CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

block geometry inside fluid domain

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 10, 2004, 09:37
Default block geometry inside fluid domain
  #1
jeff
Guest
 
Posts: n/a
i am working on extending SIMPLE to simulate the solid block within fluid domain. now, SIMPLE maps a rectangular domain and uses domain extension method to treat the solid domain. i am trying to a bakward-facing step problem, but don't wanna use domain extension method. So the i-, j-, k-, cannot be numberred simply from 1 to max. anyone can provide some advice or reference on this? Thanks a lot
  Reply With Quote

Old   April 10, 2004, 19:04
Default Re: block geometry inside fluid domain
  #2
Mike
Guest
 
Posts: n/a
Very fun solition

add one more array - logical and one else array - integral then all points which is inside let 99 then found numerals which is wont repeated for border points it will took other values then your back ward facing step will look like (2d)

71 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 33

66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 9999 99 99 99 99 99 91

66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

59 32 32 32 32 11 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

00 00 00 00 00 66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

00 00 00 00 00 66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

00 00 00 00 00 66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

00 00 00 00 00 66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

00 00 00 00 00 59 32 32 32 32 32 32 32 32 32 32 32 32 32 32 32 32 55

main disadvantage - you will have idle points, but if your solver is non commercial but just for study - I found it rather usefull

and it will be need to add into the solver logical switches which will control fluxes for border points (you cwn use one solver for all variables)

i.e. internal points 99

which won't be in use 00

e border points - 91

w border points - 66

n border points - 77

s border points - 32

wn corners - 71 (external)

ws corners - 59 (external)

es corners - 55 (external)

en corners - 33 (external)

and so on for 3D case

before you will generate grid - make such array

but look through classic work - by Kim - he had rectangular domain
  Reply With Quote

Old   April 10, 2004, 21:29
Default Re: block geometry inside fluid domain
  #3
jeff
Guest
 
Posts: n/a
thanks a lot, Mike.

I am modeling the turbulence flow and I need special treatments for the solid walls. this is why i don't wanna follow the domain extension any more.

In my previous code, the finite volume equations are solved using TDMA+ADI. My question is "can they still work if I add the array as you advise?".

I am thinking between two options: a) using two zones of grids to map the upstream and the downstream sections, respectively. Something is like the multi-block method. In this way, the solver (ADI+TDMA) can still be used because the compuational domain is rectangular in either zone. b) changing the coefficients of the finite volume equations. Only one zone of grid will be used, but the regular TDMA+ADI algorithm cannot be used directly (not from 1 to maximum).

By the way, could you provide more information about the classic paper by Kim? Paper title, journal, vol. and issue numbers?

Thank you very much.
  Reply With Quote

Old   April 11, 2004, 07:25
Default Re: block geometry inside fluid domain
  #4
Mike
Guest
 
Posts: n/a
Sure it will work

Unfortunately I've lost my code and can't send it to you I should add that you will apply this procedure and for TDMA ADI

all nodes with "99" will be treated as internal points (P and Q computation)

in I direction

- nodes which marked as "66" will be treated as "1st" point,

- nodes which marked as "91" will be treated as "max" point,

in J direction

- nodes which marked as "32" will be treated as "1st" point,

- nodes which marked as "77" will be treated as max point,

flow over cylinder

71 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 77 33

66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 9999 99 99 99 99 99 91

66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

66 99 99 99 99 99 99 32 32 32 32 32 32 32 32 32 32 99 99 99 99 99 91

66 99 99 99 99 99 99 91 00 00 00 00 00 00 00 00 66 99 99 99 99 99 91

66 99 99 99 99 99 99 91 00 00 00 00 00 00 00 00 66 99 99 99 99 99 91

66 99 99 99 99 99 99 91 00 00 00 00 00 00 00 00 66 99 99 99 99 99 91

66 99 99 99 99 99 99 91 00 00 00 00 00 00 00 00 66 99 99 99 99 99 91

66 99 99 99 99 99 99 91 77 77 77 77 77 77 77 77 66 99 99 99 99 99 91

66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

66 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 99 91

59 32 32 32 32 32 32 32 32 32 32 32 32 32 32 32 32 32 32 32 32 32 55

what is concerned Kim's work, I also had it but lost. so may be yoy will find it at Kim's web (look through CFD guru's list at CFD on line)
  Reply With Quote

