November 24, 2020 at 9:55 pmTingWangUNOSubscriber
Dear ANSYS learning forum,
I’m an ANSYS Fluent academic version user.
I’d like to request help in improving convergence (better continuity residuals) for the phase-change modeling of steam condensation of steam condensation inside the paper dryer (domain shown in Fig. 1). The simulation results are good for low heat flux cooling (-1000 W/m2), however, as the cooling heat flux is increased the continuity residual becomes higher a lot. To be specific I would like to improve the convergence and get lower continuity residuals for Cases S-5 (steady-state) and S-10 (transient) with details below. Please reach out if you would like more details on the setup.
The objective of this simulation is to model condensation of steam inside the domain shown in Fig. 1 above. The model is simulated as an axisymmetric domain as shown in Fig. 1 (b).
Steam (water vapor) and liquid water (1e-6 volume fraction as seeding droplets) enter the domain from the inlet (shown in blue) with a constant velocity inlet. The gage pressure is specified at the outlet of the domain. A constant heat flux (negative in value as heat is removed) is specified at the circumferential wall.November 25, 2020 at 4:26 pmRobForum ModeratorIf you look at the flow field what is different in the later cases? Which model are you using for phase change? nDecember 1, 2020 at 3:56 amTingWangUNOSubscriberThank you for your response.nI'm using the Eulerian model with evaporation/condensation model: thermal phase change with constant value of saturation temperature. The heat transfer coefficients are defined using the two resistance model with the Ranz Marshal correlation to estimate the Nusselt number of each phase.nCase S-2 and S-5 (which are both steady-state) have similar velocity vector diagram with more water-liquid volume fraction in the domain for Case S-5 compared to Case S-2.nHowever, for Case S-10 (transient case) the velocity becomes extremely high, I believe it doesn't converge.nPlease find the comparisonn of the three cases attached. Thank you.nDecember 1, 2020 at 1:53 pmRobForum ModeratorS10 looks to be seeing a max velocity of 300m/s so I'd check convergence carefully. You also tend to see poor mass balance on a transient if there is any pulsing in the flow field: you need to monitor what goes in, what leaves and what's inside the domain for these models. nS2 & S5 look OK, but check mesh resolution around the jet. Have you enough cells to resolve the full gradients? nDecember 3, 2020 at 10:21 pmTingWangUNOSubscriberBy resolving the velocity gradients you mean to get lower value of y+ value? right now it it ~220.nI believe the velocity gradients are resolved as the case S-2 gives good results. However, is it possible that the Case S-5, which has more heat flux at the wall and hence more condensation, is affected by the temperature in the domain and not the velocity gradients?nThank you.nDecember 4, 2020 at 10:46 amRobForum ModeratorGradients also occur away from the wall:y+ is a much abused term which is ONLY applicable for the near wall cell. It has no bearing on whether the boundary layer is resolved or the overall flow field is captured. Plot the results with node values off. If the result is more-or-less the same as with on then it's OK, if it's a very jumpy plot then you need more mesh. In the latter case I'd use adaption as I'm too lazy to remesh. nDecember 7, 2020 at 4:55 pmTingWangUNOSubscriberthank you for your response.nIncreasing the mesh and lowering the y+ in Case S-5 led to flow reversals at the outlet. Thus, I tried extending the outlet and ran a new case: Case S-21. Seeing the results do you thing this could be the issue and how could I compensate for it in Case S-5?nThe comparison of Cases S-5 and S-21 showed that Case S-21 has better convergence in terms of mass flow rate difference at inlet and outlet. Moreover, to make sure the gradients are resolved the plot comparing velocity inside the domain with node values and by turning off node values is shown in the plot below.nnDecember 7, 2020 at 5:04 pmTingWangUNOSubscriberDear ArraynI tried improving the mesh for Case S-5, but I get flow reversals at the outlet. Thus, I ran a new case S-21 that has the outlet extended. This was done to avoid any flow reversals. The results shows the Case S-21 had much better mass convergence for Case S-21 compared to Case S-5. Do you think that Case S-5 could be improved in any way?nAlso regarding the transient Case S-10 is it possible that at a transient time step the mass is not conserved as the simulation has not reached a steady-state? May be I could wait for it to reach steady-state?nI'm attaching the following belowComparison of domain and results for Case S-5 vs. Case S-21nComparison of vapor velocity plot with node values on and off. Could I say the gradients are converged? The contour plot do seem very similar.nI look forward to your suggestions. Thank you.nnnDecember 8, 2020 at 4:05 pmRobForum ModeratorI'd review the meshing. You need cells to pick up the jet, but why use a single mapped block? Pave and decomposition are very usable: the only people that use full mapped meshes tend to be looking at turbo machinery or didn't read any of the solver updates for 15-20 years. nDecember 8, 2020 at 6:05 pmTingWangUNOSubscriberThank you for the response Array. The current mesh has face split at planes to divide the domain. Is that still single mapped block?nI could use slide to decompose the mesh. However, in term of simulation results will it impact if I have a single mapped block or a decomposed mesh?nRight now the mesh size is ~ 15,000 elements. Any idea what I should increase it to?nThank you!nDecember 9, 2020 at 11:59 amRobForum ModeratorYes, if you look at the mesh you can see it concentrates to regions and doesn't expand in both directions. Making the domain with a few faces means you can choose the mesh type. nIn terms of cell count, it's not the total count that matters (within reason) but where you focus the resource. nDecember 14, 2020 at 6:17 pmDecember 15, 2020 at 10:31 amRobForum ModeratorAssuming the cell quality is good (I can't tell without the tools) that looks much better. You can see the benefits that you've clustered cells where you need them but not wasting cells where not much is happening. nViewing 12 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
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Difference between K-epsilon and K-omega Turbulence Model
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- Suppress Fluent to open with GUI while performing in journal file
- error: Received signal SIGSEGV
- Using GPU in FLUENT
© 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.