to nodes. Then, I think something like this should help:

Basically, what you are just seeing here is the average values displayed in the first picture of my post. 

Hope this helps.


  • Liked by
  • jonsys
jonsys posted this 12 October 2018

thank you for the clear answer Sandeep