# jumpCyclic

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 July 17, 2011, 12:06 jumpCyclic #1 Senior Member   Join Date: Nov 2009 Location: Michigan Posts: 135 Rep Power: 9 Is there any tutorial for jumpCyclic boundary condition?

 July 18, 2011, 02:18 #2 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,236 Blog Entries: 1 Rep Power: 18 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

 July 18, 2011, 02:46 #3 Senior Member   Join Date: Nov 2009 Location: Michigan Posts: 135 Rep Power: 9 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.

 July 18, 2011, 03:58 #4 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,236 Blog Entries: 1 Rep Power: 18 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

 July 18, 2011, 14:02 #5 Senior Member   Join Date: Nov 2009 Location: Michigan Posts: 135 Rep Power: 9 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(const word&) const in file /home/opencfd/OpenFOAM/OpenFOAM-1.7.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 139. FOAM aborting

 July 18, 2011, 14:12 #6 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,236 Blog Entries: 1 Rep Power: 18 use a boundary like this patchName { type fan; patchType cyclic; f List 1 (2); // put ur value difference here value uniform 0; }

 July 18, 2011, 17:28 #7 Senior Member   Join Date: Nov 2009 Location: Michigan Posts: 135 Rep Power: 9 Its working. I was using the boundary condition for fan as: type fan; patchType cyclic; f List 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!

 July 18, 2011, 17:50 #8 Senior Member   Join Date: Nov 2009 Location: Michigan Posts: 135 Rep Power: 9 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.

 July 18, 2011, 21:24 #9 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,236 Blog Entries: 1 Rep Power: 18 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.

 July 18, 2011, 22:10 #10 Senior Member   Join Date: Nov 2009 Location: Michigan Posts: 135 Rep Power: 9 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

 July 19, 2011, 15:06 #11 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,236 Blog Entries: 1 Rep Power: 18 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

 June 3, 2014, 11:48 Error mapping p #12 New Member   Dominik Pöltl Join Date: Jul 2013 Location: Hamburg Posts: 16 Rep Power: 6 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 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(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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post leejc OpenFOAM 2 July 15, 2016 04:17 brahim OpenFOAM Running, Solving & CFD 3 July 17, 2011 21:23 doubtsincfd OpenFOAM 0 July 12, 2011 18:02 Ivo OpenFOAM 1 July 30, 2010 11:22 hjasak OpenFOAM Running, Solving & CFD 10 April 16, 2010 15:35

All times are GMT -4. The time now is 00:54.

 Contact Us - CFD Online - Privacy Statement - Top