Learning Forum

[cvish92]

Hello all,

 

I am trying to run a conjugate heat transfer analysis for a 2D system. I am trying to understand the temperature evolution profile of the blocks as hot air is blown across it. 

 

 

As you can see, initially the temperature of the air is patched to be 500 and that of the block is around 300. I have modeled it with aluminium as the material. 

 

When I run a steady state conjugate heat transfer analysis, I get results as shown below : 

 

 

This makes sense since at steady state the block will eventually reach the temperature of the hot air blowing across it. 

 

But when I run a transient simulation, my temperature profiles after a small interval of time are as shown below : 

 

 

Zooming in further : 

 

 

It looks like the thermal gradients only develop on the fluid side and not in the interior of the solid. I reran the simulation with a very high thermal conductivity and I still get the same result. Also - I probed the nodes to find the temperature values and those on the block still remain to be at 300 K. Is there something I am missing out in my simulation modeling  ? 

 

Left end - Velocity Inlet 

Right end - Pressure Outlet

Walls - Adiabatic 

Block - Modeled with Aluminium (also modeled it with very high conductivity in second trail) 

I look forward to your response. 

 

Thanks ! 

[peteroznewman]

I am studying Conjugate Heat Transfer and will take a look at your model. Please create an archive .wbpz file and attach it to your post.  Also say what version of ANSYS you are using.

I made my own 2D model.

Here is the air after 1000 s.  The block started out at 300 K.

Here is the block colored with the Local, not the Global range of temperature.

If I wanted to see higher thermal gradients in the aluminum block, I would lower the thermal conductivity, not raise it.
I divided the conductivity by a factor of 1000 and simulated 200 seconds.  Here is the block of aluminum.

The air mesh should have an inflation layer around the block. Your mesh seems to have tet elements that are way too big.
Here is an example of an inflation layer.

[Rob]

Did you set any wall temperatures? You want to retain the coupled wall between fluid & solid, and use a Patch for higher/lower temperature and not a boundary condition. Patch is covered in the initialisation section of the manual. 

[Rob]

Nicely done Peter. You may want to refine the mesh to pick up separation: remember in CFD we have to mesh to geometry & flow. Adaption is your best option here. 

[cvish92]

Thank you so much @Peter and @Rwoolhou.

 

Peter - I believe I ran it with the 2D inflation layers (I know it's kinda hard to see it). The reason I increased the thermal conductivity was to decrease the size of the time step to run the transient simulation - The temperature profile should change in a short period of time.I will double check my model and get back to you both. The one thing that I did not check and should have was the y+ values for the system. I will check that as well. The ANSYS version used was 19.2.

Rwoolhou - I did not set any wall temperatures. The walls of the air flow channel were set to no slip and adiabatic. As mentioned, I patched the initial temperatures for the fluid and solid domains. I gave an air velocity inlet with the temperature of the air domain I initialized in the patch to keep it consistent. 

Let me know if there might be anything else that I should check. I will update this post today and let you know if I have any issues  

Thanks again ! 

 

[cvish92]

Hello @Peter and @Rwoolhow

 

It looks like I can now see a gradient. I made small changes : 

 

1. Increased inflation layers 

2. Selected required turbulence model based on y+ values 

3. Used an adaptive timestep 

4. Ran a simulation with scaled down conductivity for around 1000s. 

And now I see the gradient : 

 

 

I will use a hex mesh to run the next simulation to save more on computational costs. 

 

Thanks ! 

 

-Vishnu 

[Rob]

Looks better. In 2d don't select any surfaces for plotting contours, that way you won't see all the cell edges. 

[cvish92]

Sounds good. I know this is pushing it but, is there any way to overcome the CFL restrictions ? In general - it would take a long time to run the simulations. 

Or any other ways to general optimize the runs to reduce machine processing time ? (Other than getting more cores)

 

Thanks ! 

-Vishnu 

[Rob]

Sort of, but it depends on the precise physics of the problem. Unfortunately, that also falls foul of our engagement rules: I know how to break the (physics) rules but I can't tell you on a public forum.....  

Speeding up the current solve means more cores, re-ordering the mesh (now done automatically) or a faster cpu.