Setting up a porous medium

Omerta · January 21, 2012, 16:38

I'm working on a design for one of my projects in university. Its a duct for a tidal turbine.

To simulate the turbines presence in the duct, I wanted to use a porous medium in the center to replicate the rotor. But I am having a hard time setting that center area as just the porous medium. I embedded a cylinder in my CAD drawing so now there are two bodies. But I do not know how to define the interaction between them in the simulation.

Could somebody send me in the right direction of where to start looking? Thanks

ghorrocks · January 22, 2012, 07:32

Use a momentum source term to do this. They are move general and you can apply a resistance to the flow in any form you like that way.

And the source term can be applied as either a volume or a surface the flow passes through (eg an interface).

Omerta · January 22, 2012, 13:35

ok, my prof recommended a porous medium over a momentum source... but you are right it should work fine.

Any suggestions on setting up the cylinder in the center? I cannot get them to interact well with eachother. It wants me to define the cylinder's surface as a wall or outlet etc. Should I stick with opening?

ghorrocks · January 22, 2012, 18:56

If you like you can use the porous flow equations in your region. But because your region is a turbine and not a porous region then I cannot imagine why you would want to. A general momentum source can be written which has the performance curve of the turbine you are using - you cannot do this with porous regions and it is far more accurate.

Assuming you are applying this as a 3D region, then select both the fluid volume and the turbine volume as the domain. Then you make the turbine region a sub-domain and apply the source term (or porous region if I am not convincing enough). No need for inlets or outlets. Also make sure the mesh is continguous between both regions.

Omerta · January 23, 2012, 02:21

Hmm, for some reason, it will not allow me to define the turbine region as a subdomain. Is that because it is a boundary region? Should I leave the CAD model as 2 bodies, with the second being the rotor and overlapping the fluid region around the shroud?

ghorrocks · January 23, 2012, 06:42

A subdomain is a 3D region. A boundary is a 2D surface on the outside of a 3D region.

Omerta · January 23, 2012, 10:48

Yes, but it will not allow me to select it as a subdomain because I subtracted the cylinder from the rest of the model.

When I didn't combine them it seemed to get confused on the interaction between the bodies

ghorrocks · January 23, 2012, 17:39

You need to decide what approach you are going to use. If you remove the region then you use a inlet/outlet pair to produce the flow. While this is simple it does make it hard to link to a fan characteristic curve. You can leave the region in and apply the fan as a momentum source. This is a little trickier as you have to do some extra meshing operations and define the momentum source term but is a better approach for most applications.

Omerta · January 25, 2012, 23:35

Hmm, I'm trying it with two bodies and using a momentum source. But, I've never sucessfully done a simulation with two bodies and am getting this error:

Quote:

+--------------------------------------------------------------------+
| Checking for Isolated Fluid Regions |
+--------------------------------------------------------------------+

2 isolated fluid regions were found in domain Default Domain

If the isolated regions do not have the pressure level set either
by the boundary conditions or using a reference pressure equation,
you may encounter severe robustness problems.

This situation may have arisen because a domain interface was not
properly defined during problem setup. Please carefully check
the setup.

The solver will stop now and write a results file. The isolated
regions can be visualised in CFX Post by making plots of the
variable "Isolated Volumes".

If you are sure that the pressure level is set in each isolated
fluid region then you can force the solver to turn off this check
by setting the expert parameter "check isolated regions = f".

Probably a basic mistake

Omerta · January 26, 2012, 00:56

Quote:

Originally Posted by Omerta

Hmm, I'm trying it with two bodies and using a momentum source. But, I've never sucessfully done a simulation with two bodies and am getting this error:

Probably a basic mistake

I can't figure out how to tie the two regions together in CFX-Pre.

When I set a domain interface, it one let me select the end of the main body. Only the cylinder itself. Do I need to separate them and make a void in my CAD software? Because I think they are overlapping in the CAD software.

ghorrocks · January 26, 2012, 06:59

You need to define an interface to connect them with your current mesh. It can be a bit tricky selecting the correct surfaces but if you hide and unhide the bodies you can do it.

But a better approach is to remesh and make the common surface have a matching mesh. Then you will have no need for an interface.

Omerta · January 26, 2012, 20:01

Finally got that to work.

I had to separate my model again, making a void for the cylinder, then placing one as a second body inside of it.

Placed connections in CFX-Pre for their contact, and then the domain interfaces.

The subdomain is set as a -10 kg/m^2 in the Z component (against flow).

I'm having problems with divergence of the solution now, at about 25-40 iterations my KTurbKE starts to oscillate.

Any hints on how to keep that under control? What should I look into modifying?

ghorrocks · January 26, 2012, 20:09

Good progress.

You will probably need a source term linearisation coefficient. Read the documentation about source terms for this, but if you have defined a constant source then I think that goes to zero anyway so will not help.

Be careful with constant source terms - that means you are always adding momentum there, regardless of the flow conditions. It is better to define a fan curve.

It is also better to not require the domain interfaces. Try to mesh it with contiguous meshes so you do not need the interface. If you do not know how to do this then do some meshing tutorials.

But for your current convergence issues I would not worry about the turbulence equations too much yet. Get the pressure & momentum equations converging before you worry about the turbulence eqns.

Omerta · January 26, 2012, 20:20

I just used a constant because I wanted to get a solution to work, I will add a fan curve as I make more progress.

The turbulence equation stated oscillating and I was assuming that it threw off the rest of the solution as it had started then the pressure and momentum were soon to follow.

I'm using Ansys meshing and the tutorials suck for it. Its very difficult to have defined control over what is going on. But I'll see what I can dig up.

ghorrocks · January 26, 2012, 20:31

Let me give you a tip on the meshing - you need to define the two bodies as a single part and the interface surfaces will get a contiguous mesh. Look up multi-body parts in the tutorials or doco.