Old   April 11, 2004, 07:31
Default Re: block geometry inside fluid domain
  #5
Mike
Guest
 
Posts: n/a
as for treatment of solid walls I used additional domain for boundary conditions above mentioned array only describe computational domain, and I also added an array wich described solid walls, inlet and outlet conditions, I had a very complex geometry and a lot of holes with fuel sprays
  Reply With Quote

Old   April 11, 2004, 07:42
Default Re: block geometry inside fluid domain
  #6
Mike
Guest
 
Posts: n/a
configuration in this case may vary as only you want to and you will only need to build universal solver, and

all work will be in preparation for computations when you build a grid and compute values of alfa beta gamma. This work will be done separately

  Reply With Quote

Old   April 11, 2004, 07:56
Default Re: block geometry inside fluid domain
  #7
Mike
Guest
 
Posts: n/a
you will apply the procedure to the whole domain (e.g. 300 x 300 x 300) and your solver will decide all itself where it will solve, and where it won't.

it does not matter, what will be in it and what geometry will be - you all describe earlier, when you build a grid and this additional array.

  Reply With Quote

Old   April 11, 2004, 08:10
Default Re: block geometry inside fluid domain
  #8
Mike
Guest
 
Posts: n/a
look at this line

and I hope you will understand idea

i >>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>>> >>>>>>>>>> max

66 99 99 99 99 99 99 91 00 00 00 00 00 00 00 00 66 99 99 99 99 99 91

It doesn't matter for your TDMA ADI solver. It solves the whole domain. and P and Q arrays have the same dimensions P(300) Q(300)

Just in "00" it won't work at all

points marked as "66" will treated as "1st"

points marked as "91" will treated as "max"

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

the same thing and with Aw, Ae, As, An, At, Ab coefficients

for example

you add in your solver addition that for point "77" convective flux at "N" face equal zero
  Reply With Quote

Old   April 11, 2004, 08:18
Default Re: block geometry inside fluid domain
  #9
Mike
Guest
 
Posts: n/a
May be it won't be zero in common case, it depends from boudary conditions, but I hope you understand me rather well.

When I used HLPA and other TVD schemes, it was important to describes such points, cause HLPA scheme uses (e.g. E face) ee + e + P values, and it's important to point, where it own't be used.

Also it's important when you use Rhie and Chow monotonizator for colocated grid arrangement
  Reply With Quote

Old   April 11, 2004, 08:27
Default Re: block geometry inside fluid domain
  #10
Mike
Guest
 
Posts: n/a
Corner points I described separately

so you have to describe all cases

edge faces "E" "W" "N" "S" "T" "B"

corners "es" "en" "ws" "wn" "ts" "tb"

corners such as "est"

all that was for non orthogonal complex geometry, TVD schemes for convective fluxes, and standard k-eps model and colocated arrangement

It took three years for me to build such sover from complete zero (Patankar's book) and a lot of disturbances

  Reply With Quote

Old   April 11, 2004, 08:43
Default Re: block geometry inside fluid domain
  #11
Mike
Guest
 
Posts: n/a
The same and with wall functions (in K-eps model) and with Sp terms

I made all using fluxes' treatment

and logical switches for boundary's nodes

  Reply With Quote

Old   April 11, 2004, 10:17
Default Re: block geometry inside fluid domain
  #12
Mike
Guest
 
Posts: n/a
I remember how I implemented boundary values

It's very plain

First node I put at the boundary volume's face

e.g.

W-boundary control volume

!----------------------------------------------------------------------------!

!................................................. .................................................. .................!

!................................................. .................................................. .................!

!................................................. .................................................. .................!

