

June 16, 2020 at 2:33 pmMed91Subscriber
Hello,
i am simulating natural convection in a 2D pipe section with two material layers (r1 and r2) as shown, i want to know if it is possible i can impose a heat flux as a WALL boundary condition at r2, expressed in wat/m2, should i precise the wall thickness ?
also is it possible to impose this heat flux as a source term for the first layer material, expressed in wat/m3? if yes what calculation should be made(since it is a 2D model)

June 16, 2020 at 7:33 pmKarthik RAdministrator
Hello,
1st question  yes, you need to specify thickness here (at r2). Once you specify thickness, you will need to specify the volumetric heat generation rate (in W/m^3).
2nd question  All 2D models in Fluent use 1m as depth into the plane. You should base your calculations on this.
I hope this answers your questions.
Regards,
Karthik

June 16, 2020 at 7:56 pmMed91Subscriber
Thank you for your response, could you explain more why i should impose a heat generation rate ? since i have only one condition which is a heat flux on the wall in W/m2

June 17, 2020 at 12:25 amKarthik RAdministrator
You have two fluids surrounding the wall region, the wall boundaries in Fluent will have a coupled condition. You might not be able to apply a heat flux boundary condition on these coupled walls. To avoid this issue, I was suggesting you use the volumetric heat generation rate.
I hope this helps.
Karthik

June 17, 2020 at 8:08 amMed91Subscriber
just to be more precise, the fluid domain is only the external domain,outside the circles where i draw a square as fluid domain , and i impose temperature on each side of the square of 278k, i also applied on r1 a convective wall heat condition with temp of 338 k and h=587 W/m2.k
(r1 = 115mm, r2 = 136mm, r3= 186mm)
i am getting a very high values of temp when i apply a heat flux boundary condition of 25000W/m2 on r2 , and when i plot the surface heat flux and r1 wall , the value is 0!! as if there was transfert to the inside, and on r3 i got a very high value for heat flux
i tried to put a heat generation rate of 25000W/m3 on r2, and specified a wall thickness of 1m, and i left the heat flux as 0, i am still getting the same problem (very high values of temp).

June 17, 2020 at 12:38 pmKarthik RAdministrator
Thank you for the explanation.
I misunderstood your question. I thought there were two fluid regions. If you have just a single fluid region and if heat flux on the wall is physically correct, then that is what you should apply.
Are you running a steady state model? What material properties are you using between r1 and r2, and also between r2 and r3? What is your initial temperature of the domain?
Also, is your solution fully converged?
Thanks.
Karthik

June 17, 2020 at 12:57 pmMed91Subscriber
thank you for your reply, well i am using two materials,and i am running in steady state and using hybrid initialization
first Material (r1 r2) : steel with density of 8000kg/m3 , thermal conductivity = 45k/mk and Cp = 450J/kgk
second material (r2 r3) : density = 4000 kg/m3 , thermal conductivity = 0.17 k/mk and Cp = 1700J/ kgk
on the 4 walls of the suqare outside (fluid domain) , i am applying T= 278k
on r1 i applied a convective heat boundary condition with h = 587 w/m2k and T = 338.4 k
on r2 i applied heat flux of 25489 W/m2 with 0 wall thickness ( even if i put a value for wall thickness that does not make big change)
yes the solution has converged pretty well with 10 e3 residuals for velocity and 10e5 for energy
the problem is i am getting temperatures of order of 3000 k !! ,and when i plot the surface heat flux on r2, it is zero !!

June 17, 2020 at 1:10 pmKarthik RAdministrator
There is something fundamentally incorrect with your setup. Have you performed shared topology on your geometry when you create the CAD?
Ideally, you should see a coupled wall at the r2 boundary because you have two different material properties across it. If you provide a volumetric heat source in the cell zone between r3 and r2, you should see thermal energy being conducted across r2 into the cell zone between r1 and r2.
Right now, the boundary r2 is acting as an insulated wall and therefore, you are not seeing any flux.
Please perform share topology on your geometry in SpaceClaim and reload the mesh in Fluent. You should see a coupled wall condition on the surface r2. During meshing, please create surface named selections for each material (solidsteel1 and solidsteel2)
Let me know if this helps.
Karthik

June 17, 2020 at 2:47 pmMed91Subscriber
i did the shared topology on space claim on both edges r2 and r3, and i set the condition as coupled wall as shown
you said the volumetric heat source will be in solid2 (cell zone r2  r3) , but that case, the heat source should be in solid1 (cell zone r1r2)! with convective boundary condition on r1
i put the heat flux i have in W/m2 as a source term in solid1 (r1r2), expressed in W/m3 ( please confirm if it is correct to put it that way since i have the heat flux in W/m2)
now i am getting normal temperature and i am getting good values of heat flux 352 W/m2 on r3 and +264 W/m2 on r1
the problem is that when i do curve plot for the temperature on r1 and r2 are the same (337.9K) , almost similar to convection temperature boundary condition i put on r1 (338.4) , is it logical to have this similar temperature and the fact that the temp of r1 did not change much from initial value ?

