Adaptive Mesh in Multi Phase Flow Simulation Using Ansys Fluent
HTML-код
- Опубликовано: 29 июн 2024
- What is Adaptive Mesh?
In this video, on behalf of Alpha Omega team, 3D Dam break, a classical two-phase flow problem, was solved using the adaptive meshing technique in ANSYS Fluent. Mosaic meshing (Poly-hexcore) was used in ANSYS Fluent meshing to generate the mesh with the total number of 50,753 cells. The Volume-of-Fluid (VOF) method was implemented in ANSYS Fluent to simulate the two-phase (air-water) flow in a tank. In order to refine the mesh, only near the gas-liquid interface, the dynamic adaption mesh with maximum refinement level of 2 was applied. It is demonstrated that such dynamic adaptive mesh can successfully refine the mesh near the interface region and keep the coarse meshes elsewhere in the computational domain., which can be helpful to reduce the computational time.
Example: 3-D Dam Break
Mesh number: 50,753 cells
Mesh type: Mosaic meshing (Poly-hexcore)
Fluids: air and water
Multiphase method: VOF + Dynamic adaption mesh with maximum refinement level of 2
Mesher: ANSYS Fluent Meshing 2020R1
Solver: ANSYS Fluent 2020R1
Get in touch:
Contact form: aopds.com/contact-2/
Email: john.condon@aopds.com
Phone: (724) 544-0393
www.aopds.com
Learn more about our ANSYS upcoming Webinars & Events:
aopds.com/ansys-webinars/
See what's new with our Blog:
aopds.com/blog/
#aopds #ansys #simulation #cfd #flow #fluent #multi #phase #adaptive #mesh #dynamic #spaceclaim 
Наука
Nice simulation, and great job in providing step by step tutorial. Thanks for sharing
You are welcome!
Interesting video, enjoyed it a lot!
Glad you liked it.
Thank you.
Thanks 😊
You are welcome!
That's a great detailed tutorial. Love it!
How many mesh elements did you have? Please also share the details of your simulation machine and the simulation clock time. Thank you.
Please see the description for more information related to this tutorial. The base mesh number was 50,753 cells. For 2 seconds of simulation time, using 112 Cores and 8 nodes (in ANSYS Cloud), the computation took about five hours.
The Adaptive mesh must be computationally heavy to take 5 hours on just 50,000 cells on 112 cores. Did you use Ansys elastic cloud?
Thank you very much for this step-by-step video tutorial on FLUENT, really helpful.
Also, can we perform the same in ANSYS 19.0 version?
This specific multiphase VOF predefined dynamic adaption is available after ANSYS 2020 release. For the prior versions, the user needs to go through several other manual tasks for VOF dynamic mesh adaptation. You need to enable the "Refine and Coarsen" options in the "Gradient Adaption" dialog box. Please see Chapter 30 of the Fluent User's Guide (2019) and go through Dynamic Gradient Adaption Approach (see Section 30.4.1).
@@alphaomegaproductdevelopme323 much praise for your kind response. I was trying to figure out the procedure for Dynamic/adaptive mesh in my VOF model and with the help of your assistance I will finally be able to do it.
@@alphaomegaproductdevelopme323 I've been using version 2023R2, and boy it seems the VOF adaptive mesh is much more cumbersome and super unintuitive. It isn't activated by default (even with VOF multiphase setting) unlike in the previous versions, and there's no clear instruction to do so (not even in the manual). Looks like a bug but who knows.
Tq u so much for the video ♥️.
Of course, let us know if you have any questions!
@@alphaomegaproductdevelopme323
I have a doubt if this simulation has baffle with holes do we need to define contact or just same process?
@@tejeshreddy1055 The simulation process will be essentially the same. No need to define contact. The only thing you may consider is to refine your mesh near the holes by adding local sizing in the pre-processing.
@@alphaomegaproductdevelopme323 on doing so I am unable to see animation if time step is 0.0001 but I am able to see pressure contours and if time step is given 0.01 then simulation gets stopped after 20 iterations.
1. Should I need to refine my mesh more ?
My current mesh size is 1mm at all edges
And default at remaining surfaces.
