Thermal input from non-linear static state to linear static state simulation

[Anonymous]

I'm looking for some assistance on where I'm going wrong setting up these analysis. 

I'm analyzing a piping system that is subject to high temperature load from the material (1400F). The system is bolted onto the outlet of feeder.

I set-up a nonlinear stead state heat transfer analysis and applied an initial temperature of 70F, a temperature load of 1400 to the inside of the piping and a convection load to the outside components of the system (ambient temp 70, convection coefficient 1.6985e-5 btu/(s*in^2*F). 

I load that temp output into a linear static analysis and also apply gravity to the simulation to see the combined stresses that will be seen throughout the model. But I get really high stress results and the stress locations are spotted throughout the chamber, piping and slide gates. 

My question is am I setting this up correctly? Or is the nonlinear analysis not necessary? (I did a linear steady state as well with similar results) 

Not applying the temperature output gives a max stress of around 52000 psi. With the temperature output from the nonlinear analysis its 712724 psi.

[John_Holtz · Accepted solution]

Hi @Anonymous 

I apologize for not responding to this your post early.

The type of thermal analysis does not matter, as long as the temperature distribution is what you want it to be. (linear steady state, nonlinear steady state, or transient. Of course, these different analysis types will produce different types of results, but you do not need to the "match" the thermal analysis type to the stress analysis type.)

It looks like the model is held at the flange where the 1400 F temperature also occurs. Are the constraints rigid and preventing expansion? Or have you allowed the part to expand?

It is not unusual for the thermal stress to be much higher than reality in the area of fixed constraints, basically because the analysis is not considering that the "ground" to which the model is attached is also heating and expanding, or that fully fixed constraints are an idealization that rarely exist in the real world.

In some cases, you may want to make a dummy part that you can bond to the model where is it constrained, and let that portion heat up in the thermal analysis. In the stress analysis, you put the constraints at the "ground end" of the dummy part, and then hide the dummy part (which now has the high stress) when presenting the results.

[Anonymous]

Thanks John.

I'm still getting really high stresses in the connection between the piping and the weld neck flanges. Intuitively these seem unrealistic. I've tried switching up the contacts at those contacts to see if they help but it doesn't seem to help. Maybe my intuition is wrong and I'm trying to get the simulation to confirm my preconceived notion but I'm not too sure.

Do the bonded contacts/separation contact interact differently with the thermal load? If those connections (pipe and weld neck flanges) are to be welded in the real world is a bonded contact the best solution in the simulation when analyzing the thermal stresses?