Learning Forum

[mital.patel]

I have a 2mm thick square object, and I'm applying an 800K temperature to one side. For both steady-state and transient thermal analyses:

• Should I explicitly apply room temperature to the opposite side, or is it automatically considered as room temperature? 
• If I specify the thermal conductivity of the material, does it automatically account for reducing the temperature on the opposite side?

Thank you 

[peteroznewman]

If you have a solid body with 6 sides and you apply an 800K temperature to one face and no boundary condition to the other 5 faces, Ansys assumes those 5 faces are insulated.  That means the Steady State solution is the entire body will be at 800K.

If you apply a room temperature boundary condition to the opposite face and leave the 4 other faces unspecified (insulated), the steady state solution will be a linear temperature gradient from room temperature to 800K through the thickness of the body.

If you apply a convection boundary condition to the opposite face and provide a film coefficient and set the ambient temperature to room temperature, the steady state solution for that face will depend on the value of the film coefficient and the thermal conductivity.

Thermal conductivity is a physical property of the material. The conductivity can be temperature dependent.

I suggest you take the free course: Intro to Heat Transfer.

[mital.patel]

Dear Professor,

Thank you for your comprehensive explanation. I have a follow-up question regarding thermal boundary conditions in structural analysis, particularly in the context of a pressure vessel.

In my scenario, the Fluent analysis assumes an adiabatic outer side wall (Q = 0), and I have only inside wall temperature values along with thermal conductivity data for different temperatures. For the structural analysis, should I apply a boundary condition of room temperature or an appropriate thermal condition to match the adiabatic condition on the outer side?

Additionally, considering the pressure vessel context, where I have inside wall temperature and thermal conductivity information, how should I handle the thermal boundary conditions on the outer side in the structural analysis?

Your insights on both aspects would be immensely helpful. 

[peteroznewman]

Dear Mital,

I'm not a Professor, but thank you for the compliment.

The Fluent model used an adiabatic (insulated) outer side wall, and you solved the model with the Energy term enabled to obtain the inside wall temperature. Was the wall a solid body so there is a mesh through the thickness, or was the wall a surface and the thickness was an assigned property of the surface? In Fluent, did you use temperature dependent conductivity for the wall material? If you had a solid body and the correct conductivity, then Fluent has already solved the wall temperature and there is no need to do a Thermal analysis in Mechanical.  You can export the wall temperature from Fluent and use that as a load on a Static Structural analysis where other loads such as pressure and supports on the pressure vessel can be applied to calculate the stress in the wall material.

Did the Fluent model also solve for the Pressure on the inner wall?  That load can also be transfered to the Static Structural analysis unless it is essentially a static pressure (or hydrostatic pressure if it is a liquid and you solved with Gravity) that can just as easily be defined in Mechanical without transfering that data.

What is the actual boundary condition of the real pressure vessel you are simulating?  Is it well insulated or is the outer surface of the wall warmer than the room air temperature and there is convective heat transfer into the ambient air?  If that is the case, and you know the heat transfer coefficient for that wall, you would create a convective heat transfer boundary condition in Fluent on that outer wall.  If you don't know the convective heat transfer coefficient for the outer wall, then you can create an air domain outside the outer wall and let Fluent compute a temperature on the outer wall and the inner wall.

[mital.patel]

Dear Sir,

Thank you for your detailed explanation regarding the thermal and structural analyses of the pressure vessel.

In the Fluent analysis conducted by the thermal analyst, it was assumed that there is no heat transfer through the outer wall of the pressure vessel. As a structural analyst, my objective is to determine the structural response of the vessel to the thermal loading.

Here is my understanding of the setup:

1. Fluent Analysis:

   • Adiabatic boundary condition assumed for the outer wall, with no heat transfer through it. This analysis done by CFD people, And as a output they are giving the inner side wall temperature to solve  structural analysis.

2. Structural Analysis:

   • Using the wall temperature obtained from the Fluent analysis as a thermal load in the structural analysis.
   • Applying fixed supports and pressure loading on the inner wall.
   • emperature-dependent material properties considered for the pressure vessel.

Considering these conditions, I intend to run both steady-state thermal analysis and structural analysis in ANSYS Mechanical.

My question is whether the proposed approach for the structural analysis, utilizing the Fluent-derived wall temperature as a thermal load and incorporating fixed supports and pressure loading on the inner wall, is appropriate for assessing the structural response of the pressure vessel to the thermal loading. or in this case also i have to apply outside room temperature ?

Your insights on the correctness of this approach and any additional considerations would be greatly appreciated.

Thank you for your assistance.

