[skuznet]

I have OF version 2.2.

[derekm]

Originally Posted by wyldckat

Quick answer:

1. I don't have time to diagnose something that was derived from a case that probably wasn't working properly in the first place.
2. Do not jump directly into solving a bigger problem than you're able to do. Start with something small, which is known to work and has at least some documentation, such as this tutorial: http://openfoamwiki.net/index.php/Ge..._-_planeWall2D

Unfortunately going to 2.3 has broken planeWall2D in a few places

changing

neighbourFieldName T;

to

Tnbr              T;

in ChangeDictionaryDict for bottomAir and topAir
and adding

laplacian(rhorAUf,p_rgh) Gauss linear uncorrected;

to fvSchemes in topAir and bottomAir appears to fix it.

[wyldckat]

Greetings Derek,

Many thanks for the feedback! I've uploaded the adapted tutorial for OpenFOAM 2.3, with some additional changes, based on the changes made on the OpenFOAM tutorials: http://openfoamwiki.net/index.php/Ge..._-_planeWall2D

Best regards,
Bruno

[ahmmedshakil]

Hi Foamer,
I have to solve a problem of heat transfer between two solids. I have to solve the transient heat conduction equation for both of the solids with a volumetric heat source. Now, I'm wondering about how to do this for the conjugate heat transfer problem in OpenFOAM. Specially which boundary condition will be good to use at the interface of the two solids. Please advice me.

cheers
shakil

[a19910112a]

hi, everyone. I'm trying to simulate a similar problem with the panelWall2D.I have learned the OpenFoam for three days by reading the 2.3.0 user guide now. I have the following questions:
1.Am I supposed to write up every single file in the example to simulate this question? That's a lot of them! Are there any files are generated automatically?
2.Since the question is looking at a 'air-wall-air' region, why there is only one bloke in the blockMeshDict? My first guess was three.
3. I can roughly understand what each file tries to define, but not quite sure how these are coupled with each other. Is there any document clarifies how I should allocate my question into the files.
4. Is there any file that defines the question that has been solve with the panelWall2D. It's a little bit confusing with only the openfoam file.

Thanks a lot

[wyldckat]

Greetings a19910112a and welcome to the forum!

Originally Posted by a19910112a

1.Am I supposed to write up every single file in the example to simulate this question? That's a lot of them! Are there any files are generated automatically?

OpenFOAM was designed to use text files, because it's actually easier to use things this way... well, up to a certain point, that is. Essentially, it's as simple as copy-paste-adapt the files from the tutorials.

Keep in mind that OpenFOAM is mostly a "DIY - Do-It-Yourself" kind of software toolbox, which is why it's so... manual
Read (again) the first chapter of the User Guide and you'll understand what I mean: http://www.openfoam.org/docs/user/userch1.php

But if you're looking for more interactive ways of dealing with OpenFOAM, check this wiki page: http://openfoamwiki.net/index.php/GUI

Originally Posted by a19910112a

2.Since the question is looking at a 'air-wall-air' region, why there is only one bloke in the blockMeshDict? My first guess was three.

As the wiki page states: http://openfoamwiki.net/index.php/Ge..._-_planeWall2D

topoSetDict - Here you defined the extents of each region. It's here that you can select which cells of the mesh that belong in each region.

The initial mesh is done with blockMesh, but topoSet helps select which cells are associated to each region.

Originally Posted by a19910112a

3. I can roughly understand what each file tries to define, but not quite sure how these are coupled with each other. Is there any document clarifies how I should allocate my question into the files.

Not that I'm aware of. But check the report given in the first reference at the section "4. References": http://openfoamwiki.net/index.php/Ge...l2D#References

Originally Posted by a19910112a

4. Is there any file that defines the question that has been solve with the panelWall2D. It's a little bit confusing with only the openfoam file.

Sorry, I didn't understand your question. Perhaps the report mentioned above answers your question?

