

August 17, 2023 at 7:55 amyusuf uzunSubscriber
Hi,
I am trying to do CHT analysis of an exhaust manifold. Manifold geometry is not complex. I use polyhedral mesh and my mesh quality is sufficient. There is no sudden growth in cell size(i use grow rate 1.1). Some of my solver's setups are:Turbulence Model: SST kw. (mesh is adjusted to reach y+ value under to 1)
Coupled algorithm.
Gradient: GreenGauss Node Based
Pseudo Time Method : Off
Exhaust gas is defined as a ideal gas.
Back Pressure is defined to outlet.I have 3 inlet and 1 outlet.
I used hybrid initialization.
I started the analysis with first order and then switched second order(In the first order part, the analysis was converged and variables that i controlled were stabil.).
I iterated with decrease the courant number periodically.(from 200 to 1)
After switching to second order scheme residuals and variables started to fluctuate and fluctuation did not finish.What is the reason of fluctuation?
What is solution for convergence and stabilization?I added residuals and variables plots.

August 17, 2023 at 7:58 amyusuf uzunSubscriber
Journal that i used:
rc manifold.cas.h5
#
/solve/monitors/residual/convergencecriteria 1e4 1e3 1e3 1e3 1e6 1e3 1e3
#
/solve/set/pvcontrols 200 0.5 0.5
#
/solve/set/discretizationscheme/pressure 10
/solve/set/discretizationscheme mom 0
/solve/set/discretizationscheme omega 0
/solve/set/discretizationscheme k 0
/solve/set/discretizationscheme temperature 0
/solve/set/discretizationscheme density 0
#
/solve/initialize/hyb
#######################################################################
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#
/solve/set/pvcontrols 100 0.5 0.5
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#######################################################################
/solve/set/discretizationscheme/pressure 12
/solve/set/discretizationscheme mom 1
/solve/set/discretizationscheme omega 1
/solve/set/discretizationscheme k 1
/solve/set/discretizationscheme temperature 1
/solve/set/discretizationscheme density 1
#######################################################################
/solve/set/pvcontrols 200 0.5 0.5
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#######################################################################
/solve/set/pvcontrols 150 0.5 0.5
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#######################################################################
/solve/set/pvcontrols 100 0.5 0.5
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#######################################################################
/solve/set/pvcontrols 50 0.5 0.5
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#######################################################################
/solve/set/pvcontrols 20 0.5 0.5
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#######################################################################
/solve/set/pvcontrols 10 0.5 0.5
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#######################################################################
/solve/set/pvcontrols 5 0.5 0.5
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#######################################################################
/solve/set/pvcontrols 1 0.5 0.5
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#
/solve/iterate 200
y
#
wcd manifold_out.cas.h5
y
#######################################################################
exit
yes 
August 17, 2023 at 8:05 amSRPAnsys Employee
Hi,
I suggest to check mesh created. For that I suggest to check exhaust manifold tutorial, which guide you for meshing Chapter 1: Fluid Flow in an Exhaust Manifold (ansys.com)
Chapter 2: Fluent Postprocessing : Exhaust Manifold (ansys.com)
Hope you find this useful.

August 17, 2023 at 8:31 amyusuf uzunSubscriber
Thanks for the answer. I think there is no problem on mesh. Width of geometry approximately 46 centimeter and there are 7,000,000 cells. Mesh quality and resolution is good enough i think.

August 17, 2023 at 2:44 pmNickFLSubscriber
Sorry ignore what I wrote below. For some reason I thought it was a transient simulation. Maybe plot contours of the residuals to see where it is not converging. Could there be some inherent unsteadiness in the solution, such as vortex shedding? Also, in my experience, mesh quality can be a cause for a solution failing when moving from first order to second order. The numerical dissipation of first order meshes sometimes overcome mesh quality problems, whereas the second order discretization will amplify it. Also consider moving to the segregated solver and see if you get better convergence there.
You are plotting those each iteration. If instead you plotted those per time step those spike will smooth out. If you plot every iteration the plot will be corrupted by intermediate “incorrect” solutions.Trying to look at the last iteration per timestep in your plots, I can imagine some sort of convergence to a fixed value.
August 23, 2023 at 1:31 pmyusuf uzunSubscriber
I tried to use Simple algorithm as a solver but it didn't work. Then i changed turbulence model to ke realizable with Enhanced Wall Treatment. With this change residuals converged and selected variables became stabil. What is the reason of that?
Also, in the end of two simulations, results show that:
I think there is a big difference. I don't know it is true to compare that way but fluctuations occur around particular value.

August 25, 2023 at 4:38 amNickFLSubscriber
What do you mean the SIMPLE did not work? Did it diverge on you?
What you seem to be experiencing is poor convergence and when you add "extra" dissipation it converges. Granted, this is simply based upon what you have posted here. Back in your post from August 17th, you wrote "is good enough i think". These are words that have led many (including myself) astray. If I were you, I would create a region that identifies the poor quality cells. To do this, rightclick on Cell Registers and select New>Field Value Variable. Change the type to "Cells Less than" and then pick Ortho Quality under the Mesh variables. A good starting point would be to pick cells with less than 0.05 and select Save/Display. How many bad elements are there, and where are they located? From here there are two approaches. One would be to Refine the mesh in these areas, the other approach would be to use Poor mesh numerics (which basically runs 1st order upwind solver on these cells). To do either of these simply rightclick on the created Register in the tree.
I would not necessarily trust either of the solutions obtained from the above approach, but it would help to identify problem areas.

September 11, 2023 at 6:33 amyusuf uzunSubscriber
Thanks for the answer. When I say "simple algorithm didn't work," I mean it has resulted in like previous analysis. It has not converged, fluctuations still continue like picture that i attached below.
I follow your suggestion and checked my poor quality meshes. It is clear until 0.16 orthogonal quality(attached picture). Also this is my skewness measure:
name id cells (quality > 0.90) maximum quality cell count
    
Overall Summary none 0 0.831676 8694808Total Number of Cell Zones : 16
[Quality Measure : Skewness]



 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.
Ansys Blog
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.
 Floating point exception in Fluent
 What are the differences between CFX and Fluent?
 Heat transfer coefficient
 Difference between Kepsilon and Komega Turbulence Model
 Getting graph and tabular data from result in workbench mechanical
 The solver failed with a nonzero exit code of : 2
 Suppress Fluent to open with GUI while performing in journal file
 Mesh Interfaces in ANSYS FLUENT
 Time Step Size and Courant Number
 error: Received signal SIGSEGV

7742

4502

2961

1449

1322
© 2023 Copyright ANSYS, Inc. All rights reserved.