[peteroznewman]

Assuming the Fluent model used a thick solid wall, Fluent solved for the temperature at every node in that wall, including through the thickness of the wall. The outer wall will have a temperature above room temperature.  Since the Fluent analyst assumed no heat transfer at the outer wall, you will do the same.  Was the Fluent analysis Steady State or Transient?  You may have results for both.

As a Structural analyst, you will start with the Fluent Steady State temperature results for the wall.  You will use a Static Structural model.  You don't need to do a Steady State Thermal analysis. Since the assumption of no heat transfer past the outside wall of the pressure vessel has been made, the temperature of the supports will be unchanged, so there is no unknown temperature in the Structural model. The supports will be at room temperature.

Compare the geometry for the solid body wall of the pressure vessel that was imported into Fluent with the solid body of the pressure vessel you want to use for Structural analysis.  Ideally, you have the exact same geometry, however, you may have other bodies such as supports for the pressure vessel that you will need in your model that were excluded from the Fluent model.  Describe how the supports interface to the pressure vessel wall and how they are fixed to ground. How will you model that connection?

In Static Structural, you will import the Fluent temperature load and apply the internal pressure load. Those loads will cause the pressure vessel to expand and that will cause stress in the vessel wall and in the support structure. Is the fluid in the vessel a gas or a liquid?  What is the density of that fluid?  Do you need to consider the weight of that fluid in the analysis?  If it is a gas, then the pressure load is all you need.

[mital.patel]

Thank you for your guidance and clarifications. I'd like to provide additional details regarding the approach I'm taking, as per your suggestions.

1. Fluent Simulation Details:

   • The Fluent simulation was conducted in a steady-state mode.
   • The simulation results provide temperature profiles for the inner side wall of the pressure vessel and the pressure inside the vessel.

2. steady-state thermal module:

   • This temperature profile represents the temperature distribution within the inner side pressure vessel wall.
   • I am uncertain whether I should also apply the outside temperature of the outer body in the analysis. If not applied, would the outside temperature be assumed to be the same as the inside temperature due to the insulation effect you mentioned. 
   • so this temperature output is use as a thermal load in static structure module.

    

3. Static Structural Model:

   • In the Static Structural model, I'm applying the imported temperature profile as a thermal load to represent the temperature distribution within the vessel wall.
   • Additionally, I'm applying the internal pressure load to simulate the pressure inside the vessel.
   • The fixed support is applied at the bottom of the vessel to simulate its fixation.

4. Material Properties:

   • All material parameters for the geometry are temperature-dependent, reflecting the behavior of the materials under thermal variations.
   • The stress calculations in the structural analysis are based on the thermal-structural coupling, considering the effects of temperature on material properties.

Overall, the analysis aims to accurately capture the thermal and structural behavior of the pressure vessel under the specified loading conditions. Your insights and guidance have been invaluable in refining the approach.

I would appreciate any further suggestions or considerations you may have regarding this methodology.

[peteroznewman]

Steady State Thermal

A solid body for the pressure vessel will be meshed. The Fluent output of the temperature of the inner surface of the pressure vessel wall will be imported as a load to this model. The boundary condition on the outer wall will be insulated (zero heat flux) which you can apply or leave out since it is the default behavoir on any surface that has no boundary condition in a thermal analysis. The solution will be the temperature throughout the wall.

Static Structural

I suggest you create a support structure for the pressure vessel. The base of the support structure can be a Fixed Support, while a few small pads at the top of the support structure can have bonded contact to the pressure vessel wall. This will allow the deformation in the pressure vessel wall between the pads to be spread over the dimensions of the support structure, keeping the stress in the pressure vessel wall low. If you directly apply a fixed support to the pressure vessel wall at those same pad areas, large stresses will be created in the pressure vessel wall.

If you don’t have any design for a support structure, you can simply pick three or four pads on the outer surface of the pressure vessel and use a Remote Displacement. Set all six degrees of freedom to 0 and change the Behavior to Flexible. The will avoid any stress from being created in the pressure vessel wall by the fixation.

Drag the solution cell of the Steady State Thermal onto the Setup cell of the Static Structural to import the wall temperature load. 

For the pressure you can use External Data to import the Fluent pressure load if it is non-uniform due to flow conditions in Fluent. A uniform pressure can be created in Static Structural, but since you have Fluent data, use that instead.

[mital.patel]

Thank you very much for providing such a detailed explanation. Your insights will be immensely helpful for referencing in my work. I appreciate your guidance and will certainly look into the free course you suggested.

Please consider this discussion closed. Once again, thank you for your time and assistance.