[JohnPuentes]

Hi everyone,

I am working on a flow problem that deals with Re numbers lower than 1. I am modeling a resin flowing through a porous medium at a very low speed, 0.4m/min (0.00667 m/s), with high viscosity values (1.5 Pa-s to 10000 Pa-s), in a rectangular profile (Dh= 0.008 m). Any combination of conditions gives Re numbers lower than 1 or at most 1.

It is the sample process that l.ts was working on in 2012 (Pultrusion, see link below), and it is similar to that in 2005 by Taner.

http://www.cfd-online.com/Forums/cfx...-variable.html

http://www.cfd-online.com/Forums/cfx...-flow-cfx.html

Does any one know if CFX has a Stokes solver or the possibility to neglect the inertia terms from the Navier Stokes equation? Does CFX has a limit in what is lowest Re that can be solved? Will Fluent be more suitable for this task?

I already know how to setup my problem in CFX, but I am concerned about the solver crashing due to creeping flow (Stokes flow).


Thanks

[flotus1]

I dont see any reason why CFX would be unable to solve low Reynolds number flow.
Convergence may be slow though, but the solution should be stable.

I cant think of a way to neglect inertia terms in CFX, but since you are dealing with Reynolds numbers much higher than zero, you should not neglect them anyway.

[JohnPuentes]

Thank you Alex for the update. In my problem, inertia is always negligible because Re numbers are always lower than one.

I am concerned about convergence, because these type of problems are normally solved in a Stokes flow solver. As some posts mentioned before, CFX may crashed for such low Re numbers, but I agree, for a steady state-creeping flow, the problem should be easier to solve.

Here is the post about creeping flow being a problem:

http://www.cfd-online.com/Forums/cfx...-variable.html

Here is another post about creeping flow not beign an issue in CFX:

http://www.cfd-online.com/Forums/cfx...-flow-cfx.html

any thoughts on this?

[flotus1]

A Reynolds number lower than one does not mean that inertia terms are negligible.
But I agree that for most combinations of your parameters the Reynolds number is low enough to make this simplification.
And for such REALLY low Reynolds numbers CFX may not be the best tool.

I have no experience with Stokes solvers though, so any experts on this are welcome to contribute.

[ghorrocks]

CFX cannot ignore the inertia terms as it is a Navier Stokes solver. Fluent is as well.

CFX does have convergence problems with VERY small Reynolds numbers. Do a sensitivity study to check that it is behaving itself.

But if your flow is truly Stokes flow then you should either get Stokes equation software, use a general PDE solver to model it or write your own. No commercial software that I am aware of can do it.

[JohnPuentes]

Thanks Glenn. I am working on a sensitivity analysis. I will update everyone whether or not CFX works for my model.

[JohnPuentes]

Glenn and Alex,

I was able to run a basic model without any issues. I think that the laminar flow option of CFX can handle very low Re numbers, but it is important to limit the highest value of the viscosity. I am still trying to validate my results with lab values.

My issue now is that I am working on a flow problem that involves a moving domain. My domain is a porous medium moving at a constant speed that transports a fluid through a tapered channel. When I activate the solid motion option in CFX, I only get realistic results with limited option of boundary conditions.

I can only use open-inlet and open-outlet or static pressure at the outlet. Everytime I try to add a velocity or mass-flow rate at the outlet, I obtain nonsense results or the model does not converge.

Also, when I couple heat transfer to the problem, the energy equation only reaches a residual convergence of 10^-3, which is pretty high. I tried several combinations of boundaries, Tinlet-Toutlet, Open inlet-heat transfer outlet, Open inlet- adiabatic outlet. None of them converged.

I do not want to add a moving mesh to my problem, because the problem itself is already very complex. I think that adding a velocity field (with the solid motion option) is a good simplification for my model, but I haven't found more information dealing with boundary conditions for flow in the case of a moving domain. There is some info for the boundaries in the energy equation, but not much for flow.

Does anyone know if these two boundaries, velocity and mass flow rate, need a special treatment for a domain in motion? Any ideas about my issue with the energy convergence?

Thanks a lot

[ghorrocks]

Can you post an image of what you are modelling and your output file?

[JohnPuentes]

Here is some info about my model.

File 1

This is the geometry (the length is 100 times the thickness). My case study can be approximated to 2D and steady-state. The porous domain is moving with at a costant speed. The fluid is dragged through the tapered channel by the motion of the solid. I added an open-inlet since the flow tends to be squeezed out of the domain at the entrance, and a static pressure at the outlet. The wall has a not slip condition and there is symmetry in the center of the geometry. I am only modeling half of the domain.

File 2

This file includes heat transfer conditions. Tinlet, Twall and heat transfer between the fluid, solid and the room.

File 3

This is the cfx output file.

File 4

This is the pressure profile obtained. This agrees with several authors who show how there is a build up pressure in the tapered channel. I am interested in finding the pressure build up in the system.

Thanks

[ghorrocks]

I do not understand exactly what you are trying to model. What have you applied the solid motion of U=Pulspeed to? How have you done this? What is driving the flow as you inlet and outlets are both zero pressure?

You mentioned moving mesh - you cannot use moving mesh in a steady state simulation.

[JohnPuentes]

Glenn

The flow is driven by the motion of the solid. I applied the Pulspeed (0.3m/min) to the entire domain (see the attached picture). I consulted the solver theory manual and it says this:

'' You can model the motion of a solid that moves relative to its reference frame by selecting the Solid Motion option and specifying a velocity. Examples of such motions include: A material being continuously extruded.
The solid motion model does not involve changing the mesh. Instead, motion of the solid is simulated by imposing a velocity field in the solid domain. The velocity field causes the advection of energy and Additional Variables as applicable.''