Best regards,
Bruno

[a19910112a]

hi,wyldckat.
Thank you so much for you reply.I have looked through the wall2D example, and understand most of it now.

The problem I'm trying to simulated is similar to it:
I need to replace the bottom air with some matter that can generate heat, and the top air with liquid coolant (e.g. water,sodium). This is more like the example 3.7 described in the Fundamentals of Heat and Mass Transfer book (http://www.ualberta.ca/~seyedsha/Fun...-Incropera.pdf). Is there any Foam example on this? I have several questions on this problem:

1. Do you think I can still use the chtMultiRegionSimpleFoam solver for this question? If not can you suggest one? (my main concern is that the solver is designed for compressible fluid, isn't it? In addition to that, a heat source is added)
2. The wall2D example is a natural convection or half-natural convection problem to me (I'm not quite sure about this), so that factors like pressure and gravity may matter. My case will be forced convection, therefore I think the factors such as gravity will not matter any more. How should I eliminate them from the code?
3. It seems that how to define the changeDictionaryDict file is not described in the official User guide, is there any instructive documents on this?

question on Wall2D example:
4. What is the alternative way to run the ALLRUN file? As my ssh server does not allow this kind of script to run.

Thanks a lot.

[zfaraday]

Hi man/woman with a weird name!

Originally Posted by a19910112a

The problem I'm trying to simulated is similar to it:
I need to replace the bottom air with some matter that can generate heat, and the top air with liquid coolant (e.g. water,sodium). This is more like the example 3.7 described in the Fundamentals of Heat and Mass Transfer book. Is there any Foam example on this? I have several questions on this problem:

1. Do you think I can still use the chtMultiRegionSimpleFoam solver for this question? If not can you suggest one? (my main concern is that the solver is designed for compressible fluid, isn't it? In addition to that, a heat source is added)

I think that chtMultiRegion(Simple)Foam is what you need if you are looking for a conjugate heat solver for compressible fluids. I don't know exactly what could be the problems (if there is any) if you need to solve a water region as an incompressible fluid. However, I think that incompressible version of chtMultiRegion solver have been already developed and you can find information in the forum. Let's see if someone can shed some light on it...

Originally Posted by a19910112a

2. The wall2D example is a natural convection or half-natural convection problem to me (I'm not quite sure about this), so that factors like pressure and gravity may matter. My case will be forced convection, therefore I think the factors such as gravity will not matter any more. How should I eliminate them from the code?

I'm not so sure about the unnecessity to use the parameters you mention. However, you can change their values easily without the need of modify the solver's code. For instance, you can modify the file constant/<fluid region>/g in order to decrease the value of the gravity

Originally Posted by a19910112a

3. It seems that how to define the changeDictionaryDict file is not described in the official User guide, is there any instructive documents on this?

This utility is used when you need to modify dictionaries. In this case, what you are doing is to update the files 0/<x_region>/<y_variable> and also, perhaps, constant/<x_region>/polyMesh/boundary if needed. This is done after the region spliting process because you need to define the boundary conditions in the interface of the different regions. Initially you can only define the general (outer) boundary conditions of the firsts blocks you defined with blockMesh, but, afterwards you have to define the interregion coupling. You can do it either manually or with the use of the changeDictionary utility.

Originally Posted by a19910112a

question on Wall2D example:
4. What is the alternative way to run the ALLRUN file? As my ssh server does not allow this kind of script to run.

As I'm not a linux expert user I don't know alternative ways. Have you tried to modify the permissions via chmod command? Otherwise you can run the case manually, running each command one after another manually.

Originally Posted by a19910112a

Thanks a lot.

You're welcome! Hope it helps a little...

Regards,

Alex

[a19910112a]

hey,Alex. Thanks for your reply. I have the following ideas on your answer:

Question 2: You mentioned that I could change the gravity in the g file. I knew that,. But what if the gravity is not a factor I will need to consider in my situation? I simply set it to 0?
Question 3: That answer is very helpful. Do you have any ideas on how to swap the bottom air area with a heat generating area? I saw people were talking about adding a fvOptions file, is that right? What should the fvOptions file define? This is also not described in the user guide.

