Learning Forum

[Chris1opher]

Hey all,

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

[Rob]

What's the Reynolds Number in each scenario? Use the inlet velocity & pipe diameter to calculate it. 

[Chris1opher]

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?

[Chris1opher]

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?

[Rob]

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. 

[Chris1opher]

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

 

 

 

 

 

[DrAmine]

Lack 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.

[Chris1opher]

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.

[DrAmine]

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.