Learning Forum

[manelaero2020]

Hi all, 

I am modeling the following problem (please see picture ) with Fluent. 

What do you think about what I have input (ok? no? more suggestions? ) 

• for conduction heat transfer through the thin wall,>> shell conduction model, specification of the thickness and number of layers (here 1 layer)
• For convection heat transfer between the outer side of the wall and the cold-free stream,>> the convection model is on with the specification of heat transfer coefficient h and the temperature of the cold-free stream. 

I'm very thankful for your assistance 

Kind regards 

 

[Rob]

You only need shell conduction if you are seeing hot spots on the wall, for most applications the flow will convect heat as rapidly as conduction so it's not needed. 

Otherwise, yes, a "thin" external wall with a set thickness (you may want to change the wall material from aluminium) with external HTC and free stream temperature is usually a good approach. 

[manelaero2020]

Hi @Rob , 

Thank you for your response :) 

Yes, there are hot spots on the external wall due to significant hot air Temperature ( 150°C) 

I'm more sure now of the approach: shell conduction for HT through the wall and convection HT for exchanges between the external side of the wall and the cold-free stream 

[Rob]

Shell conduction is for ALONG the wall in the solid part. A thin wall with a thickness will handle heat passing perpendicular through the wall. 

[jackhc0609]

hi I tried to use the sheet separate the 2fluids but when go to fluent ,it shows wall and wall shadow belongs to fluid1 and fluid2.but there is no thin wall.howcan I set the thin wall thickness?thx

 

 

[jackhc0609]

then I tried to interface the wall and wall shadow .but still into going well

[Rob]

Wall & wall:shadow should be set as Coupled (default option) and you may want to give it a thickness. That means you have a conformal mesh and (should have) heat transfer. 

[jackhc0609]

wall and wall shadow each belongs to fluid1 and fluid2, I can directly set the wall thickness on the wall or wall shadow?

[jackhc0609]

I think I should create the thin wall then set the prototype and thickness ,am I right?

[Rob]

If you have a wall & shadow pair then you already have the wall. You can then give it a thickness (only need to do this once) and a material type unless Aluminium (default) is OK. 

[jackhc0609]

in other words,though wall and wall shadow belongs to flui1 and fluid2.I can directly regard wall and wall shadow as the solid zone, directly set as AL METAL and 0.30mmthickness? am I right ?

[Rob]

Correct, the two labels are the two sides of the wall. You only set the thickness once, and leave the thermal setting as "coupled". You may also want to review shell conduction. 

If the wall is truely "external" then you can set a HTC to the outside and a free stream temperature. It depends where you want to end the modelled domain. 

[jackhc0609]

could i consult u another question.in the Steady-state simulation of fluent of a gyroid heat changer,1. the converge  curves are very fluctuant,but the outlet temperature tend to be stable.my volume mesh is 0.89 measured by fluentmeshing skewness.how can i deal with the fluctuant converge curve?

 

[Rob]

Assuming you're just monitoring an area/mass average on the outlet you may be missing some flow features in the domain. 

Remember, a residual is a function of the solver error. So, your initial condition could be really good; or (more likely) there's an unresolved flow feature or transient in the solution. For the latter point monitors will pick up more information, as will taking contour/vector plots every 5-10 iterations for 50-100 iterations. 

What you may find is the fluctuation/error/something is negligable. I always cover "poor" convergence in training: check monitors, fluxes and residuals. Then think about what each is telling you. 

[jackhc0609]

what I cannot understand  is wall and wallshadow each belong to fluid1 and fluid2,if I click on wall and wallshadow to set the thickness of the solid wall ,i thick the fluid may have a leakage due to wall and wall shadow becoming part of solid wall.I also think another wall and wall shadow is needed to represent the solid separated wall .it must be something wrong with me?

[Rob]

A wall without a shadow only has cells on one side, so the grey and blue surfaces, if external, would be wall with no shadow. Change one of the fluids to solid (you will have to turn off flow boundaries) and see if any walls form or you see any warnings. I'd be surprised if the wall & shadow switched anywhere, but if you have isolated regions it could be correct. 