My problem is that if I add a velocity at the outlet or mass flow rate at the outlet, I get nonsense results or the simulation does not converge.
When I add heat transfer my simulation does not converge with any combination of boundary conditions.

I knew about the restriction with the moving mesh, so I decided to use solid motion instead. In my experiment, the domain (fibers) that are impregnated with the fluid (epoxy) are being pulled through the channel at a constant speed. This causes the resin and the fibers to travel through the domain.

I found a link of a short video that shows the process:

https://www.youtube.com/watch?v=sxWtzlitq1A

I hope this clarifies my model somehow. Any thoughts?

[Opaque]

From the following quote, it is not clear what is the inlet/outlet boundary condition pair.

My problem is that if I add a velocity at the outlet or mass flow rate at the outlet, I get nonsense results or the simulation does not converge.
When I add heat transfer my simulation does not converge with any combination of boundary conditions.

If you have an inlet/outlet boundary condition pair that does not include pressure on either end, the problem is not well specified which may lead to what you call garbage solutions.

For example, if you take the "catalytic converter tutorial" provided in the installation, and you add solid motion to the porous domain, does it work ? Does the heat transfer solution converge ? What ANSYS CFX release version are you using ?

Hope the above helps,

[JohnPuentes]

Thanks for the info Opaque. I am going to add motion to the tutorial to see if it works. That can give me some insight into my boundary conditions problem.

To clarify the inlet/ outlet pair, these are the combinations that I have tried so far:

Open inlet (entrapment) / static pressure=0 outlet. Only solid motion drives the flow.
Open inlet (entrapment)/ velocity outlet= constant. This creates a conflict with the velocity of the solid.
Open inlet (entrapment)/ mass flow rate outlet= constant. This case does not converge.

I tried all the above cases with static pressure at the inlet, but since the fluid is been squeezed out of the system, this inlet option is very unstable.

[Opaque]

You should be using Total Pressure inlet instead of static pressure. The modeling guidelines warn about the issues of using static pressure inlet.

[JohnPuentes]

Originally Posted by Opaque

For example, if you take the "catalytic converter tutorial" provided in the installation, and you add solid motion to the porous domain, does it work ? Does the heat transfer solution converge ? What ANSYS CFX release version are you using ?

Hope the above helps,

I ran the catalytic converter tutorial, adding solid motion (0.005 m/s) in the z-direction (direction of the flow), and I obtained the same convergence problem that I have in my model. The model does run, but in order for the temperature residuals to go down to at least 1e-4, it is necessary to run the model for a very long time (the simulation time grows exponentially). Perhaps, without solid motion, it takes 100 iterations to converge, on the other hand, with solid motion, it did not converged after 1000 iterations.

Any ideas why this convergence problem happens with the energy equation when adding solid motion in a domain?

Does anyone know if I need to add the same velocity of the solid domain to any surface that is selected as wall?

[Opaque]

Are you solving the problem in steady state ? If so, what timescale is being used for the energy equation in the solid part of the porous domain.

The timescales in the solid and fluid are usually very different, and if you run with the fluid timescale for both fluid and solid phase, it will take the age of the universe to converge. Check that the solid timescale is a lot (4 -> 6 order of magnitude) larger.

[JohnPuentes]

Opaque,

yes, I am running my model in steady-state. This is my first time simultaneously solving energy for a fluid and a solid. Where do you modify/control this parameter in CFX? Should I look at the solver options? That would be great if you can tell me where to find more info about this parameter.

Thanks

[ghorrocks]

Have you seen this in the CFX documentation? Have you done as it recommends?

On an external boundary, if the solid has a velocity component normal to the surface, then consider activating the advection term(s) on the boundary condition for that surface, by visiting the Boundary Detailstab and selecting Solid Motion > Boundary Advection. For details on setting up boundary advection on a wall, see Solid Motion: Wall.

[JohnPuentes]

Glenn and Opaque

yes, I activated boundary advection in all my runs, and I also followed all the rules for walls in solid motion. Still, as opaque mentioned, looking at the convergence for the two energy equations (one for the liquid and one for the solid), one converges very quickly (couple of minutes), while the other does not converge after 1 or 2 days of running the model.

I am now checking about this discrepancy between timescale for a solid and a fluid while running a steady state simulation. My two questions are how to identify in the results which energy convergence belongs to the fluid and which one belongs to the solid. There is T-energy and H-energy, but I am not sure which one is the solid.

My last question is how to setup the timescale for the fluid and for the solid. Looking at the timescale of my results H-energy has a value of 2e-4, while the time scale of T-energy is 100. I am not sure is that difference is enough, since I always choose the automatic time scale in the solver options. Maybe I have to manipulate that parameter myself.

Running the catalytic converter tutorial T-energy does not converge (I assume this is the solid since the timescale is 100) and H converges quickly (fluid with timescale 2e-4).
The opposite happens in my model, T-energy converges (timescale 100) and H does not converges (timescale 2e-4). Any thoughts?


Thanks

[ghorrocks]

H-energy is the fluid, T-energy is the solid.

The term you are looking for is "solid time scale factor". This accelerates the time scale in the solid domain and can greatly speed convergence. As the thermal equation in a solid is a very stable one in general you can accelerate this quite a lot usually - factors of 100 or 1000 are common, sometimes even more.

Oh - I see the solid converges and the fluid does not. In that case I would write the residuals to the output file and have a look at them in the post processor. Try to identify a region or reason for the poor convergence. It usually is a small region of very high residuals.