[CFDJonas]

Hello CFD Online!

I'm currently trying to model a quite simple problem: a double-piped (laminar) flow. For this, I created a 2D axisymmetric rectangular mesh to model the inside of a normal pipe. The pipe or tube is quite long and has a small diameter (very high L/d ratio).

The annular gap of the double pipe is used for heating. One assumption is, that the heating stream is isotherm and the heat transfer coefficient along the tube axis is constant. Thus, for the modeled 2D mesh I chose for the thermal boundary condition of the wall "convective" and entered the constant heat transfer coefficient and the temperature of the heating agent.

Now to my problem regarding this model: By calculating the reynolds number I am definetely in the laminar regime (around 1200). Therefore my idea was to use the laminar viscosity model. However, this leads into divergence quite fast.

On the other hand, when I use the k-omega model (standard or SST) the simulation converges quite easily.

Do you have an explanation for this observation? Is the idea of choosing the laminar model not suitable when I introduce radial temperature gradients? Can I believe the results of the k-omega model or should I use another turbulence model for this kind of situation?

Thanks in advance!

Edit:
Added a sketch of the model situtation in the attachment (the length of the pipe is in reality much longer):

Edit2:
Added a (segment of) contour plot of the temperature... A diverged simulation with the laminar viscosity model is shown. The temperature inhibits these oscillating "regions" as seen in the picture.

[LoGaL]

Basically the ultimate effect of any RANS model is to add additional viscosity, which, coincidentally, can, sometimes, stabilize the simulation.. so long story short, in my experience, laminar viscosity model (i.e. bare bones navier stokes) can be less forgiving than RANS…
Maybe the mesh is bad, maybe you need more robust settings… hard to say

[CFDJonas]

Originally Posted by LoGaL

Basically the ultimate effect of any RANS model is to add additional viscosity, which, coincidentally, can, sometimes, stabilize the simulation.. so long story short, in my experience, laminar viscosity model (i.e. bare bones navier stokes) can be less forgiving than RANS…
Maybe the mesh is bad, maybe you need more robust settings… hard to say

Thank you for your answer!
That makes sense, that the turbulences introduce "stabilizing" effects.

I just thought that the case described is actually a kind of standard problem. I am thinking, for example, of heat exchangers. Of course, these tend to be operated turbulently in order to generate a higher exchange rate, but there must surely have been someone who looked at this laminarly.

Regarding the mesh: I tried several steps of reducing the cell size, with no real success. Furthermore - correct me if I'm wrong - my literature research shows that I should actually need a less fine mesh for laminar flow than for turbulent flow. What are some rule of thumbs for generating a mesh with laminar flow and/or radial temperature gradients.

What do you mean with more robust settings? I played a little bit with the Under-Relaxation Factors, but this just tends to push the problem to a later point in simulation. And at this point it is important to say that the described problem should only be the beginning. I don't want to come to solution with a crowbar, because later on, among other things, chemical kinetics should also be added.

Thanks again!

[LoGaL]

It is a standard problem, no worries..

Concerning the mesh, it's not a matter of element size, but rather, of element quality.. Can you show me a picture of the mesh? Als, you can run some mesh check in ansys fluent...

For what concerns the settings, for example, are you using SIMPLE or Coupled method? the latter is more robust.

[CFDJonas]

Originally Posted by LoGaL

It is a standard problem, no worries..

Concerning the mesh, it's not a matter of element size, but rather, of element quality.. Can you show me a picture of the mesh? Als, you can run some mesh check in ansys fluent...

For what concerns the settings, for example, are you using SIMPLE or Coupled method? the latter is more robust.

Regarding the element quality: In this kind of mesh I am even able to generate a structured mesh. So I should have a perfect orthogonal quality. The aspect ratio should also be not too bad (only for inflation layers, of course). But the main flow is still in axial direction.

I have tried several different settings. Currently I use the multizone method and a global element size. Additionally I tried the simulation with and without inflation layers. I added a picture of one of my meshs in the attachments with the use of inflation layers. But with my understanding the laminar simulation not get worse when I add inflation layers, but the turbulent simulation needs inflation layers. So I went with them.

Currently I'm using SIMPLE. I have switched the method a little time ago, but I am not quite sure in which setting exactly. I will run a simulation with coupled and laminar right now, and may edit this post with the result.

Edit: I ran a simulation with the coupled solver. It does not diverge directly, but delivers really instable residuals (does not converge either). Furthermore I keep having reversed flow at the outlet. I added a screenshot of the residuals. I only solve for the flow field and energy equation.

I should add that I put in a laminar velocity profile as an inlet. To get this profile I simulate the same geometry with the laminar model under adiabatic conditions with a mass-flow inlet (I know the mass stream). Then I write the boundary profile at the outlet and use the axial and radial velocity as an inlet condition for the successive simulation with turned on heat-transfer. I hope this is not a completely wrong way of thinking. Thanks again.

[LoGaL]

If anything, laminar simulations need inflation layers more than RANS simulations, because you need to resolve the BL. WHat is going on with the inflation layer near the wall? I see first small element, then larger one, then small again.. Just don't assume hexa mesh = good quality. Do this check

[CFDJonas]

Originally Posted by LoGaL

If anything, laminar simulations need inflation layers more than RANS simulations, because you need to resolve the BL. WHat is going on with the inflation layer near the wall? I see first small element, then larger one, then small again.. Just don't assume hexa mesh = good quality. Do this check

I think this was due to a bad screenshot, sorry. I attached a zoomed in version of the inflation layer. It is definetely "growing".
I know to estimate the inflation layers when using turbulence by calculating the y+ value. How do I estimate the needed thickness for laminar models? How do you rate the "size" of the inflation layers in my mesh? Do you think this is already quite fine or really coarse?

Thank you very much!

PS: I added the results in the post above and added additional information.

[LoGaL]

I read now the thing of the laminar profile...The idea is not wrong. I am not sure however if you are implementing it right, or if you are messing up something. Hard to say, without troubleshooting directly your setup (and I won't do it xD).

Try first not to impose the profile and just give mass flow rate, and see if the simulation converges. You may even think to split the tube in two parts, one you apply adiabatic, one you apply heat transfer BC.

If the simulation does converge, then you messed up with the profile. The point is that you started with a maybe too complicated approach, and now you don't know who's producing the error

[LuckyTran]

As far as gridding goes, pretend you are doing a DNS (because you are when it is laminar). y+ can be estimated using the same philosophy as turbulent flows, the difference is your boundary layer thickness should be estimated using laminar solutions / correlations rather than turbulent ones. Laminar boundary layers are thinner than turbulent ones...

Debugging a laminar mesh can be as simple as making a uniformly fine grid. It's doable for laminar cases because the Reynolds number is low.

The other thing to check for is initial conditions. Your solution stability is highly dependent on the initialization. Lowering urf's or Courant number if you're using any of the coupled approaches can help stabilize a solver when you give it a really bad initial guess but can also reveal that it is a problem with the initial guess. You can crank up the urf's after this initial transient.