In addition, since there are a lot of useful functions of openFOAM is not mentioned in the user guide, how did you learn about them?

And do you know if there is a tutorial that is similar to my case? It seems to be a very common situation in heat transferring.

Thanks a lot.
Zech

[zfaraday]

Originally Posted by a19910112a

hey,Alex.

Hey, R2D2 friend.

Originally Posted by a19910112a

Thanks for your reply.

You're welcome.

Originally Posted by a19910112a

I have the following ideas on your answer:

Question 2: You mentioned that I could change the gravity in the g file. I knew that,. But what if the gravity is not a factor I will need to consider in my situation? I simply set it to 0?

Yes. Althoguh it may give you problems if you give it a value of 0. Thus, you can try with a small value, e.g. 1e-3, instead.

Originally Posted by a19910112a

Question 3: That answer is very helpful. Do you have any ideas on how to swap the bottom air area with a heat generating area? I saw people were talking about adding a fvOptions file, is that right? What should the fvOptions file define? This is also not described in the user guide.

That's right, fvOptions is what you need to set up a volumetric heat source. The proper type of it shoud be scalarSemiImplicitSource so that you can define the value of the generation in it. It's easy to do that, just find more info in $FOAM_SRC/fvOptions/sources/general.

Originally Posted by a19910112a

In addition, since there are a lot of useful functions of openFOAM is not mentioned in the user guide, how did you learn about them?

On my own! Looking for info in the code, the header files (those ended with .H) contain a brief explanation of the utilities' usage so that you can know how they work. Reading related threads in the forum. And last but not the least, by making use of an ancient method our ancestors used to use a lot. With this method they could discover really great things, such as the fire!!! This method is know as Trial and Error.

Originally Posted by a19910112a

And do you know if there is a tutorial that is similar to my case? It seems to be a very common situation in heat transferring.

No idea...

Originally Posted by a19910112a

Thanks a lot.
Zech

You're welcome.


Regards,

Alex

[a19910112a]

hey, one quick question:
I know that, in the wall2D example, the changeDictionaryDict is used for defining the boundary functions. But what do the expressions such as "topAir_to_.*" and "ILambda.*" mean? I guess ".*" could mean "rest of them" or "those that are not defined",but cannot even guess that.

And p and p_rgh are given same values. somebody told me that P_rgh=p- rho*g*h. If that is true, then rho*g*h some how becomes 0?

It's also confusing that how the value of epsilon and k are calculated according to equation 2.8 and 2.9 in the user guide.

[a19910112a]

Dear All,

I find a problem will the planeWall2D case.

I drew the temperature profile of the bottom line of the topAir area and found a curve rather than a straight line as I expected.

I looked at the case description. Because the wall and fluids are infinity that should not be the case. I also checked all the temperature boundary conditions that are defined in both 0 and system folders.

Also I think the temperature of the topAir should in crease along the direction it flows as the bottom air keeps transferring heat to it along the direction. However, the temperature profile shows the temperature is constant. This should also be a problem.

Anyone knows what's going on?

[wyldckat]

Greetings to all!

@a19910112a: To start off, please do take some time to add new information to the tutorial on the wiki, specially after checking with people here on the forum what's right or not

Originally Posted by a19910112a

hey, one quick question:
I know that, in the wall2D example, the changeDictionaryDict is used for defining the boundary functions. But what do the expressions such as "topAir_to_.*" and "ILambda.*" mean? I guess ".*" could mean "rest of them" or "those that are not defined",but cannot even guess that.

