March 19, 2021 at 6:37 pmAnadi_MondalSubscriber
Greetings! I am using EWF and DPM to model annular flow.
For EWF , I got these information ANSYS user guide:
1.The material properties for the secondary phase should be the same as the DPM particles.
2.The name of the secondary phase material should be included in the name of the DPM particle’s material and should be appended with the string ‘-particle’ (for example, if the secondary phase material name is waterliquid- eulerian, then the DPM particle’s material name should be waterliquid-eulerian-particle).
3.The wall film cannot be solved without first initializing the wall film model (using the Initialize button) to initialize the wall film variables and prepare the solver for the solution procedure.
I am using vapor as primary phase and water as my secondary phase and droplets .
Here is the short description of model:
"The simulation includes a two-dimensional Eulerian liquid film model coupled to a three-dimensional core model (including vapor flow and droplets) based on the Eulerian – Lagrangian approach"
Please see the attached image and would you give me any idea why I am not getting any residuals for liquid phase? Why the model is not showing data for wall film?(I know know it's not converging but that is not my concern now ,I can change other setting but I want to see the residuals for water)
AnadiMarch 25, 2021 at 12:00 amSurya DebAnsys EmployeeHello, Not really sure what is the issue here. I see all the proper residuals being displayed. I also see the volume fraction and velocity residuals of water.nThat is all the residuals that you need. You will be able to visualize EWF variables in Contours separately as well.nRegards,nSDnMarch 25, 2021 at 1:09 amAnadi_MondalSubscriberThank you sdeb!nHere you are seeing 6 residual curve (3 for vapor, one for continuity, one for k and final one for omega). I check the values for water in console ad it is zero. I have attached two images . I have tried to draw film thickness but not getting any single graph. Will you check the parameters ? I draw the pipe on XY plane and extrude in z direction. I have attached tube with zone for your convenience. I apply liquid mass flux at injection wall by EWF option. Mainly I need to draw wall film thickness of water and mass flow rate of water in annular section.nRegards,nAnadinnMarch 25, 2021 at 7:13 amDrAmineAnsys EmployeePlease plot first along a line and not the wall surface.nMoreover I am aware that some problems in the past related to EWF have been fixed during the last versions. Please update to the most recent version.nnWhat do you want to do?nMarch 25, 2021 at 7:23 amAnadi_MondalSubscriberHi DrAmine,nWhere should I plot a line? It'a 3D pipe. Actually I am trying to simulate annular flow in a tube. I divided the pipe in 3 section . 'Injection wall' to apply liquid mass flux, 'stabilization wall' to form the film and finally the film in 'annular' region. Mainly I need to draw wall film thickness of water and mass flow rate of water in annular section.nMore info about model,The simulation includes a two-dimensional Eulerian liquid film model coupled to a three-dimensional core model (including vapor flow and droplets) based on the Eulerian – Lagrangian approachnThe liquid film should be simulated as a two-dimensional Eulerian model while the vapor-droplets model should be simulated as a three-dimensional Eulerian – Lagrangian model, both models are simultaneously coupled.nnThank YounAnadiMarch 25, 2021 at 7:31 amDrAmineAnsys EmployeeI understand but why are you solving Eulerian Multiphase here if your core is (DPM) particle laden gas flow?.Doing XY Plot on surface is not pretty as you saw. Rather first check the contour plots of film thickness.nMarch 26, 2021 at 3:38 amMarch 26, 2021 at 6:02 amDrAmineAnsys EmployeeYou have discrete droplets so you do require DPM model and not Eulerian model. Model the droplets with DPM.nMarch 26, 2021 at 6:42 amAnadi_MondalSubscriberHello DrAmine,nI am modeling the droplets with DPM. But if turn off multiphase then there is not option to select vapor or liquid at inlet. Actually I am flowing only vapor at the inlet . Please see the attached image. How to select 'vapor velocity' at inlet after turning off multiphase? or should I select water-vapor in cell zone conditions for both zones to confirm only water-vapor in tube initially? So water-vapor in the tube and we will apply water-liquid mass flux through EWF at the wall to form film in the tube. Am I correct?nnMarch 26, 2021 at 11:07 amYasserSelimaSubscriberI see you have been in this issue for a while.nI suggest you increase the water void fraction at the inlet to a very small value .. let's say 1e-04 ... And then you can monitor the mass of liquid and see if condensation happens or not.nMarch 26, 2021 at 1:27 pmDrAmineAnsys EmployeeArray that is wrong: he wants to use DPM Model.nArray: DPM is relying on Lagrangian Framework. You can add whatever you want as droplet as Injection. In the Injection you prescribe from where the particles should be injected, the flow rate, their initial velocity, diameter, etc...nnKeep default DPM Boundary at Inlet and Outlets.nAt the wall please change the DPM Boundary to Trap and enable EWF on that particular wall. For EWF Model activate DPM Coupling.March 26, 2021 at 1:36 pmRobAnsys EmployeeIs the aim to have the droplets form the film? Note, the Eulerian multiphase model and Eulerian Wall Film are not linked and are not the same model. nMarch 26, 2021 at 5:05 pmAnadi_MondalSubscriber,Mainly