March 23, 2021 at 7:29 pmharshabharadwaj1Subscriber
Hope you guys are doing well. I have a three phase system with oil, plastic and oil and I wanted to use dynamic meshing since the region between oil and plastic is of vital importance to me and I have to maintain good volume conservation of the oil droplet.
I am using Sphere of Influence method for meshing and not only is it taking too long, there is still not good enough volume conservation. The volume of the oil starts out at 1 and ends up at 0.8 approx after a while.March 23, 2021 at 10:13 pmYasserSelimaSubscriberThe panel is for mesh adaption ... it has nothing to do with dynamic mesh. Dynamic mesh could be selected from the left enu, under setup.nAlso I am not sure if you actually need dynamic meshing?nCan you explain what you want to do? Is it mesh adaption, or moving walls or mass transfer?nMarch 23, 2021 at 10:29 pmharshabharadwaj1SubscriberThanks a lot for the reply. nLet me make things clearer.nnAs seen in the image above, there exists an oil region that I patched at the top of the channel. This droplet exists inside a plastic region.nWith the current mesh(image attached above) that I am using, there is not good enough volume conservation and I am losing mass as the oil deforms. I am thinking of alternate modes of meshing and as suggested by dynamic meshing would greatly help my case. Hence, I was thinking of setting up dynamic meshing between the oil and the plastic region, since I have to accurately predict the shape of oil droplet.nHope I am being clear enough.nMarch 23, 2021 at 11:22 pmYasserSelimaSubscriberI see. Dynamic mesh adaption based on VOF .. Thanks for explaining this to me. nI think you should select cell registers and then field variable and define the VOF of oil in your case. nMarch 24, 2021 at 12:56 amharshabharadwaj1SubscriberHello,nThanks for the reply. Can you/someone please elaborate on this? I read up some stuff but I am still a bit unsure as to how I can do this.nWould I have to delete the current region that I have patched?nMarch 24, 2021 at 2:48 amYasserSelimaSubscriberNo, do not delete it ... As I understand, Rob suggested to have fine mesh where you have oil ... So, you need to have the dynamic adaption occur according to the criteria of having oil VOF larger than certain amount ... 1e-04 for example.nTo set this criteria, select cell registers and field function ... then phase .. volume fraction ... oil .. and set range with max and minimum ... and select the number of time steps you want fluent to check the criteria for remeshingnMarch 24, 2021 at 9:46 pmharshabharadwaj1SubscribernThanks for the help. I think I got it, Although I still need something clarified. nHere is how I do it. nnWhy is the droplet like this?. The way I understand this, you setup a coarse mesh and you define the interface where you want a refined mesh. So, shouldn't the shape hold accurately, if we do this?. Below are images for 0s, 0.02s and 0.04s. What am I doing wrong?nnThe shape holds properly if I do not do mesh adoption. Should it not be the opposite, since we are increasing the number of elements at the interface.nAlso since I am using a STUDENT version, is there a way I can limit the maximum number of elements/created ?. Because from what I can see from above, it is creating a huge volume for mesh adaption, even though its not needed.nThanks for all the help.nMarch 24, 2021 at 10:20 pmYasserSelimaSubscriberThe droplet is like this because oil diffuse inside the polymer ... Care bout the mass balance. Monitor the mass of the oil and see if it being conserved or not, within certain error of course.nNot sure if you can limit this or not, but you can change the criteria of 1e-04 to decrease this volume if you are close to the upper limit of cell countnMarch 25, 2021 at 10:37 pmharshabharadwaj1SubscriberHello.nMy mass increases considerably after a point and I do not seem to understand why. Increase in mass does not make sense to me. What does this mean?nDerivative option is gradient and scaling option is Scale by Global Maximum. nnThe increase happens when the drop is about to leave the converging section of the channel.nnAlso, if the volume fraction of the drop does not change, does that not mean that the mass is being conserved?.March 25, 2021 at 11:02 pmYasserSelimaSubscriberCan You show the residuals?.March 25, 2021 at 11:44 pmMarch 25, 2021 at 11:56 pmYasserSelimaSubscriberI suggest you increase the number of iterations in the time step. nThe change in the mass is because of the high residuals ... Double the number of iterations and see if this makes a difference nMarch 26, 2021 at 3:13 pmharshabharadwaj1SubscribernThanks for all the help. Increasing the number of iterations in the time step, gives me a great mass conservation (around 98 - 99%).nAlthough, the residuals still do not converge. Do you have any suggestions as to what I can do about this?. nAlso, how accurate are my results if the residuals do not converge?nMarch 26, 2021 at 3:44 pmYasserSelimaSubscriberI will discuss the accuracy in a later comment this weekend. But for now, I think this is a great achievement. Give it a try by increasing the iterations a little bit more and see the effect.nnMarch 26, 2021 at 4:19 pmharshabharadwaj1SubscriberThank you.nI did. I was initially doing 20 iterations/time step. After that I did 40 iterations/timestep which gave me around 98%. Doing it at 50 iterations/timestep gives me around approx 99.5% mass conservation, which is quite good.nI look forward to your comment explaining the accuracy of the simulation when the residuals do not converge.nThanks again.nMarch 26, 2021 at 4:40 pmRobAnsys EmployeeI'd also try halving the time step. The most common cause of mass loss/gain (other than exercise and chocolate) is failing to resolve the time scales seen in the model. nMarch 27, 2021 at 12:29 amYasserSelimaSubscriberHere is my comment regarding accuracy. nAny numerical calculations, has some sort of error. And we try to minimise this error until it is negligible. To minimise this error we do sensitivity test trying to find the coarsest mesh size that makes the error negligible. We do the same with the time step trying to have largest time step that makes the error negligible ...nWhen we run the simulation, we look for convergence ... what is convergence, it is a solution that does not change with doing more iteration, or change within our acceptable error margin .. To know that the solution does not change, we look for the residuals to become constants ... reaching straight line. Even if the value is still large 1e-2 for example, we can still consider this as converged solution.ow the question is, can I trust the results after all of this? The answer depends on the application ... If you try to publish CFD results without comparison with experimental data, the first comment from the reviewers will be on validating the model. So, we always look for the closest trustful experimental data and try to replicate the results. Then we validate the model within uncertainty range .. And now we are able to change the parameters and do our study.nSo, I am not going to judge the results and I am leaving this for validation!nViewing 16 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
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.