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

BuoyantSimpleFoam solver crashes

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 11, 2008, 02:05
Default Its difficult for me to commen
  #1
Member
 
Prashant Ojha
Join Date: Mar 2009
Posts: 38
Rep Power: 8
prashant24983 is on a distinguished road
Its difficult for me to comment on your case. But in the case for buoyantSimpleFoam in the tutorial of OpenFOAM-1.5, you need to change internal pressure field (hotRoom/0/p)

internalField uniform 0;

To

internalField uniform 100000;

The case should work properly.

Goodday.
prashant24983 is offline   Reply With Quote

Old   October 11, 2008, 02:08
Default From the error output of your
  #2
Member
 
Prashant Ojha
Join Date: Mar 2009
Posts: 38
Rep Power: 8
prashant24983 is on a distinguished road
From the error output of your case, I would suggest you to check your k & epsilon. Hopefully, they are not set to zero.
prashant24983 is offline   Reply With Quote

Old   October 13, 2008, 02:41
Default Thank you for helping me out.
  #3
Member
 
Christian Lindbäck
Join Date: Mar 2009
Posts: 55
Rep Power: 8
christian is on a distinguished road
Thank you for helping me out. The tutorial case worked fine after modifying the pressure field. My own case runs now as well. In the User Guide it says that the type "calculated" has no data to specify. In fact, a value has to be added.

The problem I'm trying to solve involves a room with a number of air inlets and outlets as well as components which generates heat. So it's a problem involving buoyancy. I have a number of questions. I'm grateful for help in any of these questions:

1) In the buoyantSimpleFoam solver one solves for a scalar field called "pd" as wells for "p". Why is this?

2) In the tutorial, the boundaries have a "pd" type called "fixedFluxBuoyantPressure". What is this and where can I read more about this type to understand it?

3) In the tutorial, the boundaries have a "p" type called "calculated". Does this means it is calculated from "pd" and "rho"? But still, a value of this "calculated" type is requested to be input, why?

4) Talking about boundary conditions, I basically have a number of inlet and outlets where I know the volume flow. The remainder is walls. What would be the appropriate boundary conditions? I assume I could set the pressure at one of the outlets to 1 bar.

5) I want to impose a uniform heat flux on some of my boundaries. Is that done by setting a fixed gradient for T according to q = k*A*deltaT? I realise now that a gradient involves a distance, so maybe I'm wrong here?
christian is offline   Reply With Quote

Old   October 14, 2008, 05:12
Default Hi, Chrisitian, Q1) I haven
  #4
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 197
Rep Power: 9
mkraposhin is on a distinguished road
Hi, Chrisitian,

Q1) I haven't tried boussinesqBouyantSimpleFoam, but with boussinesq assumptions liquid density depends only on temperature rho=beta*T. bouyantSimpleFoam solver uses equation of state (perfect Gas only today) rho=f(p,T). So, as your liquid is air you can use both solvers

Q2) p=pd+rho*g*h

Q3) fixedFluxBuoyantPressure BC uses knowledge of field rho*g*h to update pressure field properly (thus, if vertical distance between two boundary faces centers c1 and c2 is h, then, p2-p1=(rho2-rho1)*g*(c2-c1)=(rho2-rho1)*g*h

Q4) What boundaries?. For what field? If boundaries for field p, then your answer is right

Q5) if you want to account only for molecular heat transfer, then q=-lambda*gradT, if you want to account for both molecular and advection heat transfer, then you can use formula q=alpha*(Twall-Tliq), where alpha is empirical coefficint. For heat transfer, have a look at patch definition for enthalpy (src/thermophysicalFunctions/basic...)

Q6) About division by zero: set 0.1 for k internal field and 0.01 for epsilon internal field
mkraposhin is offline   Reply With Quote

Old   October 14, 2008, 06:52
Default Thank you. Question 4 above
  #5
Member
 
Christian Lindbäck
Join Date: Mar 2009
Posts: 55
Rep Power: 8
christian is on a distinguished road
Thank you.

Question 4 above was badly expressed:

I know the volume flow for my 2 inlets and 4 outlets of the ventilated room. I set the velocity for my 2 inlets and 3 of the 4 outlets. For the last outlet I set an absolute pressure of 1 bar.

1) For a velocity inlet I normally use a zero pressure gradient. I have never been using the pd formulation before. What would be the appropriate boundary condition for p and pd for a velocity inlet?

2) p is of type calculated. Still OpenFOAM requests a value to be input. Why is this? I mean, pd is solved for and p is calculated as pd+rho*g*h. Could p be of any other type than calculated?

3) What is an appropriate boundary condition for p and pd at an outlet where I want to set the pressure to 1 bar absolute?

4) What is an appropriate boundary condition for p and pd for walls?

5) I want to impose a constant heat flux at some of my boundaries. I don't wish to consider any heat transfer coefficient, only add a heat flux to the temperature field at the boundary faces. How can this be done?
christian is offline   Reply With Quote

Old   October 17, 2008, 15:07
Default Hi Christian, I'm afraid I
  #6
Member
 
Kati Laakkonen
Join Date: Mar 2009
Location: Espoo, Finland
Posts: 36
Rep Power: 8
kati is on a distinguished road
Hi Christian,

I'm afraid I can't help you much further. I've struggled with same problems in a very simple case in 1.4.1, and I found that for flow inlet and outlets only mass flow rate based boundary worked. In 1.4.1 the boundary condition was massFlowRateInletVelocity for U, and for pressure I used fixedFluxBuoyantPressure everywhere, also on inlets and outlets. This BC should be used in boundaries where you would use zeroGradient in non-buoyant cases. I didn't manage to make any sort of fixed pressure boundary work. (Which of course does not mean that they would be impossible :-|).

The 1.4.1 buoyantFoam did not require pd field. New one reads it from a file, and uses that field to set p. p is not explicitly read, it is set by thermo library. Maybe the library wants to have the file p.

One more thing: I also didn't have much success with buoyantSimpleFoam, but buyantFoam worked nicely with mass flow rate BC's. Many buyant cases are inherently transient, so try using the transient solver first.

I hope this helps.

Kati
kati is offline   Reply With Quote

Old   October 28, 2008, 07:03
Default I have 2 inlets (for which I s
  #7
Member
 
Christian Lindbäck
Join Date: Mar 2009
Posts: 55
Rep Power: 8
christian is on a distinguished road
I have 2 inlets (for which I set the velocity and leave the pressure as a zero gradient) and 4 outlets. I ended up with a successful buoyantSimpleFoam computation using the totalPressure boundary condition for both p and pd. I set the velocity for 3 of the 4 outlets and used totalPressure for the fourth. The other 3 used the fixedFluxBuoyantPressure condition. Right now I'm running with all four outlets set to totalPressure. There seems nufortunaltely to be a convergence problem for the pd equation although the flows going in and out of the domain looks ok. I will try running buoyantFoam.
christian 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
BuoyantSimpleFoam amitshah OpenFOAM Running, Solving & CFD 4 June 3, 2009 06:04
Solver crashes (PVM parallel) Marco Müller CFX 2 February 4, 2009 03:51
Instability in buoyantSimpleFoam smehdi609 OpenFOAM Running, Solving & CFD 1 August 20, 2008 15:38
Error in buoyantSImpleFoam solver antopnieta OpenFOAM Running, Solving & CFD 2 January 18, 2008 08:30
Solver crashes only while writing a bak file hagupta CFX 1 April 11, 2006 18:10


All times are GMT -4. The time now is 04:25.