".*" is part of the regular expressions syntax:

• http://en.wikipedia.org/wiki/Regular_expression
• http://www.openfoam.org/archive/1.6/...s.php#x4-30000
• http://www.cfd-online.com/Forums/ope...tml#post306742
• http://www.cfd-online.com/Forums/ope...tml#post273069

Originally Posted by a19910112a

And p and p_rgh are given same values. somebody told me that P_rgh=p- rho*g*h. If that is true, then rho*g*h some how becomes 0?

The example given at http://openfoamwiki.net/index.php/Ge..._-_planeWall2D does emphasise that the reader should do several exercises in order to understand better how things work.
This to say that you are correct in pointing out that the values seem very suspicious. Nonetheless, there is a trick being used in the "changeDictionaryDict" file that isn't very well explained, but that it's implied by the settings. For example:

• For "p_rgh":
  

              leftLet
              {
                  type            fixedValue;
                  value           uniform 1e5;
              }

• For "p":
  

              leftLet
              {
                  type            calculated;
                  value           uniform 1e5;
              }

This implies that the "p" field on the patch "leftLet" will be calculated based in the first few iterations.
In addition, this:

internalField   uniform 1e5;

is only the initial value. It will be adjusted accordingly by the solver, so you'll have to let it run for a while until it stabilizes.

Originally Posted by a19910112a

It's also confusing that how the value of epsilon and k are calculated according to equation 2.8 and 2.9 in the user guide.

?? I don't remember reading this on the User Guide a few years ago... this is now in subsection "2.1.8.1 Pre-processing"!
I know I wrote something about this sometime ago... OK, after a quick search, this thread seems to be detailed enough: http://www.cfd-online.com/Forums/ope...on-values.html

Originally Posted by a19910112a

I drew the temperature profile of the bottom line of the topAir area and found a curve rather than a straight line as I expected.

OK, the 2 points for the line are:

1. 0; 0.6; 0.05
2. 1; 0.6; 0.05

Uhm... see the next quote/answer:

Originally Posted by a19910112a

I looked at the case description. Because the wall and fluids are infinity that should not be the case. I also checked all the temperature boundary conditions that are defined in both 0 and system folders.

You didn't fully read the exercises, namely section "3 Suggested Exercises", did you?
There it's written this: http://openfoamwiki.net/index.php/Ge...sted_Exercises

• Extend the wall or apply the cyclic boundary condition to the outlets and inlets (the ones named leftLet and rightLeft), turning this into an infinite wall.

Which implies that the presented example is not an infinite wall. It's a very finite wall, which is why you're seeing a curve instead of a linear effect, namely because the flow is not fully developed!

Originally Posted by a19910112a

Also I think the temperature of the topAir should in crease along the direction it flows as the bottom air keeps transferring heat to it along the direction. However, the temperature profile shows the temperature is constant. This should also be a problem.

Again, not an infinite wall

Originally Posted by a19910112a

Anyone knows what's going on?

Yes, I do: you didn't fully read into all of the (implied and explicit) details of this tutorial/example
This tutorial explicitly states not being complete right in the introduction section and essentially tries to give the reader the sense of "this is only a start and every single detail is important, because it's not explained in every single detail"!
And that you should do the mentioned exercises, in order to gain more experience on this type of simulation

Best regards,
Bruno

[a19910112a]

Thanks for your answer, Bruno.

Well I think the 'the case is not infinite' might be able to explain why the curve appears and therefore the temperature profile along the same line in the wall and topAir area doesn't match. But, it seems that it could not explain why the temperature doesn't increase along the line: infinite or not, heat is accumulated along the x direction, without changing in mass and heat capacity, the temperature should increase anyway.

I have done the step mentioned in the exercise ( change the boundary condition to cyclic and set the wall to be infinite long). There seems nothing has changed with the temperature profile. The 'curve' is still there.

I cannot upload the case file here, as I don't really know how to properly set the cyclic boundary conditions using the changeDictionaryDict, therefore many setting steps are done manually. Every time I try to do that, I get a floating point exception error.

Waiting for more answers...

