Learning Forum

[al1419]

Hi all, this is meant to be a thermal analysis of the molten metallic alloy in a pipe but it seems as though the conduction feature is not working out despite using coupled walls for the fluid walls and the pipe's inner walls. This is what I did during the pre-processing stage:

1. volume extract inside the pipe to generate the fluid volume. The pipe is meshed with the fluid
2. create named selections - inlet,outlet,pipeinnerwalls, fluidwalls
3. This later autogenerated coupled conditions for the wall/shadowwalls

I ran the simulation with my velocity-inlet and pressure-outlet conditions and I think these are correctly assigned considering the results of the first image. Please does anyone know why heat conduction through the walls is not working? I don't think I'm able to use shell conduction as there's an already assigned thickness to the walls from the mesh.

[al1419]

also, I've varied the mode instead of using 'constant' mode (thinking there was something wrong with the post-processing but this didn't work either 

[Nikhil N]

Did you turn on the energy equation? If yes, what are the thermal boundary conditions?  Also check if the cell zone for pipe has been assigned with the correct material (and material properties). 

 

Nikhil

[al1419]

Hi Nikhil,

Thank you for your reply, yes I did turn on the energy equation and my thermal boundary conditions are 

velocity-inlet : velocity 2.21 m/s,temperature 470 c

This is the material property for the pipe

[Nikhil N]

'I don't think I'm able to use shell conduction as there's an already assigned thickness to the walls from the mesh.'

If you are explicitly meshing and solving for the solid pipe domain, you don't need to use shell conduction. 

 

Can you post a screenshot of the temperature contour?
Make sure you assign appropriate thermal boundary condition on the outer pipe wall as well. 

 

Nikhil 

[al1419]

Hi Nikhil,

 

Here is the temperature contour for the outer pipe wall! 

This is the boundary condition for the outer pipe wall. It's in contact with the surroundings so is it sensible to use a convection condition?

  

 

Many thanks,

Annie

[Nikhil N]

There you go. With heat flux = 0 there will be no heat transfer and you won't get the desired temperature distribution. If you know the temperature of the outer wall, go with the Temperature condition, else go with the Convection condition. 

Nikhil 

[Nikhil N]

Basically, assigning heat flux = 0 tells the solver that the walls are insulated. 

[al1419]

Hi Nikhil,

The temperature distribution showed (good news!) but is there a reason why I cannot see the pressure distribution on the outer wall on a local range? (I also have other pipelines as shown on the left)

[Nikhil N]

Instead of the outer wall, plot pressure contour on the inner wall of the pipe. 

[al1419]

Thank you!

I also have another issue with post-processing if you don't mind kindly looking at it. Whilst looking at the temperature distribution of this certain pipe, I've applied a 330 degree velocity inlet BC to the two pipes shaded in dark blue and a pressure-outlet at the end shaded in red. However the temperature distribution suggests the fluid's temperature increases? I don't think this makes sense. Is there something wrong with my initialization method? I used hybrid initialization and the velocity-in and pressure-out are the only BCs I used

[Nikhil N]

I think you are monitoring the temperature on the outer pipe and not the bulk fluid temperature along the length. If you want to check the temperature change for fluid, check for temperature at the inlet and the outlet. 

 

Nikhil

 

[al1419]

Hi Nikhil, 

Thanks for your reply, I checked the inlet of the fluid (see the image below)

and outlet 

The outlet still shows an increase in temperature and I don't know how to rectify this.

[Nikhil N]

Temperature contours won't give you a correct picture in this case. Can you check the mass-weighted average of the temperature at the inlet and outlet of the fluid domain? 

[al1419]

This is the mass weighted temperatures of all fluid outlets for 40 iterations and the outcome is unchanged still

 

[Nikhil N]

You should get 4 different values (2 for inlets and 2 for outlets). Assign the reports separately and not combined. 

However, for inlets, it will be the same as the boundary condition. Look out for outlets. 


Btw, what is the thermal boundary condition on the outer pipe wall? 

[al1419]

 

How comes there are 2 temperature values for inlet and outlet? And also, the thermal BC for the outer pipe wall is convective

(edit: apologies I've accidentally applied the report to only 1 outlet instead of all, I've assigned 1 outlet to the end of each fluid - will this be a problem? )

[Nikhil N]

There are 2 different pipes, right? Correct me if I am wrong. 

[al1419]

Yes there are. I see, when applying the outlet boundary conditions in the pre-processing stage, I applied 1 named selection to all 'outflow' faces of the fluid. Is this incorrect and instead I should apply 1 named selection to each face? (think this might the issue)

[al1419]

Oh I see, thank you so much! I'll let you know of the outcome

 

Many thanks,

Annie