November 1, 2018 at 8:31 amprashant kumar jhaSubscriber
i'm simulating heat and mass transfer inside two phase closed thermosyphon using 2-d axysymmetric geometry.i've selected pressure based solver and transient.I am using ANSYS /FLUENT 19 student version .VOF method with Lee Model is used . Water is used as secondary phase and Vapor is used as primary phase. SIMPLE algorithm scheme for pressure velocity coupling and a first order upwind scheme for the determination of momentum and energy is included in the model. Geo –Reconstruct and PRESTO discretization for the volume fraction and pressure interpolation scheme, respectively, are also performed in these simulations. but,after running the calculation,contour is showing only in the evaporator region as shown in attached figure.I've also patched the liquid water fill ratio with volume fraction=1 in the evaporator region.Can anyone help me out?
November 1, 2018 at 9:30 amDrAmineAnsys Employee
First of all: Please avoid generating Entropy by creating several topics regarding the same questions.
1/2D Axis Symmetric is only for the cases which are axis-symmetric. Can you confirm that from your side?
2/The contour shows only that some vapor has been generated in the evaporation section. Try to clip the contour to some lower values to detected condensation regions. You can even check the Mass transfer under Phase Interaction for post-processing.
3/With the Lee Model you have coefficients (frequency) and those would require a high amount of tuning and this tuning won't make any sense without exp. data or references. Generally the condensation frequency is set to lower value than the one of evaporation but it is case dependent.
November 2, 2018 at 6:33 amprashant kumar jhaSubscriber
sir.i am simulating the work done by B.Fadhl https://www.sciencedirect.com/science/article/pii/S1359431113004699.i've selected an axisymmetric domain as attached .The line at x=0 is the centerline.i've further splitted the right wall into three parts namely evaporator,adiabatic and condenser in ANSYS SPACECLAIM 19 student version.Frequency is 0.1 in Lee model as given in the article attached. The problem that i'm facing is that Contour shows the phase change only in the evaporator section.
November 2, 2018 at 6:42 amDrAmineAnsys Employee
I have said a couple of times: we do not have access to all journals across the world. From the abstract: the authors are using an UDF.
I wanted just to let you check if the case if rotational about the x-axis. If this is not fulfilled either you go to planar 2D or fully 3D.
You can clip the contour lines to something smaller to detect the condensation zones. Please check too the phase interaction post-processing variable.
November 2, 2018 at 8:51 amprashant kumar jhaSubscriber
it is rotional about the y-axis. Thermosyphon is cylindrical in shape.So,can i go for planar 2D.
November 2, 2018 at 9:04 amDrAmineAnsys Employee
No you do not need to do that. You can stick to axis-symmetric but we need to rotate it. So the "Y-direction" of the model will be your X-Axis. You can then take only the half of the diameter and model the section to be aligned with the X-Axis.
November 2, 2018 at 11:36 amKarthik RAdministrator
Just to add to Amine's comments:
- Please read the paper and make sure you are using the same set of source terms as the authors. If I am to speculate, they are using sources terms responsible of evaporation and condensation in the mass and energy equations.
- In addition to this, please make sure you are using consistent initial conditions, similar to what the authors have done.
- Another important factor is the mesh. If there is a way to verify the mesh, please make sure you are using the same resolution of mesh.
Replicating the results from a paper is always a challenging task. The most important suggestion I would like to give you is this - when in doubt about the exact steps used by the authors, you can always contact the authors of the paper via email. This is important as they might be able to clarify the exact model for you. Please let us know and we might be able to help you with questions regarding best usage and practices of the modeling tools.
November 2, 2018 at 11:53 amprashant kumar jhaSubscriber
So,is there any problem having vertical direction aligned with y-axis not with x-axis?
November 2, 2018 at 12:25 pmDrAmineAnsys Employee
In Fluent if you want to use the 2D Axis-symmetric solver then the symmetry/ rotational axis needs to be the x-axis. You can then just apply gravity in the -X direction.
November 4, 2018 at 9:26 amprashant kumar jhaSubscriber
sir, i that case,what will be the sign of g.Will it be g=9.8m/s^2?
November 4, 2018 at 8:10 pmDrAmineAnsys Employee
Example if the height goes from 0.0 to +HMAX in the positive x-direction. Then g will be -9.81 m/s^2.
November 5, 2018 at 8:51 amprashant kumar jhaSubscriber
November 5, 2018 at 9:08 amDrAmineAnsys Employee
All the stuff described in the paper is already implemented in FLUENT. You do not need to add any UDF. All required secondary source terms are accounted for.
November 5, 2018 at 9:13 amprashant kumar jhaSubscriber
for the energy source term,since latent heat of vaporization is 2455 kj/kg.I've incorporated the following udf for energy source term.Please,check it sir.
#define T_SAT 373
#define LAT_HT 2455.1345e3
DEFINE_SOURCE(enrg_src, cell, mix_th, dS, eqn)
Thread *pri_th, *sec_th;
pri_th = THREAD_SUB_THREAD(mix_th, 0);
sec_th = THREAD_SUB_THREAD(mix_th, 1);
m_dot = -0.1*C_VOF(cell, sec_th)*C_R(cell, sec_th)*fabs(C_T(cell, sec_th) - T_SAT)/T_SAT;
dS[eqn] = -0.1*C_VOF(cell, sec_th)*C_R(cell, sec_th)*LAT_HT/T_SAT;
m_dot = 0.1*C_VOF(cell, pri_th)*C_R(cell, pri_th)*fabs(T_SAT-C_T(cell,pri_th))/T_SAT;
dS[eqn] = 0.1*C_VOF(cell, pri_th)*C_R(cell, pri_th)*LAT_HT/T_SAT;
return LAT_HT*m_dot; }
November 5, 2018 at 9:30 am
November 5, 2018 at 9:30 amprashant kumar jhaSubscriber
November 5, 2018 at 9:39 amDrAmineAnsys Employee
You do not need require any UDF. Furthermore if UDF then I will go for DEFINE_LINEARIZED_MASS_TRANSFER.
November 5, 2018 at 9:47 amprashant kumar jhaSubscriber
sir, in paper they have considered latent heat of vaporisation as 2455kj/kg,how to incorporate that value in ANSYS FLUENT 19 STUDENT VERSION.
November 5, 2018 at 10:33 amDrAmineAnsys Employee
You use your working boundary conditions. Regarding mass transfer just use the implemented model and just provide the saturation temperature and change the frequencies.
Latent Heat in Fluent is in J/kgmol and you have the molar weight so you can incoprarte theier setting in Fluent.
You need to carry out some tutorials in order to get really started...
November 6, 2018 at 8:35 am
November 6, 2018 at 8:51 amDrAmineAnsys Employee
Same as usual: smaller time steps, lower URF's.. etc.
If it does not help then perhaps other community members might help you because as ANSYS Stuff I am not allowed to give more that I have already done.
November 6, 2018 at 8:59 am
November 9, 2018 at 5:48 amDrAmineAnsys EmployeeOr just take the molar weight in kg/kmol and multiply by the standard state enthalpy in j/kg.
November 20, 2018 at 3:20 pmgiovanni_ianzitiSubscriber
Hello, I`m working on the same model. Can we discuss about it if you want.
February 8, 2020 at 10:29 ampritam1688Subscriber
Can you share the case file if it's working well for you? I also want to know whether UDF is required or not?
- 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.
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 non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.