Thankyou sir/madam for your reply
@@tejeshreddy1055 Instead of a fixed time step, you may use the "Adaptive Multiphase-Specific" time step as shown in this video. This method adjusts the time step based on the Courant number in each iteration. In addition, this type of simulation (multiphase + dynamic mesh) is a heavy computation and generates huge amounts of data and requires high RAM, so if you are having difficulty to see the animation, it might be related to the hardware capability. You can try selecting “In Memory” or “HSF File” for storage type in Animation Definition to see how it works. And regarding your mesh size, as long as you have a good mesh quality (Minimum Orthogonal Quality>0.1 and Mesh Skewness
Hello, thanks for such an informative video, but I would like to request you to answer one question. What are the boundary conditions, PV-Coupling Scheme, and URF values that you have set for this calculation? You have not used the energy equation, is it necessary or not?
Thanks for watching our video. Boundary conditions are all no-slip walls. SIMPLE method was used for pressure-velocity coupling. Under-relaxation factors are all the default values of VOF method:
Pressure: 0.3, Density: 1, Body forces: 1, Momentum 0.7, Turbulent Kinetic Energy: 0.8, Specific Dissipation Rate: 0.8, Turbulent Viscosity: 1
Since this is an isothermal example and we were not interested in temperature and heat transfer calculation, the energy equation was not used in this particular tutorial.
Hello, sir, can you please tell me, why I'm not able to patch cells that I've marked, with (Volume fraction= 0) for air ?? I've tried a lot but my whole volume is showing air.
Check the input coordinates in the region register. This issue normally occurs when the input coordinates are not properly assigned.
Thanks for the really nice step-by-step explanation!! Could you please comment on two settings you did?
1.Why did you chose k-omega model? I would assume the flow is mainly laminar, or am I wrong?
2. Why did you chose explicit VOF formulation? From my experience the implicit formulation is much faster and also reliable. Thank you very much for your reply.
Turbulence model is selected because the flow is locally turbulent, especially at the initial moments where the water column hits the obstacle.
The explicit VOF formulation was used to allow using geometric-reconstruction scheme to capture clear, crisp interface without numerical diffusion. In addition to that, explicit scheme generally has better numerical accuracy than implicit scheme. Let me know if this helps.
@@alphaomegaproductdevelopme323 Thank you for your reply! That helps a lot. Regarding the turbulence, how did you determine if the flow is locally turbulent? Was that an assumption or have you calculated that theoretically? I have a similar problem and I am not sure if the laminar model is adequate to use (overall the flow is laminar according the Reynolds number)
@@janweggen7606 The assumption of the mentioned locally-turbulent flow is more intuitive in this case and it comes from the nature of flow features when it suddenly hits solid obstacles. In addition to that, a rough calculation of Reynolds number using the initial water column height (H), and maximum velocity of sqrt(g*H) shows that it exceeds the critical value for channel flows. Therefore, the assumption of turbulent flow seems to be more realistic in this case. It is worth to mention that since the main purpose of this tutorial was to demonstrate the multi-phase adaptive meshing technique, the other settings related to the model setup are not probably the best choice and can certainly be enhanced. For example, the model can be fine-tuned by testing laminar flow or choosing some other turbulence models and compared to the existing experimental data or theoretical results.
Thanks for your comment on that! That helped a lot.
Hello, thanks for this great video. Could you explain a little bit on how to apply adaptive mesh if Eulerian model is applied rather than VOF? I found the adaptive mesh button is grey when I selected the Eulerian model. But as you showed in this video, it works well with VOF. Thank you.
The multiphase VOF mesh adaption is unavailable in Eulerian model, and therefore, you cannot select anything from "Predefined Criteria". Perhaps, in the future release, there will be some built-in mesh adaption for Eulerian model. Remember that VOF and Eulerian models are based on two different approaches of solving momentum and continuity equations. However, you should be able to manually apply mesh adaption in Eulerian model. You need to first create a new "Field Variable" under cell registers, and then active the dynamic mesh adaption under "Adaption Control". Please refer to the mixing elbow example (the 1st example) in Ansys Fluent Tutorial for the detailed information.
@@alphaomegaproductdevelopme323 Thank you.
AMR is not required in other 3D hydraulics VOF codes for such cases with maintained accuracy. Neither is the requirement to solve for the gas phase.
Thanks for this helpful tutorial. Does mesh adaption significantly slows your solution? This always happens to me when I try to simulate droplet motion.