June 17, 2020 at 3:45 pmKarthik RAdministrator
I'd say  calculate the overall power in W from your heat flux (W/m^2)  Simply multiply W/m^2 with the surface area over which you are applying. This will give you the equivalent W.
Then, calculate the volume of your cell zone where you intend to apply this power to (remember depth is 1 m for 2D analysis in Fluent). Now divide the equivalent power by the effective volume of the cellzone to get the W/m^3 value. You should be using this value.
Remember that the overall input power to your computational domain must remain effectively the same in both cases.
Regarding your second point, could you please increase your heat transfer coefficient to 10,000 W/m^2.K and change the free stream temperature to 273 K? Please apply this value to r1 and see if the results are different.
I think you are getting physical results. Heat is being added in your problem at r1 as well as in the cellzone between r2 and r3 (via the volumetric heat source). Because the thermal conductivity is relatively high for steel between r1 and r2, you are seeing a more or less uniform steady state temperature.
If any of the previous posts was useful in answering your question, please mark is as 'Is Solution' to benefit others on this community.
Thanks.
Karthik

June 17, 2020 at 4:30 pmMed91Subscriber
well , i tried to change the convection boundary conditions as you said ( T =273k and h = 10000 W/m2), still same remark T at r1 = T at r2 = 273K = initial condition
for the calculation of W/m3 i did like you said , now the source heat rate is bigger = 373498 W/m3 and the T at r1 = T at r2 = 345 k ( which is different now from the initial convection Temp at r1 which is 338.4k)
another thing, you said "Remember that the overall input power to your computational domain must remain effectively the same in both cases."
can you explain more about that ?
and also one more question, when i plot the heat flux on r1 its only 14300 W/m2 and on r2 is 680 W/m2, if we do the sum up it is not even the value of initial heat flux injected which is 25489 W/m2

June 18, 2020 at 12:32 pmKarthik RAdministrator
Hello,
 Regarding my comment on the overall input power being the same  When you are converting the surface heat flux to the volumetric heat generation rate, it is important to ensure that the total power (in Watts) for both cases remains the same. The total power (in W) is obtained by either integrating the surface heat flux over the area or the volumetric heat generation rate over the volume. Please take a look into your Total Heat Transfer Flux Report. You should find this in the Results Tab of Fluent (Results > Reports > Fluxes > Total Heat Transfer Rate)
 Regarding your second question: The heat fluxes should not add up to your input power. If your solution is properly converged, you should see that your net power (in W) crossing all your boundaries (and your sources) should be small. Again, please take a look at the heat flux report.
Thank you.
Karthik

June 18, 2020 at 2:16 pmMed91Subscriber
well, for the flux report, i am getting a user source of 5463 W and an overall net Result of 15373 W ( when i select all boundaries, as shown)
this value of user source is exactly the sum up of power on both r1 and r2,(which are the boundaries of solid2 where i injected in cell zones a heat rate of 1297934 W/m3 based on calculations you said), and this net resut is the difference which describe the error ?
one thing also i noticed, when i compute area in surface intergrals in r1 for example i got 0,3618m2, while my r1 is only 0.1152m !! so how it is calculating this area (same for all other area which are differnt from reality)
when i add up all the values of fluxes , i get a value of 20837, what represent this value ?
and also, even that i imposed all my residuals to be 1e6 for all i am not getting this value in results, do that mean my solution has not fully converged ?

June 18, 2020 at 3:27 pmKarthik RAdministrator
Yes, your solution is not converged. Are you solving natural convection here?
What solution methods are you using? What density model? What are your operating conditions? Can you share your screenshots?
Thanks.
Karthik

June 18, 2020 at 7:07 pmMed91Subscriber
Yes i am solving natural convection,in that case it is stated that the fluid domain has to be in 278k initially) , and it is infinite, fluid domain, so i took a square and i defined all 4 sides as walls and imposed 0 heat flux ( please confirm if it is the right way to define those boundary conditions ? or should i put pressure boundary conditions ?
Now, the solution residuals changed, and the Net Results value is less (which means i have better energy balance ?)
do you think now the solution has converged ?