Thanks and Wishes
Zech

[wyldckat]

Quick answers:

Originally Posted by a19910112a

But, it seems that it could not explain why the temperature doesn't increase along the line: infinite or not, heat is accumulated along the x direction, without changing in mass and heat capacity, the temperature should increase anyway.

I'll have to take a closer look (won't be able to do so in the next couple of weeks), but my guess is that what you're seeing is a plume effect... I can't find any pictures right now, but the explanation is simple: the heat is inducing an expansion layer and as it expands, it dissipates the heat along that boundary layer.

Originally Posted by a19910112a

I have done the step mentioned in the exercise ( change the boundary condition to cyclic and set the wall to be infinite long). There seems nothing has changed with the temperature profile. The 'curve' is still there.

Mmm... I suspect that something might be missing.

Originally Posted by a19910112a

I cannot upload the case file here, as I don't really know how to properly set the cyclic boundary conditions using the changeDictionaryDict, therefore many setting steps are done manually. Every time I try to do that, I get a floating point exception error.

The idea is to leave the case folder as clean as the one provided on the wiki and then compress the whole folder to a "zip" or "tar.gz" file. As long as the file is smaller than 100kB, the forum should accept it.

[a19910112a]

Hello,Bruno. Thanks for answering again.

Can you please clarify what should be set to be infinite for the exercise? Just the wall or the flows as well? If it's the flows, how could you define the boundary as cyclic and fixed inlet values at the same time?

[a19910112a]

Hi,Bruno. I know that you will not be able to look at the posts recently, but I will just post things I did related to the question here.

With the previous results, I thought: 'fine! If that problem is still too complex for me, I will try an even simpler one'. Therefore I wrote up a case uses buoyantBoussinesqPimpleFoam to solve only the topAir area (by setting a fixed T gradient at the topAir_bottom boundary). As the problem is not with quantity, I disregarded the thermal properties numbers and used the files copied directly from the solver's tutorial case's files directly and even a different sized block was defined. The result is that I get the exactly same two problems:
1. The drops at the edges (the curved temperature profile) along the top_air bottom boundary.
2. Temperature does not increase along the flow direction.

I did not use the cyclic boundary as the question in post #56 is not answered yet.

Please find the attachments for more details.

[wyldckat]

Hi Zech,

Originally Posted by a19910112a

Can you please clarify what should be set to be infinite for the exercise? Just the wall or the flows as well? If it's the flows, how could you define the boundary as cyclic and fixed inlet values at the same time?

Let me check what I wrote...

Extend the wall or apply the cyclic boundary condition to the outlets and inlets (the ones named leftLet and rightLeft), turning this into an infinite wall.

So, if I reverse the sentence:

To turn this into an infinite wall, either:

1. Extend the wall;
2. or apply the cyclic boundary condition to the outlets and inlets (the ones named leftLet and rightLeft).

Nice... I inverted a sentence as if it was an equation

But since you asked, the idea behind that sentence was as follows:

1. Changing the geometry of the case to have something that is 100 times longer would make it pretty big. Not infinite, but pretty big.
2. Using cyclic boundary conditions will essentially make the fluid teleport from patch A to patch B, making it go round and round and round... until it reaches infinity when it converges... assuming of course, that it ever converges, which it might not converge.

Oh, as for an example that either uses changeDictionary or cyclic boundary conditions...

• http://openfoamwiki.net/index.php/In...with_the_Shell
  • http://openfoamwiki.net/index.php/In...hing_for_files

    • find $FOAM_TUTORIALS -name "changeDictionaryDict"
      find $FOAM_TUTORIALS -name "blockMeshDict" | xargs grep -sl cyclic

-------------

Originally Posted by a19910112a

With the previous results, I thought: 'fine! If that problem is still too complex for me, I will try an even simpler one'.

Thumbs up! Simpler the case, the better to start understand how things work.

