August 5, 2019 at 3:11 pmChris1opherSubscriber
I am simulating a laminar flow through a pipe in 2D.
I have convergence problems when I'm using a high density to viscosity ratio.
The fluid in my pipe is water at 80°C. The physical properties are density 1000 kg/m^3 and viscosity 1e-4.
The model converges when im using a higher viscosity of 5e-4.
It also converges when I'm using a lower density of 100 kg/m^3.
So my conclusion is that there is something with the ratio of density/viscosity.
Is there any link from that ratio to solving issues?
I am using the default settings for the solver.
Thank you in advance
August 5, 2019 at 3:31 pmRobAnsys Employee
What's the Reynolds Number in each scenario? Use the inlet velocity & pipe diameter to calculate it.
August 5, 2019 at 3:55 pmChris1opherSubscriber
My diameter is 10mm and the velocity is 0.0402m/s.
Re(density=1000, viscosity=1e-4) = 4020 (not converged)
Re(density=1000, viscosity=5e-4) = 804 (converged)
Re(density=100, viscosity=1e-4) = 402 (converged)
Is it a problem that the first combination is in the transition region to turbulence?
August 6, 2019 at 6:11 amChris1opherSubscriber
I just tried to run a simulation with density=1000 kg/m^3 and viscosity= 3e-4 kg/m^3 which leads to a reynoldsnumber of 1340 and this is not converging as well. Do you have any other idea?
August 6, 2019 at 1:10 pmRobAnsys Employee
At Re = 4020 it's not very laminar is it? At 1340 you may have some localised turbulence: plot contours of Residual -> mass imbalance and look for areas that are red & blue.
August 6, 2019 at 3:57 pmChris1opherSubscriber
Thank you for your advice.
I plotted the mass imbalance contour and attached the pictures. As reference i attached a picture of the model with viscosity 0.0005 which is converging.
Can you tell if that could be the reason my system is not converging?
Is an imbalance of e-08 to high?
Viscosity: 0.0003 Pa s
Viscosity: 0.0003 Pa s Zoom
Viscosity: 0.0005 Pa s
August 6, 2019 at 4:10 pmDrAmineAnsys EmployeeLack of resolution for flow which might turned to turbulent using zero model for turbulence. This might be an issue and leads to high mass imbalances. What happens if you turn turbulence midel on for high Reynolds case.
August 7, 2019 at 7:08 amChris1opherSubscriber
I tried using different pressure velocity coupling schemes. It is not converging for SIMPLE, SIMPLEC and PISO. When I use coupled it is working well.
I used SIMPLE for all of my previous simulations and I would rather not change my method. Do you have any idea why coupled is converging while all the other are not converging in this case?
I tried using the k-e-turbulence model and it is converging as well.
August 7, 2019 at 7:23 amDrAmineAnsys Employee
It is related to building up the stiffness matrix: central and neighborhood coefficients. Coupled is completely different to segregated approaches and is the default solver. It does converge quicker than other SIMPLE based solvers.
- 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.
- 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.