Learning Forum

[aleM2]

Hello everybody,

I've got some residual stress measurements in a structure and I would like to know if there is a way to implement the stresses in a FE model and then run an additional structural analysis. The residual stresses are only measured in a few points in the structure and not over the entire body. I've read that in Ansys it is possible to use the command INISTATE to implement a prestressed state but my question is what happens if I try to add these residual stresses in just a few points in the structure? Will the structure be in equilibrium? What will happen in the rest of the structure where I do not insert residual stresses?

Does anyone have experience with a similar problem?

Thank you in advance!

[Sean Harvey]

You can use inistate yes and that is the command at the mapdl level, but you can also use Workbench with external data component. You import your residual stress into external data. Then you can map onto a mechanical mesh by connecting it to the setup cell. You could also import an mapdl mesh to map onto using external model component in Workbench. If you need more details on this, let us know.
The issue you brought up is real. We know in a real part, if you sample it at some locations you will get a spatial distribution of residual stress, but where you don't measure does not mean the values are zero. So you will have to check the mapping and use some of the mapping options to see how the mapping should hand data points outside the point cloud, etc. Sometimes you need to modify your spatial data to include some other locations and values such that you don't end up with physically unrealistic mapping.
Your structure will achieve equilibrium during the solve as it will expand, contract, bend, etc. to balance the initial stress. Where you don't have residual stress, there won't be any, so the key is to get the mapping correctly.
I've seen customers do this successfully. They do need to work with the data and the mapping to get a good spatial representation.

Let us know if this helps.
Regards Sean

[aleM2]

,
Many thanks for your reply. Your comment is very helpful.
so in practice what I should do is to export my nodal coordinate and then modify the text file adding the columns for the residual stresses? my model is pretty complex with many nodes so I guess I will need a script to do that or do you know another method?
after having created the text file with the nodal coordinates and stresses, I import it into Mechanical as you described, connecting the external data module to the setup. Following, I add my loads, pressure, temperature etc.. and the residual stresses will be applied as external load.
is my understanding correct?

thank you!

[Sean Harvey]

So, there is no need to export your nodal coordinates, but you can imagine a bounding box that would have data points values for other regions of your model away from the measured locations. The interpolation/extrapolation can be controlled via the options in the imported initial stress object. You can set the mapping control to manual, and then change weighting and transfer type, etc. There are lots of advanced options too. You don't want to be trying to assign initial stress to your nodal coordinates as this would be too painful, but rather have some data points that can encompass the model thatthe mapping can use and come back with values. Now you will need to tinker to get this to give you reasonable data, and may need to add more points, but the idea is to let the mapping algorithm do the work. Again, provided what it comes back with and shows contours of looks reasonable.


For your 2nd question yes. Here I have fixed supports, displacements pressure, and imported initial stress from external data. That entire initial stress is applied at the very start of the solution.

Best of luck. Thanks.
Sean