Originally Posted by a19910112a

Therefore I wrote up a case uses buoyantBoussinesqPimpleFoam

Sorry to say that using that solver is not simple enough "buoyant Boussinesq" is an approximation for incompressible flow: http://en.wikipedia.org/wiki/Boussin...%28buoyancy%29
In other words: it won't always work as expected, specially if you work outside of the operational temperature zone.

It's preferable if you use buoyantPimpleFoam or buoyantSimpleFoam. (FYI: I use bold for telling apart solver names from text.)

Originally Posted by a19910112a

to solve only the topAir area (by setting a fixed T gradient at the topAir_bottom boundary). As the problem is not with quantity, I disregarded the thermal properties numbers and used the files copied directly from the solver's tutorial case's files directly and even a different sized block was defined. The result is that I get the exactly same two problems:
1. The drops at the edges (the curved temperature profile) along the top_air bottom boundary.
2. Temperature does not increase along the flow direction.

I did not use the cyclic boundary as the question in post #56 is not answered yet.

Please find the attachments for more details.

I will only be able to look into more details about this near the end of the year, which hopefully will be when I get some vacation time.

What I can say right now and which I only now noticed that I should have emphasized once again (I think I wrote this sometime ago on this very same thread): In order to fully understand what's happening with these solvers and to properly validate if they are working correctly, is to find the analytical solution for this problem. In other words, you need to find the function of temperature dependant on the distance to the wall.
This requires that you study chapter 3 from the book Fundamentals of Heat and Mass Transfer by Frank P. Incropera et. al, or a similar book.


Back when I wrote this particular wiki page, I did try to find a similar tutorial online that explained this in detail, namely the analytical part, but I wasn't able to find one
If you can ask one of your teachers for another example of this, please let us know about it!


By the way, at the end of the wiki page for the "Plane Wall 2D" are links to a project that used this wiki page as a basis. The author of that report has some more details on this topic and also shows a similar temperature distortion near the outlet.


Which reminds me: I originally was thinking that you're aware of what a "boundary layer" is. If you aren't aware of what it is, here's some interesting reading material: http://en.wikipedia.org/wiki/Boundary_layer

Best regards,
Bruno

[wyldckat]

Greetings to all!

I had this on my to-do list for sometime now and over a period of 10 hours today I worked on and off on the tutorial page discussed on this thread, namely this tutorial: http://openfoamwiki.net/index.php/Ge..._-_planeWall2D

I've improved a bit the case description, by adding images and the equivalent diagram. But the bulk of the additions were by adding the new subsection "2.5 Understanding the physics", where most of the topics addressed in the past few posts have been compiled here for a better understanding of what's going on.
In addition, I've emphasized in the introduction that this tutorial is not something ready to be used as a practical case. It's only something to start with and to begin carefully diagnosing one step at a time what each detail really means.


Unfortunately I'm not willing to spend much more time on this in the coming 6 or so months, because in these 10 hours that passed today, I wanted to also have been able to answer a lot of the questions that are on my to-do list and could not do it, because I was busy with this tutorial... and some of those questions have been left unanswered for some 6 months already oh well...

This to say: if people want this tutorial to be better, please study this in more detail, test things and contribute to the wiki page as well!

Oh, and Happy New Year to everyone as well!

Best regards,
Bruno

[vasava]

I noticed that many people are having problems with the cht*.* solvers. So I would like to share my experience and how I overcame it. I am not sure if it works for everyone but you could try this.

I have been trying heat-exchanger example of my own with chtMultiRegionSimpleFoam. For all my attempts my cases use to diverge after few iteration citing an abnormally high temperature as an excuse. The transient solver chtMultiRegionFoam worked quite nicely for the same example. But it was very slow. At one point I lost my patience and decided to switch back to the steady state solver. After switching the steady state solver worked nicely without any problems.

I think the solution from the transient solver provided a better initial guess for the steady-state solver.

Do comment if you believe that I am doing something wrong or something in a wrong way.