The mesh adaption technique that is described in this tutorial applies to almost any type of volume-of-fluid (VOF) simulations including liquid droplet or gas bubble. For the motion of liquid droplets or gas bubbles, the mesh adaption set up will be the same as demonstrated in this video. In general, this method helps to avoid the unnecessary fine meshes in most of the computational domain and thus, can significantly reduce the computational time. In addition, since the mesh adaption enhances the mesh resolution near the interface of gas-liquid, it leads to a sharper transition from one phase to another and therefore provides more accurate results. In order to have a good balance between the simulation time and proper mesh resolution, it is important to have the base coarse mesh. And if still the simulation is slow, you can reduce the maximum refinement level and increase the frequency.
Thanks for your reply. Have you ever managed to do the post- processing for an adaptive mesh in CFD-post? I always get a message that adaption results are only available in CFF format and it doesn’t seem supported till now in CFD-post ( Ansys 2020R2).
Concerning my first comment, I got a reply that might be helpful from ansys forum coordinator that looks helpful.
Here is his answer : If the model is run in parallel you'll be overloading one cpu, so need to use load balancing.
@@Mohamed.wael7 There are two ways: (1) You can force Fluent to write the result out in legacy data format (.cas and .dat) which can then be read into CFD-Post. To read or write legacy files in both the current session and future sessions, open the General tab of the Preferences dialog box, select Legacy from the Default Format for I/O drop-down list. (2) You can also set up automatic export of CDAT files using File/Export/During Calculation/Solution Data.
@@Mohamed.wael7 Thanks for sharing the comment here.
can we use adaptive meshing for species transport model for chemical reactions?
Thank you, Sir. What is the difference between this method and PUMA?
It's essentially the same. In the past, automatic adaptive mesh refinement was not possible for polyhedral cells. But now, when you use multi-phase adaptive mesh, Fluent automatically uses polyhedral unstructured mesh adaptation (PUMA).
Hi. I've tried to regenerate this simulation. However, my final animation doesn't have a smooth and fine water appearance like yours, it shows exactly the scene-1 iso-contour. May I miss any settings?
There are some practices to make a better animation in FLUENT. Modifying the lighting option can change the final animation, defining proper contour for the surface, as well as proper export settings for the final rendering all have effects on the animation. Also, CFD-post is very powerful when it comes to creating visually realistic animations.
zone-surface: cannot create surface from sliding interface zone.
Creating empty surface.
Can I know why this happens
Is this error related to the tutorial presented in this video? If so, in which step you got that error?
Is the Adaptive mesh feature works for complicated VOF cases as well??
Thanks for your question - Yes, Adaptive meshing can be applied to complicated VOF simulations as well.
Hello, Can you make a video on LES and DES models on similar concepts?
I am also interested in paid course
How many hours did it take to complete for 2 seconds???
Mine is of 48 cores , still I approximated to 56 days from what numbers I got in the console. Total of 40,000,00 iterations and could complete only 56,200 in 18 hours. I used the same dimensions roughly and mesh size.
I had to terminate after 18 hours. 56 days are so long!
Please tell me how much time your pc took for 2 seconds.
It shouldn’t take that much time. Did you use parallel simulation? Be careful about recording the animation. I selected the animation to be recorded in every 0.001 s of flow-time (NOT time step), to avoid generating too much output. This will not only consume lower RAM, but also significantly increase the computational time. Also, make sure that you use a proper dimension. My domain dimension was 100mm*200mm. I actually used ANSYS Cloud for the computation. Using 112 Cores and 8 nodes, it took me less than five hours for 2 simulation seconds. If you want to know more about Ansys Cloud, please visit this video: ruclips.net/video/RGvV-_ntSvk/видео.html
@@alphaomegaproductdevelopme323 thank you so much. That helped me a lot. I used the parallel simulation. But went for every time step solution animation, I think this is the reason for massive hours.
Thanks for your response 😊.
if i would like the tank to rotate how am I suppose to set the condition, please? BTW thank you so much for this video!
Under wall boundary conditions, you can set "wall motion" as "moving wall" instead of the stationary wall, and prescribe the absolute "rotational speed" as well as the "rotation-axis origin" and "direction". Note that, you need to assign the same rotational speed and rotational axis direction for all walls. But carefully assign the different rotational axis origin to the walls so that the entire tank rotates properly. For rotating flows, due to the large pressure variations, "PRESTO" or "Body Force Weighted" should be used for the spatial discretization. Also, unlike this example where we are interested in the transient behavior, if you are looking for the steady-state behavior of a rotating flow, the better approach is to enable the "frame motion" under cell zone conditions, and set the rotational velocity there. And then, set the walls to be stationary relative to the adjacent cell zone. Let me know if this helps.
