[alberto]

Hi,

a few days ago I updated the following guides on the wiki, for those interested:

• scalarTransportFoam: http://openfoamwiki.net/index.php/ScalarTransportFoam
• bubbleFoam: http://openfoamwiki.net/index.php/BubbleFoam

If you have comments, suggestions or questions, please use this thread.

This is part of the content that should have gone in the documentation project, and the structure used for the guides is very similar to what was the structure of the documents that should have become part of it. Since it did not work out for the reasons we know, I decided to put on the wiki the part of the material I was working on. Keeping it on my hard drive was not helping anybody.

More will come in some time, since rearranging the format is all but fun (no LaTeX macros can be defined to my knowledge on the wiki. If you know a way, please share ).

Best,

[wyldckat]

Hi Alberto,

I've seen you're other thread about these same guides, but only just recently saw this thread...

Originally Posted by alberto

More will come in some time, since rearranging the format is all but fun (no LaTeX macros can be defined to my knowledge on the wiki. If you know a way, please share ).

It's been a while since I last used LaTeX, so I think there are at least two possible interpretations for "LaTeX macros":

• wiki macros that interpret LaTeX;
• "porting" LaTeX macros to wiki, i.e., using the full LaTeX system under wiki.

Uhm... both sound nearly the same. Either way, I did some searching, but haven't gotten around to test either solutions that I've encountered:

1. Convert LaTeX (and others) to wiki (and others) - Pandoc - by the description in its page, looks to me to be the most promising possibility;
2. Online and perl script, for basic convertion from LaTeX to wiki - Latex-to-Wiki-converter - this one is pretty basic, but is downloadable and is a single script
3. Plugin for openfoamwiki - Mediawiki and LaTeX - this would have to be installed in openfoamwiki.net, and might only work for some things, namely equations.

And Thank you for the solver know-how you've shared

In the mean time, I'm still hanging on to the idea of linking up openfoamwiki.net with -extend's SVN in sourceforge... i.e., putting the LaTeX PDF/PS (and even source) versions in the SVN, and making a link to them in the respective solver page in the wiki

Best regards,
Bruno

[alberto]

Originally Posted by wyldckat

Hi Alberto,

I've seen you're other thread about these same guides, but only just recently saw this thread...

Yes, I'm very sorry for the duplicate post. I did not know this thread required moderation to start a new thread, and I simply thought my message would have not been accepted because I posted it in the wrong place, so I opened the other thread. Sorry about that.

1. Plugin for openfoamwiki - Mediawiki and LaTeX - this would have to be installed in openfoamwiki.net, and might only work for some things, namely equations.

Thanks for the tips. The wiki supports LaTeX equations already. The major problem are references, sectioning, command definition and so on, but with soma patience it can be done

And Thank you for the solver know-how you've shared

You're welcome.

In the mean time, I'm still hanging on to the idea of linking up openfoamwiki.net with -extend's SVN in sourceforge... i.e., putting the LaTeX PDF/PS (and even source) versions in the SVN, and making a link to them in the respective solver page in the wiki

This does not depend on me, and you already know that.

Best,

[christian_gross]

Thanks for the guides. They are much appreciated.

[piprus]

First of all, thanks for this contribution. It's a really great job!

One question concerning:

Originally Posted by alberto

More will come in some time,

Can I expect such guide for compressibleInterFoam solver in near future?

[alberto]

Hello,

that solver is not among those I considered to document. Hopefully someone else will contribute the documentation for it, or you could write it if you decide to study how it works.

Best,

[piprus]

Originally Posted by alberto

Hello,

that solver is not among those I considered to document. Hopefully someone else will contribute the documentation for it, or you could write it if you decide to study how it works.

Best,

Thanks for your replay, sorry to read it unfortunately, but maybe something will come up due to another thread. Who knows maybe new solver guide

[alberto]

That would be nice :-)

[wouter]

Hello Alberto,

Thanks for the many contribution to this forum. I was reading the code in the wiki page on bubblefoam and in Ueqns.H I came across:
UbEqn = ... Cvm*rhob*alpha/rhob .... should this not be:
... Cvm*rhoa*alpha/rhob ... ?
I found in OF-1.7.0 of CAElinux that this statement is also in twoPhaseEulerFoam, same .H file?

