2018-07-16 16:56 BST

View Issue Details Jump to Notes ]
IDProjectCategoryView StatusLast Update
0002900OpenFOAM[All Projects] Bugpublic2018-04-13 09:35
Reporterpiu58 
Assigned Tohenry 
PrioritynormalSeveritymajorReproducibilityalways
StatusclosedResolutionno change required 
PlatformIntel-PCOSWindows OS Version10
Product Version 
Target VersionFixed in Version 
Summary0002900: wall get transparent for flow: buoyantBousinesqPimpleFoam and boussinesqPimpleFoam
DescriptionThe solvers are designed to calculate flow from heated (or cooled) surfaces. In these cases there is a strong flow away from the boundary, because of the gravity effects. The solver calculates nonsense, if they are strong velocity in the near of walls which have an external reason (no temperature).

The easiest case I could establish is a vertical wall which is heated at the lower part and has average temperature in the upper part. The flow gets accelerated by the temperature effect in the lower part. In the upper part we have a free flow without temperature effect, which leads to strange effects just above the temperature boundary. I used a plate of 5 cm and a free flow region of 5 cm too.

I reported the case en d├ętail at CFD online: https://www.cfd-online.com/Forums/openfoam-solving/200031-buoyantboussinesqpimplefoam-conservation-mass-violated.html#post688536

Please look at the images which I add.
Steps To Reproduce- Establish a case with a vertical wall
- lower part with high temperature
- upper part with normal temperature
- let it run until it stabilizes

At the region just above the temperature limit there is a region where the flow moves through the wall.

Additional InformationI used also a flow past a sphere which gives a similar effect. The effect is much stronger if external flow is added.
TagsbuoyantPimpleFoam
Attached Files

-Relationships
+Relationships

-Notes

~0009481

piu58 (reporter)

I added a case for buoyantPimpleFoam which I run last. I give a result fro t=10s in the folder E10. Rename it to "10" if you wish to see it with paraFoam.

~0009482

henry (reporter)

It sounds like you are using inappropriate boundary conditions, do you see the same problem in the tutorial cases? If not can you reproduce the problem by changing a tutorial case and if so what is the minimum change required?

~0009483

piu58 (reporter)

The tutorial case assumes that the high temperature is at the floor. It is not worthwhile to modify it so the high temperature is at the side wall. The case I give is very simple, just a rectangle.

I don't believe that I mixed something with the boundary conditions.

I used another case which is very clear, flow past a cylinder like here

https://www.openfoam.com/documentation/tutorial-guide/tutorialse3.php

I set:

- uniform temperature, no effects of buoyancy, but a flow past a cylinder, and therewith
- Usage of buoyantBoussinesqPimpleFoam as a pimpleFoam solver (which should work)

I observed:
- The start of the simulation is cumbersome, the first rounds take a lot of time
- The region with strange effect evolves immediately, and occurs in the middle the downstream site of the cylinder. Again, Flow through the wall.

The same case, started with pimpleFoam works.
You find at the downstream region of the sphere a few cells where the flow goes "outward". Th same case works, if pimpleFoam is used.

~0009484

piu58 (reporter)

I added the cylinder case. In the case there are the two results at t=0.005s. At this time this laminar simulation is stable.

~0009485

henry (reporter)

> The tutorial case assumes that the high temperature is at the floor. It is not worthwhile to modify it so the high temperature is at the side wall.

Why not? I would assume this is easy to do.

~0009486

piu58 (reporter)

If that is of worth for you, I'll do it and write again here.

~0009487

wyldckat (updater)

I've taken a quick look into the first case and here are the problems:

1- The case was configured to run with OpenFOAM 3.0.*. This version is no longer supported, unless if there really was an error that was reproducible with OpenFOAM 5 and/or OpenFOAM-dev.

2- 'buoyantPimpleFoam' uses the "p" field as the "real" pressure field for initializing, which means that this case it suffering from a sort of pressure collapse, because "p_rgh" is reset to "p - rho*g*h".

3- The pressure boundary in "p_rgh" on the wall is not advised... zeroGradient is not properly handled and it's preferable to use the same configuration as in the tutorial cases, e.g.: https://github.com/OpenFOAM/OpenFOAM-5.x/blob/master/tutorials/heatTransfer/buoyantPimpleFoam/hotRoom/0/p_rgh

4- Similarly, the "p" field does not have the suggested/advised boundary conditions: https://github.com/OpenFOAM/OpenFOAM-5.x/blob/master/tutorials/heatTransfer/buoyantPimpleFoam/hotRoom/0/p


Nonetheless, it should still be worthwhile to confirm if having a hot surface on a wall instead of the floor, based on the respective 'hotRoom' tutorial case, to confirm if it simulates properly or not.

~0009488

piu58 (reporter)

Dear Henry and Bruno,

thank you for your hints. I assume that I need to understand more of the connection between p p_rgh and gravity. I try to change my cases in the way you proposed.
Before I do this I'll modify the hot room example in a way that it comes close to my vertical wall. I think that I find the time in the next one or two days.

Unfortunately, I have only access to a version which you describe as 3.0. It is one of the newer version which are given from CFD support. Their releases are counted by the year the were released, I have 17.02.

Thank you for your help, Uwe.

~0009495

piu58 (reporter)

Good morning,

I experimented with hotRoom and my vertical wall Using the b.c. form hot room the strange effects at my wall (at the temperature boundary) disappeared. Henry was right pointing me at the boundary conditions.

The remaining problem is an external flow calculated with zip file buoyantBoussinesqPimpleFoam. I changed my flow past a cylinder so that all b.c. are equal the ones of the hot room (ErrorBuoyantBoussinesqPimpleFoamV2.zip). Nevertheless, there the problematic region at half height at the downstream side remains: A huge increase of velocity and a streaming outwards. Of course, buoyantBoussinesqPimpleFoam is not a solver for external flow. But I need a combination of temperature driven and external flow, so that effect is very annoying.
--
Uwe.

~0009496

henry (reporter)

User support request
+Notes

-Issue History
Date Modified Username Field Change
2018-04-12 08:50 piu58 New Issue
2018-04-12 08:50 piu58 File Added: 5.jpg
2018-04-12 08:50 piu58 Tag Attached: buoyantPimpleFoam
2018-04-12 08:57 piu58 File Added: ErrorBuoyantPimpleFoam.zip
2018-04-12 08:58 piu58 Note Added: 0009481
2018-04-12 09:21 henry Note Added: 0009482
2018-04-12 11:01 piu58 Note Added: 0009483
2018-04-12 11:45 piu58 File Added: ErrorbuoyantBoussinesqPimpleFoam_Cylinder.zip
2018-04-12 11:45 piu58 Note Added: 0009484
2018-04-12 11:52 henry Note Added: 0009485
2018-04-12 12:07 piu58 Note Added: 0009486
2018-04-12 12:38 wyldckat Note Added: 0009487
2018-04-12 13:45 piu58 Note Added: 0009488
2018-04-13 09:23 piu58 File Added: ErrorbuoyantBoussinesqPimpleFoam_CylinderV2.zip
2018-04-13 09:29 piu58 Note Added: 0009495
2018-04-13 09:35 henry Assigned To => henry
2018-04-13 09:35 henry Status new => closed
2018-04-13 09:35 henry Resolution open => no change required
2018-04-13 09:35 henry Note Added: 0009496
+Issue History