Combining load cases in Ansys WB

[nitinfem1]

Hi all,
I have two load cases, LC1 and LC2 that have different loading conditions.
I want to add stress values of LC1 and LC2.

For example:
Let S11, S12, S13 are principal stresses of node 1 for LC1 and
S21,S22,S23 are principal stresses of node 1 for LC2.

I want to get the summation values of corresponding stresses that is S11+ S21; S12 + S22; S13 +S23 for each node in the model.

I can export the values to excel and do the required operations, but due to large number of nodes in my model, it will be a hectic job to pursue.

Is there a way to do within Ansys workbench.

Thanks in advance

 

[FArias]

Hello

You could do it using the "Solutions combination" option, check the WB help. I think both solutions have to be inside the same simulation, though.

 

[nitinfem1]

Hi FArias,

I think the solution combination doesnt give the algebraic summation of the values. Can you please confirm it.

Thanks

 

[Drej]

Firstly. The solution combination provides combination of the results in the following way. Let's assume you have two results loadcases "A" and "B". With the solution combination selected, a third results set "C" will be created from A and B by:

C = (A x coefficent1) + (B x coefficient2)

you can choose the values of the coefficients to be whatever you want. Remember the following though:

- You need ANSYS Professional licenses and above
- Linear combinations are only valid if the analyses are linear
- The supports must be the same between Environments for the results to be valid. Only the loading can change to allow for solution combinations

Secondly. I would have a problem with why you would want to add the principals in the way that you've described. Not just the fact that you're adding shears to normals, but adding principal stresses is generally considered to be a no-no. Assume you're aware that principal stresses are direction dependent, and hence adding them will not give you a true stress state. Unless I'm missing something? Hope this helps anyway.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[nitinfem1]

Drej,

Thank you for the reply.
I want to add the normal stresses for different load cases, not the principal stresses as I stated in my first post.

what do you mean by "The supports must be the same between Environments for the results to be valid. Only the loading can change to allow for solution combinations".

You mean the boundary conditions must be same between two load cases??

I ran a simple analysis. a block with a fixed support on one face and force on the opposite face.In another analysis,I selected a different face and applied fixed support and also varied the magnitude of force.

When I checked the solution combination results, the normal stresses in X direction are equal to the summation of individual results from above load cases.

So, eventhough the boundary conditions and loads differ in load cases, the solution combination gives linear summation of the results.
Please clarify
Thanks

 

[Drej]

> You mean the boundary conditions must be same between two load cases??

Yes. The supports (restraints) have to be the same for each case. If the supports change for each loadcase, you have two different physical systems, which if you try to add the results together isn't valid.

> I ran a simple analysis. a block with a fixed support on one face and force on the opposite face.In another analysis,I selected a different face and applied fixed support and also varied the magnitude of force.

This isn't valid (see above).

> So, eventhough the boundary conditions and loads differ in load cases, the solution combination gives linear summation of the results.

Of course. ANSYS is just doing as it's told. It's up to you to provide the common sense and the interpretation of the results.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[nitinfem1]

Drej,
Thanks for the clarification.