Query stress in a node?

[Senad83]

How may I find the stress acting in one single node? If I for example want to know the stress S11 in node 14?

 

[xerf]

CAE -> Visualization->Tools Menu->Query->Select Probe Values->Apply
Then in the dialog window:
Probe: Select Nodes
Check "Key-in labels"
Select Part instance
Input node label....

 

[louisa]

How shall we probe the stress and strain tensor for an element and for the whole model? I am desperate to know this question My advisor wants these tensors.

I read this sentence in one paper: ":average stress and strain tensors are computed over all of the elements:" I wrote to the authors but they wouldn't tell me how they did it.

A stupid way may be to get the stress at the node, use interpolation function and then integrate over the volume. But I guess there should be an easy way to get average stress and strain tensors from Abaqus output.

I directly run the python code in the Abaqus Command Window. So I cannot request writing to the result file which is only available to Input File Usage. The result file should be able to compute the stress and strain tensor pretty easily, I guess.

 

[Senad83]

I`ve tried this, but I get wrong values in nodes.

 

[xerf]

louisa,
Are you interested in average stress and strain tensor for computing effective properties maybe?

You do not need to extrapolate the stress and strain at nodes. Use the suitable Gauss quadrature rule for the element type you are using to integrate each stress and strain component over each element in the domain.
then the average over entire model is:

<Sij(whole_model)> = (1/Volume)*Sum(I(Sij(elem_i)), i=1...Nelem

where I(Sij(elem_i)) means the integral of Sij over element i, i=1..Nelem

Personally, I could not find a direct way so I had to write my own code.

 

[louisa]

ah- xerf, you are brilliant! Yes, I want to calculate effective properties of composites.

You are right. Use Gauss integration weights significantly simplifies the problem. I have another question: for each element, I should divide the integrated value by the real volume of the element in x,y coordinate, or by the volume of 2x2=4 in r,s coordinate?

 

[xerf]

You should use Gauss quadrature to integrate each stress and strain component over each element. Therefore you will have one value per stress/strain component/per element. The you sum all these values (separately for each component) and in the end you will have one value for each stress/strain component per entire model.

The divide each of these values by the model volume.

To obtain the current model volume (if the volume changes significantly under the loading condition), then include EVOL in your field output request. ABAQUS will compute the volume of each element. To obtain the total volume , just sum all the EVOL values.

A simple approach might be to check if ABAQUS can output the entire model volume for you as a history request.

If you want to average over a single element then you should divide the integral over that element (approximated by Gauss quadrature) by the real volume of the element.

 

[xerf]

What type of composite are you modeling ? (I've noticed you are using a 2D model.)