Try to couple thermal to static structural, instead of modal. So You will get the stresses firstly. Then You have to couple the static structural to a modal analysis to transfer the stress stiffening effects to it. So You should be able to investigate the thermal effects in the modal analysis.

steady state thermal -> static structural -> modal

If you want to use load transfer method you need to do exactly what Anton said and you will be able to perform a pre stressed model and send the result to Modal analysis. However you can perform a Structural-Thermal multiphysics analysis by using Element Solid226 or Solid227 (depens on what mesh you want to use) by using command Snippet in workbench. Then you need to set up the analysis in Static Structural analysis and chek the thermal results by using User Define Result. After you are done with this analysis, use pre stress method and pass the results to modal analysis.

I have done that before. The main goal of the study was to predict modal response of welded plates. In fact, the solution was obtained using ANSYS multiphysics and the procedure involved three steps: first thermal analysis was done to obtain the temperature history and the results were saved as (filename.rth); second a structural analysis was carried out using thermal results as a load to obtain the subsequent mechanical stresses(here you need to switch finite elements and use prestress option); third we used the structural model with its residual stresses to run a modal analysis to obtain the natural frequencies of the welded structure.   

Thanks for all your valuable comments. They are really helpful

The problem is (as I am experiencing this my self) that Modal analysis might not "read" the imported (pre)stress/strain condition of the static structural correctly. The Modal analysis imports only linear data (even if non-linear properties are defined in Transient Thermal and Static Structural)!!! And for Modal Analysis only Youngs Modulus and Mass (densitiy of material) play an important role.

I am also trying to simulate the effect of pre-stressed conditions - RESIDUAL stresses (due to incremental "moning heat point" thermal effects - not welding just surface heat treatment at lower Temperatures) on circular plate. What is important for me is to know how this effects Eigenfrequencies. So far I did not get results good enough (compared to experiemntal measurements). Does anyone have any suggestions to my thoughts? What am I doing wrong?

Might be that my residual stresses are not computed properly...I dont know anymore... :/

Did you use pre stress thermal-structural analysis or you used a coupled thermal-structural analysis?

Thank you for your reply.

I used coupled transient thermal and structural analysis.

Matej,

Your question made me to learn new things! I ran a case study and assumed that you are using either solid226 or 227 with the keyopt of 11. These are my findings. Modal analysis uses linear perturbation type of analysis to predict the Eigenfrequencies. For that reason it doesn`t use **interpolated times** from the solution of solution of the nonlinear static analysis. Therefore, it uses the closest time saved result for calculating Eigenfrequencies. Your guess about not properly reading the result was 100 percent correct. You need to brake down your analysis to multiple time steps and substeps (of your choice) and save the result of each by generating restart points. Then, you need to create multiple prestressed modal analysis to investigate each time step or substep individually. You can adjust this in Pre-Stress(Static Structural) from modal analysis tree.

I think the problem you are solving is transient and the state of your model is changing significantly over the time. Therefore, if you want to see the variation of frequencies over the time, you need to follow this methodology. By the way, mesh generation has a significant impact on the results in this kind of analysis involved with residual stress.

That should get you started.

Hope you will solve the problem. As always, If my answer was help full, recommend it!!. Let me know how your analysis went if you want. I got cirious about it!!