July 11, 2019 at 2:37 amHHK1992Subscriber
I am trying to simulate the flow of air past an airfoil. The settings are,
steady state, ideal gas, SST k-omega, far-field pressure boundary, coupled solver with pseudo-transient option
The difference is that I have several patches on the airfoil surface and each forms a wall boundary as shown in Figure 1 (which I created for additional studies later on).
The drag and lift coefficients are showing good agreement with experiment results from the literature (less than 5%).
But I get wiggles in the plots of wall shear stress, turbulent KE, etc as shown in Figure 2.
So I removed all patches and made the airfoil a single wall boundary which gives no wiggles!
I rechecked the mesh which I created in ICEM CFD (structured, in Figure 3) but I don't find any problems in it.
Can someone please tell me why this happens?
Thanks in advance.
July 11, 2019 at 11:10 amDrAmineAnsys Employee
Several walls will imply a sort of discontinuity. Can you check the values without node values?
But now without separate walls it is working as it should as you have noticed.
July 11, 2019 at 12:37 pmHHK1992Subscriber
Thank you for the comment.
In fact, I checked it already and it does not make any difference in the situation.
I coarsened the mesh with all the wall boundaries and the wiggles seem to be disappearing. A fine mesh leads to wiggles.
Though I found that the splitting leads to wiggles, it does not fully convince me. I think with or without the splits, Fluent should give a smooth curve.
Please tell me if you have any more suggestions/ideas.
July 11, 2019 at 4:36 pmDrAmineAnsys EmployeeIf there is non continuous mesh pattern along the walls then a numerical noise might occur.
Which numerical methods have been used here? Show a near view of mesh transition between the walls colored by cell volume change
July 11, 2019 at 4:37 pmRobAnsys Employee
Can you replot using curve length rather than position on the x-axis? Also look at the pressure plot on the same line.
What does the convergence monitor plot look like?
July 12, 2019 at 3:12 amHHK1992Subscriber
The solution methods are shown in Fig1.
The cell volume change close to the airfoil surface is shown in Fig2
I already tried that but, No changes in the plot.
Fig below shows the convergence plot of cd and cl.
Thanks to both of you for taking interest and trying to help me with this.
July 12, 2019 at 5:54 amDrAmineAnsys Employee
Show a near view of mesh transition between the walls colored by cell volume change and not cell volume. That would tell us the jump in the cell size along the walls.
July 12, 2019 at 7:49 am
July 12, 2019 at 9:56 amRobAnsys Employee
That looks OK. How does the y+ value vary along the wall? Any oscillations in the residuals (continuity etc)?
July 12, 2019 at 10:44 amHHK1992Subscriber
Yes, there are oscillations in Y+, Tke, etc. as well.
There were no oscillations in the residuals.
July 12, 2019 at 10:46 amDrAmineAnsys Employee
So the near wall treatment might be the root of the wiggles.
Just for consistency can you run EWT and RKE model (not really my favorite) to see if the behavior is the same.
July 13, 2019 at 6:22 amHHK1992Subscriber
I already checked Enhanced and realizable K-epsilon models.
But no luck!
To my surprise, this even happens in the laminar flow!
July 15, 2019 at 7:04 amHHK1992Subscriber
I found the solution to the problem. It is nothing related to models in the Fluent. It starts with ICEM CFD.
Previously my procedure was,
1.Import airfoil curve to ICEM CFD from modeling software.
2. Create splits (patches) in the curve in ICEM CFD
3.Create mesh and go to Fluent simulation
Out of curiosity, I adopted the following procedure,
1.Create airfoil curve as well as splits in geometry modeling software
2.Import it to ICEM CFD
3. Create mesh and go to Fluent simulation.
And it worked! There are no wiggles! (See Fig).
I don't why it happens. Maybe splitting in ICEM CFD might have created some micro-level issues. I believe ICEM CFD is primarily a mesh generator. I should stop doing too many geometry operations in it.
Thank you so much to both of you for helping me with this problem.
July 15, 2019 at 7:31 amDrAmineAnsys Employee
Great that you fixed the issue!
July 15, 2019 at 7:32 amDrAmineAnsys Employee
Perhaps something to do with the assignment of the curves to the edge and snapping vertices? As you now fixed the issue please mark this as is Solved.
- 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.