the film will form on the tube surface due to applying water mass flux at a surface near inlet(injection_wall) by EWF model. But if liquid droplets from the core region(core region is consist of vapor and liquid droplets) touches the liquid film ,droplet will be trapped in the liquid film and added with the mass of liquid(liquid mass source)nThe overall scenario is:n1.In the core region of tube vapor and droplets will flow(core region is consist of vapor and liquid droplets)n2.Liquid film will form at the surface of tuben3.Liquid from the film can enter into the core as a droplets due to entrainment and if droplets touches the liquid film , it will be trapped ,and added with liquid mass (deposition)nI followed everything you mentioned in your last reply. nWould you tell me, Should I use Eulerian Multiphase model or not? If no, then I will turn off this model and run calculation again.nAccording to your reply, I am understanding this way,n1.Use DPM to simulate tube core. Here I can use injection to create droplets.n2.Use EWF to form liquid film on tube surface and coupled these two modelnAm I on right track?nI have added an image that I am trying to simulate.nThank you nAnadinMarch 27, 2021 at 8:00 amAnadi_MondalSubscriberHello All,nI try to run the simulation without Eulerian Multiphase but got this error:nDivergence detected in AMG solver: pressure couplednError at host: floating point exceptionnnError at Node 0: Floating point exceptionnError at Node 1: Floating point exceptionnError at Node 2: Floating point exceptionnError at Node 3: Floating point exceptionnError at Node 4: Floating point exceptionnError at Node 5: Floating point exceptionnError at Node 6: Floating point exceptionnError at Node 7: Floating point exceptionnnI have added the skewness report and I am using URF of DPM 0.1nWhat may be the problem?.Thank YounAnadinMarch 30, 2021 at 5:23 amDrAmineAnsys Employeelisten to he summarized everything in 3 lines. It is only a matter of the film thickness. If it very thick or gets wavy then Thin film model is not deployable anymore.nMarch 30, 2021 at 5:27 amAnadi_MondalSubscriberArray , I am experiencing the following error now. Do you have any idea to solve this?nDivergence detected in AMG solver: pressure couplednError at host: floating point exceptionnMarch 30, 2021 at 5:30 amDrAmineAnsys EmployeeQuite hard: Summarize now what you are using.nThe first thing if everything is well setup is to start with small time step size (assuming the mesh is of high quality).nMarch 30, 2021 at 5:46 amMarch 30, 2021 at 1:23 pmRobAnsys EmployeeI'd look at a pave mesh, the O-grid or butterfly mesh method isn't used much now we've developed solvers that don't need block structured meshes. Ie it's not been needed for about 20 years! That also resolves the high aspect ratio near the walls that may not help the film. Ironically, you've resolved the flow in the middle where we don't care too much, and not near the wall where we do! nApril 1, 2021 at 6:40 amAnadi_MondalSubscriberHello Array nI was getting this error,nDivergence detected in AMG solver: pressure couplednError at host: floating point exceptionnSo I am trying to find where is the error? This time I did not use UDF and DPM. I just use EWF and water-vapor in the core for test purpose. I check the contour and a think film is noticeable. But when I am trying to plot the film thickness, I am getting the following graph. Did I do any mistake to take the surfaces(X-axis)? How can I get a single graph of film thickness on the wall? or what is the way to plot film thickness? I plot the tube in XY plane and extrude in Z direction. If you need to know the mesh ,please see the 2nd top image of this post. If I can plot the film thickness, then I will turn on the DPM next.nThank You,nAnadinApril 1, 2021 at 9:26 amRobAnsys EmployeeYou tend to plot thickness on the wall, and use local range. For an xy plot you need a line, the easiest way is to create a plane (or iso-surface of mesh) and select the wall when you do that. The result is the intersect of the two surfaces which tends to be a line. nDivergence will be because the time step is large relative to the amount of vapour moving to the film. Time scales tend to be VERY small, so just keep dropping the timestep by an order of magnitude until it works. Also look at sub-stepping in the film set up. It's an area we're actively working on, and I'm waiting on the build so I can start testing the new options. nApril 1, 2021 at 2:56 pmDrAmineAnsys EmployeePlot on surfaces looks like that in 3D. Create a line. And: update to the most possible versions. nApril 1, 2021 at 5:05 pmAnadi_MondalSubscriberand nI create a line at the wall of the tube and getting film thickness as below. I see at some location film thickness is zero. Do you think the high velocity of vapor (12m/s)in the core is responsible for that? Actually I am expecting a stable (almost parallel line) film thickness on the wall as I did not apply any heat flux to evaporate the film yet and allowed enough time to form stable film .nMoreover, I am using water-liquid as film materials and flowing water-vapor in the core from inlet.nI am using university vLabs .I see 19.2 is the most updated version there.nThank you,nAnadinnViewing 23 reply threads
Ansys Innovation Space
- 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.Trending discussions
- 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.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.
Please Login to Report Topic
Please Login to Share Feed