"1st" i-node ................................. 2nd i-node .................................!

(u,v,w,p,k,e)..................................(u, v,w,p,k,e).......................................!

!................................................. .................................................. .................!

!................................................. .................................................. .................!

!................................................. .................................................. .................!

!--------------------------------------------------------------------------------!

then you set all necessary boundary variables from these values, and they change only if it will be outlet boundary conditions

and sure I used colocated arrangement

it took a lot of time to decide all this, cause I worked alone by trials and errors method

here - it's essential of my results

why I put "1st" - in " " ?

because it can be both 60th and 200th

just it's important that before it - "00" or it's really the 1st node

I mean it's an edge point where we set a fixed values of variables

the same and with "max" nodes and other directions
  Reply With Quote

Old   April 11, 2004, 10:20
Default Re: block geometry inside fluid domain
  #13
Mike
Guest
 
Posts: n/a
In previous case

1st will be "66"

2nd will be "99"
  Reply With Quote

Old   April 11, 2004, 10:40
Default Re: block geometry inside fluid domain
  #14
jeff
Guest
 
Posts: n/a
wow, thank you very much for your help, Mike.

I think all your posts clarify my questions. I will change the modules of coefficient generation and solver. Now the ist, jst and kst will not be a constant and might be one value, depending on how many solid "blocks" there are within the fluid demain. So will the iend, jend, and kend.

I was using staggered grid distribution. But I can switch to collocated one, if necessary.

Again, I appreciate your help very much. Happy Easter.
  Reply With Quote

Old   April 11, 2004, 10:45
Default Re: block geometry inside fluid domain
  #15
jeff
Guest
 
Posts: n/a
By the way, the corners should be okay, since they are not solved in the code. There are no algebraic equations for the corners. Actually, the wall B.C.s are not solved either in my code. Thanks
  Reply With Quote

Old   April 11, 2004, 11:15
Default Re: block geometry inside fluid domain
  #16
Mike
Guest
 
Posts: n/a
no Jeff.

I rejected the whole idea to use ist, jst, kst indexes

I used cycle do i=1,Nmax (where N max e,g, = 300) for whole domain

and switches decide what point they have to solve and what point is out of consideration.

I thought about universaal solver, which used only the ready prepared arrays of geometry (X,Y,Z coordinates) and this additional describing array where is indicated, what point have to be treated (which I showed)

Also array describing B.C.

And array of initial values of dependent variables such as U,V,W,k,eps, P, T
  Reply With Quote

Old   April 11, 2004, 11:30
Default Re: block geometry inside fluid domain
  #17
Mike
Guest
 
Posts: n/a
There are NOT any ist jst kst values in solver

only array with "99", "00", or "32" which indicated what point is boundary and what point is inside flow

only consideration of how to treat every node, depending upon is this "99", "00", or "32" point and I also made simplifyer, cause logical operataion with boolean variable is less expensive (CPU time) then with integral ones

  Reply With Quote

Old   April 11, 2004, 15:27
Default Re: block geometry inside fluid domain
  #18
Mike !!!!!!!!!!!!!!!!!!!!!!!!!1
Guest
 
Posts: n/a
I guess you didn't understand me properly

"99" "00" "32" - only signs, it even could be boolean variables,

they only changed words -

"internal point" means 99

"W border point" means 66

"E border point" means 91

"S border point" means 32

"N border point" means 77

"out of flow" means 00

and so on

I used numbers cause it uas connected with how I generated and controlled this array

  Reply With Quote

Old   April 12, 2004, 11:37
Default Re: block geometry inside fluid domain
  #19
jeff
Guest
 
Posts: n/a
I get your idea. Thanks a lot, Mike.
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
CFX domain comparison Kiat110616 CFX 4 April 3, 2011 22:43
Icem Mesh to Foam jphandrigan OpenFOAM Mesh Utilities 4 March 9, 2010 03:58
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
meshing F1 front wing Steve FLUENT 0 April 17, 2003 12:37


All times are GMT -4. The time now is 11:39.