Best regards
Wouter

[alberto]

I think it is correct as it is, the virtual mass force is given by

Cvm * rho_continuous_phase * ...

in the literature.

[wouter]

Thanks,

I assume I am wrong again if I say that rhob can be removed then altogether?


best regards
Wouter

[alberto]

You are actually right. I think they left to make the code readable, or because they cut and paste Ua, and replaced ;-)

[chenxizh]

hi alberto , I am reading the bubblefoam guides it is very usefull, i thingk there is a mistake in governing equtation of momenton , the Reynolds stress tensor term shuold not have the density rou?

Originally Posted by alberto

Hi,

a few days ago I updated the following guides on the wiki, for those interested:

• scalarTransportFoam: http://openfoamwiki.net/index.php/ScalarTransportFoam
• bubbleFoam: http://openfoamwiki.net/index.php/BubbleFoam

If you have comments, suggestions or questions, please use this thread.

This is part of the content that should have gone in the documentation project, and the structure used for the guides is very similar to what was the structure of the documents that should have become part of it. Since it did not work out for the reasons we know, I decided to put on the wiki the part of the material I was working on. Keeping it on my hard drive was not helping anybody.

More will come in some time, since rearranging the format is all but fun (no LaTeX macros can be defined to my knowledge on the wiki. If you know a way, please share ).

Best,

[alberto]

Hi and thanks for the comment.

I don't think the density should appear, since it is assumed to be constant, and the momentum equation is divided by the phase density (note that the kinematic viscosity is used).

Best,

[chenxizh]

hi, I mean that in section 3.2 the third and fourth term in momentum eqution is obvious not dimemsion balance ?

Originally Posted by alberto

Hi and thanks for the comment.

I don't think the density should appear, since it is assumed to be constant, and the momentum equation is divided by the phase density (note that the kinematic viscosity is used).

Best,

[alberto]

Thanks. I fixed it :-)

[chenxizh]

Hi alberto, recently I run the tutorial bed2(the bubble bed) used twoPhaseEulerFoam, I found that the max volume fraction of the solid will larger than the alphaMax, the alphaMax is 0.62 and alpha actually can reach 0.73? I've turned on the PackingLimter . So what is the problem? can you give me some suggestion? Thank you.
chen

Originally Posted by alberto

Thanks. I fixed it :-)

[alberto]

Hi, that's an issue on how the particle pressure is managed if you use the kinetic theory. If you take a look at the code, it is treated explicitly.

As discussed elsewhere, I proposed a fix to this problem, but it's not released yet.

[chenxizh]

So do you mean that in this version(2.1.0), the foam cannot avoid this problem ? I used Gidsaspow's radial function, the solid pressure will be large when alpha approach the alphaMax to avoid the problem in physcially. So can you give me a hint about how you fix the problem. Thanks a lot.

Originally Posted by alberto

Hi, that's an issue on how the particle pressure is managed if you use the kinetic theory. If you take a look at the code, it is treated explicitly.

As discussed elsewhere, I proposed a fix to this problem, but it's not released yet.

[alberto]

Originally Posted by chenxizh

So do you mean that in this version(2.1.0), the foam cannot avoid this problem ? I used Gidsaspow's radial function, the solid pressure will be large when alpha approach the alphaMax to avoid the problem in physcially. So can you give me a hint about how you fix the problem. Thanks a lot.

The code is implemented correctly, and, if you use a small-enough time step, it should indeed work. However its stability is not strong.

The typical approach to enforce the packing limit is to:

1. Remove the singularity in the particle pressure. One way is to use CarnahanStarling radial distribution function (btw, Gidaspow's radial distribution is not correct, since it is not 1 when alpha is zero. The correct version of that formulation for g0 is the one of Sinclair and Jackson).
2. Use a continuous function to manage the dense (frictional) limit. In such limit, the kinetic theory is not applicable anyways, because collisions are not binary anymore, and there is sustained contact among particles.
3. Include the effect of the particle pressure into the equation for alpha. OpenFOAM does this if the "ppMagf" model is used. Note that ppMagf is the "elastic modulus" of the phase, which is nothing but the derivative d(pa)/d(alpha), being pa the particle pressure. The same approach can be extended to manage packing limit with the kinetic theory model.

What kind of problems do you need to solve? I could try to merge some of the developments I have in my code into twoPhaseEulerFoam, and release them. After all, they are all written in my paper