Your convergence problem probably just needs the normal approach - smaller timesteps, better initial conditions, better quality mesh.

Omerta · January 27, 2012, 11:04

Thanks, got it to converge now, with setting the timestep (forgot I reset all the data on Workbench) and high res turbulence.

Now to figure out that pump curve.

Omerta · January 28, 2012, 18:09

Quote:

Originally Posted by ghorrocks

Let me give you a tip on the meshing - you need to define the two bodies as a single part and the interface surfaces will get a contiguous mesh. Look up multi-body parts in the tutorials or doco.

Your convergence problem probably just needs the normal approach - smaller timesteps, better initial conditions, better quality mesh.

I can't find any tutorials that use a momentum source. Any names of them come to the top of your head?

January 22, 2012, 18:56		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	If you like you can use the porous flow equations in your region. But because your region is a turbine and not a porous region then I cannot imagine why you would want to. A general momentum source can be written which has the performance curve of the turbine you are using - you cannot do this with porous regions and it is far more accurate. Assuming you are applying this as a 3D region, then select both the fluid volume and the turbine volume as the domain. Then you make the turbine region a sub-domain and apply the source term (or porous region if I am not convincing enough). No need for inlets or outlets. Also make sure the mesh is continguous between both regions. Omerta likes this.

January 26, 2012, 06:59		#11
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	You need to define an interface to connect them with your current mesh. It can be a bit tricky selecting the correct surfaces but if you hide and unhide the bodies you can do it. But a better approach is to remesh and make the common surface have a matching mesh. Then you will have no need for an interface. Omerta likes this.

January 26, 2012, 20:09		#13
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Good progress. You will probably need a source term linearisation coefficient. Read the documentation about source terms for this, but if you have defined a constant source then I think that goes to zero anyway so will not help. Be careful with constant source terms - that means you are always adding momentum there, regardless of the flow conditions. It is better to define a fan curve. It is also better to not require the domain interfaces. Try to mesh it with contiguous meshes so you do not need the interface. If you do not know how to do this then do some meshing tutorials. But for your current convergence issues I would not worry about the turbulence equations too much yet. Get the pressure & momentum equations converging before you worry about the turbulence eqns. Omerta likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Lack of local thermal equilibrium in porous medium	Chander	CFX	4	March 4, 2012 05:07
How to use non-equilibrium thermal model for porous medium in Ansys CFX 13.0?	Chander	CFX	3	November 28, 2011 15:26
Cells with t below lower limit	Purushothama	Siemens	2	May 31, 2010 22:58
porous medium and reactions	Valeria	FLUENT	1	July 10, 2009 04:58
Warning 097-	AB	Siemens	6	November 15, 2004 05:41

January 22, 2012, 07:32		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Use a momentum source term to do this. They are move general and you can apply a resistance to the flow in any form you like that way. And the source term can be applied as either a volume or a surface the flow passes through (eg an interface).

January 22, 2012, 13:35		#3
Omerta New Member Kyle Join Date: Nov 2011 Location: New Brunswick, Canada Posts: 25 Rep Power: 15	ok, my prof recommended a porous medium over a momentum source... but you are right it should work fine. Any suggestions on setting up the cylinder in the center? I cannot get them to interact well with eachother. It wants me to define the cylinder's surface as a wall or outlet etc. Should I stick with opening?

January 23, 2012, 02:21		#5
Omerta New Member Kyle Join Date: Nov 2011 Location: New Brunswick, Canada Posts: 25 Rep Power: 15	Hmm, for some reason, it will not allow me to define the turbine region as a subdomain. Is that because it is a boundary region? Should I leave the CAD model as 2 bodies, with the second being the rotor and overlapping the fluid region around the shroud?

January 23, 2012, 06:42		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	A subdomain is a 3D region. A boundary is a 2D surface on the outside of a 3D region.

January 23, 2012, 10:48		#7
Omerta New Member Kyle Join Date: Nov 2011 Location: New Brunswick, Canada Posts: 25 Rep Power: 15	Yes, but it will not allow me to select it as a subdomain because I subtracted the cylinder from the rest of the model. When I didn't combine them it seemed to get confused on the interaction between the bodies

January 23, 2012, 17:39		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	You need to decide what approach you are going to use. If you remove the region then you use a inlet/outlet pair to produce the flow. While this is simple it does make it hard to link to a fan characteristic curve. You can leave the region in and apply the fan as a momentum source. This is a little trickier as you have to do some extra meshing operations and define the momentum source term but is a better approach for most applications.

January 26, 2012, 20:20		#14
Omerta New Member Kyle Join Date: Nov 2011 Location: New Brunswick, Canada Posts: 25 Rep Power: 15	I just used a constant because I wanted to get a solution to work, I will add a fan curve as I make more progress. The turbulence equation stated oscillating and I was assuming that it threw off the rest of the solution as it had started then the pressure and momentum were soon to follow. I'm using Ansys meshing and the tutorials suck for it. Its very difficult to have defined control over what is going on. But I'll see what I can dig up.

January 26, 2012, 20:31		#15
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Let me give you a tip on the meshing - you need to define the two bodies as a single part and the interface surfaces will get a contiguous mesh. Look up multi-body parts in the tutorials or doco. Your convergence problem probably just needs the normal approach - smaller timesteps, better initial conditions, better quality mesh.

January 27, 2012, 11:04		#16
Omerta New Member Kyle Join Date: Nov 2011 Location: New Brunswick, Canada Posts: 25 Rep Power: 15	Thanks, got it to converge now, with setting the timestep (forgot I reset all the data on Workbench) and high res turbulence. Now to figure out that pump curve.