## Fluids

#### Cell reynolds number and type of flow

• Aboma Wagari Gebisa
Subscriber

Hi there,

I have a very complex fluid volume that I cannot calculate the reynolds number to check if the flow is laminar or turbulent. So I run the simulation selecting laminar flow but it didn't converge. I then changed the flow to turbulent k-e and it converged. However, when I check the cell reynolds number it is around 300. Does this value tell us that the flow is not turbulent bul laminar? or it doesn't have anything to do with the type of flow?

For a complex fluid volume (picture below), is it acceptable to assume turbulent flow?

• Steve
Ansys Employee

While it is typical that most industrial flows will be turbulent, there are applications which may be laminar, e.g. low velocity through a small geometry with highly viscous fluid. A good starting point is to calculate the Reynolds number at inlet and outlet (based on the diameter and the nominal flowspeed).

If you have limited exposure to the concepts of turbulence, there's some great Ansys Innovation Courses you can access on the Ansys Innovation Space, such as the Basics of Turbulent Flows.

• Rob
Ansys Employee

You might want to check the manual to understand what Cell Reynolds Number is: a tip, it's not overly useful.

From an engineering point of view, what is the Reynolds Number at various locations in the domain? Treat the Fluent result as you would an experiment and post your findings here.

• Aboma Wagari Gebisa
Subscriber

@steve and Rob

Thank you very much for your responses.

I already calculated the reynolds number at the inlet and outlet, they are small values around 15. It means that the flow is laminar. What I was wondering is regarding the complexity of the fluid volume.

I ran the simulation with laminar flow by refining the mesh and applying inflation layers. The velocity residuals converge but the continuity residual is not converging.  The continuity residual can't go below e-2. I also monitor volume flow rate at the outlet. It shows relative stability but it is not perfectly straight.

Do you have any suggestion on how to get the solution converge?

• Steve
Ansys Employee

Wow - that's a low reynolds!

Oscillating convergence plots: you may be able to solicit lots of ideas on this.

Your outlet is a short pipe following a complex geometry arrangement which means the flow is unlikely to be fully established and therefore liable to some flctuation at that surface. One trick is sometimes to artificially extend the outlet a little further downstream where the flow might be more established (and therefore settled).

• Rob
Ansys Employee

Have a look in the Learning courses, there are a couple on flow. Then have a look for laminar eddies. Finally, in the laminar model use a few point monitors to get the local velocity values in areas of interest in your model. I suspect the flow is slightly time dependent, and the monitors will help to judge if the solution is changing by enough to alter the results.

• Aboma Wagari Gebisa
Subscriber

Hi Steve,

I already extended the outlet further down as shown below based on different suggestions in this forum. But continuity is still not converging.

There is reversed flow on faces in the outlet in first 150 iterations even after moving the outlet further down.  Could that still be  a cuase for the reversed flow? The reversed flow goes away and appears one in a while after 700 iterations.  .

• Steve
Ansys Employee

Certainly, reversed flow can easily contribute to instability; ideally we would position the outlet suitably downstream to a location where we do not observe reversed flow (i.e. achieving fully developed flow). The pathway (and angular momentum change) through the device is likely to establish eddies which will take time to dissipate. You will often see advice on extending the outlet by x-lengthscales, e.g. 5-10 diameters, but these are only guidelines; you may find you need more or less. It may also be fundamentally transient, but at such low-Re I would hope that viscous effects will help to stabilise the flow. Instabilities (transient-like) can also be triggered by numerical effects, e.g. mesh resolution or quality upstream.

But fundamentally determine if you're satisfied with the overall mass balance and whether the flow is suitably stable (with iterations) in the areas of interest where you are investigating behaviour - that's the essence of the advice from Rob; if the instabilities are primarily downstream of your area of interest they may not be influencing your result.