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

jumpCyclic

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 17, 2011, 12:06
Default jumpCyclic
  #1
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 7
doubtsincfd is on a distinguished road
Is there any tutorial for jumpCyclic boundary condition?
doubtsincfd is offline   Reply With Quote

Old   July 18, 2011, 02:18
Default
  #2
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
please dont create the same topic several times! and usually before make a new thread you should search in forum at first, you will find many new thread about it!
you can search about "jumpCyclic" and "fan" boundary condition, you will find examples and threads about it
nimasam is offline   Reply With Quote

Old   July 18, 2011, 02:46
Default
  #3
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 7
doubtsincfd is on a distinguished road
I did read the previous posts. Fan BC is available for pressure. I want to implement jumpCyclic BC for variable "T" in laplacianFoam. No previous post is telling clearly about how to implement this BC. Which tutorial has this boundary condition implemented is also not mentioned. Last post on jumpCyclic (not fan BC) was 2 years back.
doubtsincfd is offline   Reply With Quote

Old   July 18, 2011, 03:58
Default
  #4
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
i guess
you can use the same approach for temperature
fan BC supports scalar jump, you just need to define ur temperature jump which is difference between in (Tinlet - Toutlet) as value of f in fan BC
nimasam is offline   Reply With Quote

Old   July 18, 2011, 14:02
Default
  #5
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 7
doubtsincfd is on a distinguished road
I tried for T, but it is not working. It required value of phi. I even edited the fanFvPatchFields.C and removed the phi part (the jump is calculated as maximum of specified and 0.5U*U, U is calculated using phi). But I am still getting the error:

--> FOAM FATAL ERROR:

request for surfaceScalarField phi from objectRegistry region0 failed
available objects of type surfaceScalarField are

4
(
DT
differenceFactors_
weightingFactors
(DT*magSf)
)


From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/opencfd/OpenFOAM/OpenFOAM-1.7.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 139.

FOAM aborting
doubtsincfd is offline   Reply With Quote

Old   July 18, 2011, 14:12
Default
  #6
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
use a boundary like this
patchName
{
type fan;
patchType cyclic;
f List<scalar> 1 (2); // put ur value difference here
value uniform 0;
}
nimasam is offline   Reply With Quote

Old   July 18, 2011, 17:28
Default
  #7
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 7
doubtsincfd is on a distinguished road
Its working. I was using the boundary condition for fan as:

type fan;
patchType cyclic;
f List<scalar> 2 (10.0 -1.0);
value uniform 0;

But I have no idea what that -1.0 stands for. I am not good at OF programming. But the BC you have suggested works! Thank you so much!
doubtsincfd is offline   Reply With Quote

Old   July 18, 2011, 17:50
Default
  #8
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 7
doubtsincfd is on a distinguished road
One last question.

Is it possible to implement non uniform pressure jump, say as a list of values for the cell centers or node points on the patch?

Thank you.
doubtsincfd is offline   Reply With Quote

Old   July 18, 2011, 21:24
Default
  #9
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
its a polynomial coefficient
f= 10 - 1*U + 0*U^2 + ...
as laplacianFoam doesnot have any U variable, you can not use other coefficient except the first one.
nimasam is offline   Reply With Quote

Old   July 18, 2011, 22:10
Default
  #10
Senior Member
 
Join Date: Nov 2009
Location: Michigan
Posts: 135
Rep Power: 7
doubtsincfd is on a distinguished road
What I want to implement is , lets say I have 100 nodes on my patch. I want to assign different jump values to each node. Right now, whatever value of jump I give, it remains constant for all the points on the patch. Something similar to timevaryingmappedfixedvalue
doubtsincfd is offline   Reply With Quote

Old   July 19, 2011, 15:06
Default
  #11
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
look into fanFvPatchFields.C line 50 :
jump_ = f_[0];

jump_ define the value of jump for each node

1) maybe you need to define "f" as field type or read jump_ value directly from ioDictionary , you should look deeper but its possible
nimasam is offline   Reply With Quote

Old   June 3, 2014, 11:48
Default Error mapping p
  #12
New Member
 
Dominik Pöltl
Join Date: Jul 2013
Location: Hamburg
Posts: 14
Rep Power: 4
Yeru is on a distinguished road
Dear all,
thanks for the thread so far. I had the same aim as doubtsincfd and also the same problem:

Here's what I changed according to your advice:
-defined all patches as master/slave pairs in blockMeshDict
Code:
    cyclic innerRect0
    (
        (0    1     2    3)    //0, front
        (17    20     19    18)    //12, back
    )
-set all patches to type cyclic in 0/U-file
Code:
    innerRect0
    {
        type            cyclic;
    }
-set all patches to type fan in 0/p-file
Code:
    innerRect0
    {
        type            fan;
        patchType       cyclic;
        f               List<scalar> 2(10 -1);
    }
-had to run foamUpgradeCyclics

I can even map the mesh in paraFoam without mapping the field for p.
As soon as I want to map it, here's what I get:

Code:
--> FOAM FATAL ERROR: 

    request for surfaceScalarField phi from objectRegistry region0 failed
    available objects of type surfaceScalarField are
1(weights)

    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 136.

FOAM aborting
Any idea how to solve this?
P.S. I'm running OF 2.2.0
Yeru is offline   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
JumpCyclic brahim OpenFOAM Running, Solving & CFD 3 July 17, 2011 21:23
jumpCyclic bc not for scalar field? doubtsincfd OpenFOAM 0 July 12, 2011 18:02
Velocity BC in cyclic 2D domain Ivo OpenFOAM 1 July 30, 2010 11:22
Cyclic jump boundary condition hjasak OpenFOAM Running, Solving & CFD 10 April 16, 2010 15:35
jumpCyclic? leejc OpenFOAM 1 April 16, 2010 15:10


All times are GMT -4. The time now is 15:48.