I am interested to find out the effects of the existing condition of residual stresses in the model on the structural analysis output stresses. In theory, residual stresses can alter the final state of output stresses via superpostioning of stresses. For example, a model with an intial compressive residual stress can "nullify" the external tensile stresses applied onto the part.
I have tried using thermal mapping in NX10 to create a variation of residual stresses along the depth of the model before subjecting it to further structural analysis. However, I feel that a more intuitive method is to enter these residual stress values directly into the model either nodes by nodes or elements by elements, albeit it will be rather tedious for a large model. May I enquire if NX10 is able to allow the users to enter these stress values directly into the model before performing further analysis?
Solved! Go to Solution.
NX Nastran will start supporting residual stress (or strain) as an initial condition in NXN 11 - comes out in May. This will only be supported in SOL 401.
The typical workflow is that you will have stress or strain results from some other solution in a results file that can be read by NX Post. In NX Post you would create a tensor field based on that result. Then you can create a SOL 401 solution and for it you can define an Initial Stress/Strain load type and reference the field you created. You need to put the load into a preload subcase and then define any service loads in subsequent subcases. When Nastran solves, it will first apply the initial stress or strain and depending on how balanced the load is, there can be an initial deflection as a result. Then the service loads are applied on top of these loads and the resulting stresses will be a combination of both load types.
Note that the mesh of the results file and the analysis model do not have to be the same. NX will take care and map the created field onto the analysis model mesh. And you can choose to map the load to either elements, nodes, or nodes on elements.
Hope this is of some help.
This workflow would require generating a solution that provides a residual stress distribution within a part. This solution would then be use as a stress pre-load for the subsequent stress analysis involving service loads. Thus, modelling the mechanical or thermal process that give rise to the initial residual stress would be unavoidable.
I was thinking of a more straight forward method to bypass this step. For example, I could obtain the residual stress results via experimental measurements and inputing this empirical results into the model to create a residual stress distribution. The problem is finding an appropriate method to input the obtained values into the model. One method that I have chanced upon recently was to create a load field using ISO lines.
I would love to receive suggestions on other methods of inputting these stress values.
Thanks for your prompt response Mark!
I came across this INISTATE command available in ANSYS that can take the effects of residual stresses into account. May I know if there is a similar counterpart available in Siemens NX environment?
The initial stress/strain loading that I mentioned in a previous response is very similar to the INISTATE capability in ANSYS. It will be supported in NX Nastran in the v11 release coming out this year. This solutoin will be supported in the NX Multi-Physics environment. There the user can create a tensor spatial field of stress or strain and apply it on the model as an initial load. Typically the field is created from an existing result set - but can be created from other sources including from test data.