June 19, 2020 at 11:58 amKarthik RAdministrator
Hello,
If the domain is completed enclosed by walls, please use either 'Incompressible Ideal Gas law' or 'Ideal Gas Law' for density. If you are using the incompressible ideal gas law, please make sure to fix the operating pressure. You cannot let the operating pressure float. Please don't use Boussinesq for closed domains.
Regarding energy balance  for a good converged solution, your net results should be very small compared to the smallest value of heat crossing any boundary in your flow domain. About 12%
By that standard, you solution in not completely converged. Please change the density model and rerun for a longer number of iterations.
Thank you.
Karthik

June 19, 2020 at 12:43 pmMed91Subscriber
Well in reality the domain is not closed, since it is infinite full of fluid, but it has an initial temperature of 278k, except the bottom is wall,so i put that value in operating condition, and i put pressure boundaries as shown
the problem is that i am getting a strange velocity profile,why the velocity is concentrated in one point like that ? could give more details or suggestions ?
ONE more IMPORTANT question please, in that case, how can i inject the the source term in W/m2 instead of W/m3 ? because i tried to enter an expression in the source term tab, once i set the unit as W/m2 , it can not take it

June 22, 2020 at 12:08 pmMed91Subscriber
any suggestions please ?

June 22, 2020 at 12:24 pmKarthik RAdministrator
Hello,
My apologies for not replying earlier.
If you are using a source term, you should be using the units W/m3, and not W/m2. Please use my comments above to convert your W/m2 into an effective W/m3.
Regarding the other questions  are you still using the Boussinesq approximation? If so, your operating density does not matter. You have to specify an operating temperature. If you are using an Incompressible Ideal Gas, then you need to specify an operating density.
Also, could you please change your side (both left and right) and bottom faces to pressure inlet and the top face to pressure outlet?
What are the Reynolds and Raleigh numbers of your flow?
Thank you.
Karthik

June 22, 2020 at 1:22 pmMed91Subscriber
Well, the problem is that i am using the source term only because i did not get good results when using a heat flux boundary condition on r2 so i don't know why i am not able to get good results when applying W/m2 on r2 ?
yes i am using boussinesq approx, and the operating temperature is the same i am imposing at pressure boundaries (278k)
i changed the inlet and outlets as you said, now i am getting heat balance around 1%,, and the velocity field is not really logical,
any suggestions please why i am getting this strange velocity field ? and every time i increase iterations (5000 to 7000) the velocity field change
for the rayleigh number, based on the water properties, and temperature difference (2 deg, between r3 and fluid wall temp, and length scale i have(length of the square side) , i got a value of 3.4 e7
and for reynolds number, i dont know which velocity to take , since it is varying from different boundaries

June 22, 2020 at 4:11 pmMed91Subscriber
any suggestions please ?

June 24, 2020 at 2:18 pmRobAnsys Employee
To clarify, you have walls all the way around the domain? If you want to add heat to the whole pipe region use a source term, if it's to the inner surface of the pipe it's a heat flux.

June 24, 2020 at 2:35 pmMed91Subscriber
well, the domain is supposed to be open, so i put a pressure inlet on bottom with 0 pascal and 278k, and pressure outlet on Top with same conditions
and symetries on both right and left sides, and i am supposed to have a heat flux boundary condition on the outer surface r2 of the pipe
i have two problems:
first, why when i impose a heat flux on r2, i can not see any heat transfer, but when i use a heat source i am able to see a heat transfert out of the pipe ?
second, why is my velocity field is so strange as seen in the picture attached ? i see velocity value all over the domain even that i put the fluid domain walls far
even if run for further iterations (7000 same result)

June 24, 2020 at 3:23 pmRobAnsys Employee
Assuming there is no r1 pipe then it should give much the same result. Remember the flux in r2 will be W/m2 and the source is W/m3 so it's possible you missed a digit somewhere. I assume it's a multibody part and you didn't break the coupled wall condition at r3.
You also need to check you set the operating density as per the Bousinesq Method. Try back flow from neighbouring cell too and extend the domain in the "up" direction.

June 24, 2020 at 3:37 pmMed91Subscriber
as explained in previous comments, i did convert the value i have in W/m2 to W/m3 (by multiplying by the perimeter to get Watts and then dividing by the surface to get W/m3) .
and i imposed a coupled wall conditions on both R2 and R3
for the boussinesq approx, from my knowledge it is not necessary to set up the operating density, only the reference temperature is required right ?
and could you give more details how can i set back flow from neighboring cell ? you mean in pressure outlet to set the backflow direction from neighboring cells ?

 You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 Suppress Fluent to open with GUI while performing in journal file
 Floating point exception in Fluent
 What are the differences between CFX and Fluent?
 Heat transfer coefficient
 Getting graph and tabular data from result in workbench mechanical
 The solver failed with a nonzero exit code of : 2
 Difference between Kepsilon and Komega Turbulence Model
 Time Step Size and Courant Number
 Mesh Interfaces in ANSYS FLUENT
 error in cfd post

3660

2534

1745

1226

580
© 2023 Copyright ANSYS, Inc. All rights reserved.