Alpha Omega Product Development Systems Thank you so much for your reply!
(I actually use this program to study the water flow in a hollow sphere that rotate around Y and Z axis with the velocity 100 rpm, containing water in a half of its volume: in case you want to know.) I had run the calculations already before I saw your reply (TT) I went for the Cell Zone Condition and used the mesh motion ( Will the result come out okay?) with the velocity 100 rpm right now my computer still calculating the solution.... I’ve been waiting for 2 days! Does it take such a long time like this? And due to your reply I understand more about frame motion and the other ways to control the rotation many thanks 🙏
@@Popocandy_ n general, the transient simulation of two-phase flow in combination with frame/mesh motion should be computationally expensive, and therefore you need to consider your computational resource to handle this simulation. If you are using the adaptive mesh, I would suggest you make a coarser base mesh. For more information about the rotating domain simulation in Fluent and how to set up such models, please refer to the chapter 10-12 in the Fluent User’s Guide. Regarding the time - you could consider adding HPC or using the ANSYS Cloud offering.
Alpha Omega Product Development Systems You are so helpful! Thank you so much! And one last question how did you record the animation in that water color and such a smooth surface? My calculation is done but in my solution animation the water surface is sooo rough... or I did something wrong (U__U)
@@Popocandy_ All the post-processing has been done using CFD-Post. When using the Iso-surface, I would suggest assigning a value of 0.99 or 0.01 (instead of 1 or 0) for air or water volume fraction to get a smoother interface. You can choose the water color using the constant mode in the color tab under the details of the Isosurface window. In addition, you can use the volume rendering option in CFD-Post by choosing the water volume fraction as the variable.
can u describe boundary condition in detail ?
Thank you for your question. The boundary conditions are all standard default wall. The problem was just initialized with the water column in the tank.
Can you please tell me how to use this feature in Ansys 18/19?
This specific multiphase VOF predefined dynamic adaption is available after ANSYS 2020 release. For the prior versions, the user needs to go through several other manual tasks for VOF dynamic mesh adaptation. You need to enable the "Refine and Coarsen" options in the "Gradient Adaption" dialog box. Please see Chapter 30 of the Fluent User's Guide (2019) and go through Dynamic Gradient Adaption Approach (see Section 30.4.1).
This specific multiphase VOF predefined dynamic adaption is available after ANSYS 2020 release. For the prior versions, the user needs to go through several other manual tasks for VOF dynamic mesh adaptation. You need to enable the "Refine and Coarsen" options in the "Gradient Adaption" dialog box. Please see Chapter 29 of the Fluent 18.0 User's Guide (Dynamic Adaption) and in particular, see Section 29.4 for Dynamic Gradient Adaption.
@@alphaomegaproductdevelopme323 Hello, I tried to follow the steps given in the manual, but I am unable to refine the mesh dynamically. I need to have 6 layers of refinement near the interface at time instances. Can you please guide me through the steps for Fluent 18?
@@varanasisaisubhankar8785 I haven't done this specific dynamic mesh adaption in Fluent 18 before. It is highly recommended to update to Fluent 2020. However, you should be able to do that by following the similar steps described in section 3.4.9 of the below tutorial for Fluent 18 (see pages 192-195).
Copy this link and put it in your browser: users.abo.fi/rzevenho/ansys%20fluent%2018%20tutorial%20guide.pdf
The above example uses the "curvature" of "temperature" for mesh adaption, but for VOF simulation, you may select "Gradient" for method and select "phase volume fraction" instead of temperature and also enable Dynamic in the Dynamic tab of the Gradient Adaption dialog box (pg. 193). Please also make sure to specify a proper value for both refine and corasen threshold. This should work and dynamically refine the mesh, if the rest of your VOF model is properly set up.
is it compatible with fluid structure interaction ?
PUMA is not available for FSI yet, because Polyhedral mesh is not compatible with Mechanical at this moment.
Hello sir. Can I have the geometry file?
vanderfiq9@gmail.com
Rafiq - thanks for your request - I would be happy to share the file with you - can you send me your email address to john.condon@aopds.com.
very good tutorial. could you send me the geometry file ??
muhammads.noureldin@gmail.com
I subcribe already bro, hello bro can you help me? I stuck in a cooling tower simulation for a long time still don know how to solve, thank a lot if you can help me.
Hi, the purpose of this channel is to give an example of the technology. If you would like for a consulting engagement - I recommend that your contact your local ANSYS Channel Partner.