[jackhc0609]

i really have separated regions by cell zones as fluid1(blue) and fluid 2(grey),so my consideration of interface the wall and wallshadow  to create the solid thinwall's (interface)wall&wallshadow is unnecessary?like the pic shows.
 

[Rob]

They're walls so should still be coupled. I don't recommend messing with interface zones at this point. 

[jackhc0609]

today i dothe simulation accordi.g to your methld.butwhether or not add the thinwallthinness .the result is same .

[jackhc0609]

i think there must be sth wrong with it

[jackhc0609]

could you give me a cas.h5 case about heat exchenger thin wall separate 2fluids.I think there must be some understanding on it

[jackhc0609]

https://drive.google.com/file/d/1x-K26eOqndJXMgkUgxH6lzRKeuA58oNz/view

hi today i do the simulation according to your methld.but whether or not add the thin wall thinness .the simulation result is completely same .i think something wrong in my undersatanding and precess.Could you take a look at my case by link to download.It just 60mb. thanks very very much.(probably 2023r1 cannot open it smoothly ,but 2020r2could smoothly open it . )

heat exchanger working process:

1.bafflesset 0.3mm and material s(poly).

2.set separated wall (0.3mm &material s)

[Rob]

I'm not permitted to download anything. It's one of the rules staff operate under to avoid any issues with Export Law. 

Looking at the images you have a fluid & other zone. So we can see that's working. If there is no difference in result between setting a wall thickness or not, is that because the flow is slow enough that the fluid-wall thermal transport is the limiting step on heat transfer?  Remember, the overall heat transfer is a function of fluid1-wall, wall conductivity and wall-fluid2     I can't remember the equation, it's been a while! 

[jackhc0609]

before I set the fluid0.08kg/s,now I set both fluids all 1kg/s.there is still no difference in result between setting a wall thickness or not.Please help me .I think there must be something wrong
?

[jackhc0609]

[jackhc0609]

now i run 1000iterations，they are still same

[Rob]

Please post a contour of temperature along the centre plane cutting the inlet/outlet pipes. You may need to create a separate isosurface of mesh for each fluid zone. 

How does the heat flux balance look?

[jackhc0609]

when I use fluent2020r2. two computers all use half of the ram.first computer ram256g,it most use110g.another computer ram 140g  it use 70g most .how can I use completely ram?

[Rob]

Fluent will use what it needs, so around 2-3GB RAM per 1M cells (models, solver settings etc cause the variation) as a rule of thumb. 

[jackhc0609]

today i SEE twice .when i using the FM to partition mesh,when ram is170gb,error appear (mpt_accept: error: accept failed: Not enough space),my pc ram is 256gb.how can i do.ansys 2020r2.

[Rob]

That's a parallel error. Was there anything else in the TUI? 

[jackhc0609]

[jackhc0609]

[Rob]

And at the top of that list? 

[jackhc0609]

can u give me a teaching VIDEO OR PDF of a thinwall separate two fluids to simulate the heat exchanger  in fluent thanks now i didnot go through the process

[Rob]

I don't think we have one, the tutorials in Help (or Learning on here) cover most areas of meshing and the solver. How are you for disc space in the working and scratch folders?

[jackhc0609]

 disc space 4T+ 

[Rob]

Not sure then. How many cores were you meshing on? Speed up is OK for some cores, but if there are problems try on one. 

[王 zhe]

another thing to consult you is how can i see the tpms wall temperature contour in cfd post,i cannot find the true wall so i cannot create the wall temperature contour.

[Rob]

You may need to add daat fields to the cdat file, not everything is transferred and some fields are calculated in the Fluent solver as needed. We post process mostly in Fluent too: CFD Post use for Fluent is far less common than 4-5 years ago. 

[王 zhe]

how can i add data field in dat file for the tpms wall?what shou i add?

 

[Rob]

Have a look for the cdat options in File>Export. However, wall temperature might not be an option as it's technically a facet value so switching from the Fluent cell based to CFD Post node based storage may cause issues. 

[王 zhe]

one thing i could not understand is your advise preocess of viewing the  wall heat flux,as i was using thin wall mode which has not a really thinkness wall,so i cannot choose the really wall in postprocessing like the pic shows,how can i do?

[Rob]

Heat flux should be available on internal walls too.