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

Translational Periodic Boundary Conditions

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 5, 2012, 22:55
Default Translational Periodic Boundary Conditions
  #1
New Member
 
Join Date: Jul 2012
Posts: 11
Rep Power: 4
HeatTransferFan is on a distinguished road
Hi,
I am trying to model flow an heat transfer over a pin fin (a cylinder with a thin base underneath it) with translational periodic boundary conditions in the flow direction, and symmetry conditions in the cross-flow direction. I have found in the Help section how to define these periodic boundary conditions by creating a periodic interface however, I have not found any tutorials that actually use it. Anyway, I meshed my domain in such a way that the two faces have matching meshes and started with a coarse mesh and laminar flow. I also specified a mass flow rate across the fluid domain. However, I have ran already close to 1000 iterations and the solution has yet to converge. Is there something specific that I have to do in terms of meshing or other settings to get my solution to converge for these conditions? Can anyone suggest a tutorial or an example that uses similar conditions? Do periodic boundary conditions usually mean that the convergence will be slower?
Thank you for your help,

Krsto
HeatTransferFan is offline   Reply With Quote

Old   August 6, 2012, 05:51
Default
  #2
New Member
 
Join Date: Jul 2012
Location: Germany
Posts: 23
Rep Power: 4
bratzinger is on a distinguished road
Hi
my experience is that in these models the convergence is slower and sometimes not that good.
but the important point in periodic models with heat transfer is the heat sink without destroying your temperature layers in the fluid towards the solid domain. without it your fluid gets hotter and hotter. so with the 1st law of thermodynamics u can create a expression + the variable for cell size- and massFlow-based heat sink (update: the sum of the "cell-heat-sinks" equals your total heat sink and is based on your deltaTemp/period if u choose const. heat flux). just add another term with a relaxing factor to regulate the "inlet"-temperature towards your desired temperature

Last edited by bratzinger; August 6, 2012 at 08:32.
bratzinger is offline   Reply With Quote

Old   August 6, 2012, 05:57
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
started with a coarse mesh and laminar flow.
A common beginners mistake is to assume laminar flow is simpler to use than using a turbulence model, and is therefore suitable to start out. If the flow is turbulent in fact the opposite is true - using a laminar model will make the flow harder to converge as you are not modelling the turbulence which is required to keep the flow stable. If the flow is turbulent then use a turbulence model right from the start.

Other than that, try this FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

And bratzinger's point is important - you need to make both the momentum and heat equations periodic. That means at the periodic boundary you take out of the flow the same amount of heat you put in the domain.
ghorrocks is offline   Reply With Quote

Old   August 6, 2012, 07:25
Default
  #4
New Member
 
Join Date: Jul 2012
Location: Germany
Posts: 23
Rep Power: 4
bratzinger is on a distinguished road
another point is that u have to consider the solid domain boundary influence on your periodic model. it could be necessary to model 2 or more periods and then evaluate the middle one. if you e.g. define a const. heat flux for calculating the "thermal Resistance", there also should be the same temp. (gradients) at the end of the solid/fluid domain - just with a "deltaTemp"

Last edited by bratzinger; August 6, 2012 at 08:38.
bratzinger is offline   Reply With Quote

Old   August 6, 2012, 14:46
Default
  #5
New Member
 
Join Date: Jul 2012
Posts: 11
Rep Power: 4
HeatTransferFan is on a distinguished road
Thank you for the help.
As you might have guessed, I am quite new to CFD. I have a solid knowledge of Fluid Dynamics but in terms of software I am quite new.

Quote:
Originally Posted by ghorrocks View Post
A common beginners mistake is to assume laminar flow is simpler to use than using a turbulence model, and is therefore suitable to start out. If the flow is turbulent in fact the opposite is true - using a laminar model will make the flow harder to converge as you are not modelling the turbulence which is required to keep the flow stable.
ghorrocks that was actually a question in general about CFD, whether a laminar flow solution would work with a turbulent flow. In this case, I choose the mass flow rate such that the velocity is low and the flow is laminar. The question is, since there might be separation, should I still use a turbulent model? I selected the velocity such that Re_D is about 1300 which should be laminar.

Quote:
Originally Posted by bratzinger View Post
so with the 1st law of thermodynamics u can create a expression + the variable for cell size- and massFlow-based heat sink (update: the sum of the "cell-heat-sinks" equals your total heat sink and is based on your deltaTemp/period if u choose const. heat flux). just add another term with a relaxing factor to regulate the "inlet"-temperature towards your desired temperature
Bratzinger, thank you for your help. In fact I had some questions about the heat transfer part. The point is that if you have a heat flux condition at the bottom of the heat sink and a periodic boundary condition in the fluid and solid, now the temperature in the system is not set and will depend on where in the actual heat sink you are (the overall behaviour is determined up to a constant). With a constant bottom temperature the temperature in the system is actually set. I tried both but it did not make much of a difference in term of convergence. I am not sure how to set a specified temperature increase in the system. I can use Q=m_dot*cp*DT to calculate the temperature increase DT in the system, however I am not sure where I can input that. I set periodic boundary conditions on the solid part (as a solid solid periodic interface) but that's it. How can I specify the DT?

Also, I get a warning "In Analysis 'Flow Analysis 1' - Domain Interface 'Fluid Periodic': A Mass and Momentum model is only valid for periodic interfaces if all fluids have constant density" that I am not sure how to deal with. I don't have a problem with this because the flow is incompressible. Should I just not worry about it or could it affect my convergence? Can I set the flow to be incompressible?

Thank you both for your help,

Krsto
HeatTransferFan is offline   Reply With Quote

Old   August 6, 2012, 19:01
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If the flow is laminar then you have done the correct thing to choose the laminar model. Separations are not turbulence, they are a different thing. You can have separations in laminar or turbulent flow.

Quote:
now the temperature in the system is not set and will depend on where in the actual heat sink you are
Yes, so if you cannot approximately this sufficiently well with the periodic assumption then the flow is not periodic and this approach is not valid.
ghorrocks is offline   Reply With Quote

Old   August 7, 2012, 03:29
Default
  #7
New Member
 
Join Date: Jul 2012
Location: Germany
Posts: 23
Rep Power: 4
bratzinger is on a distinguished road
Quote:
Originally Posted by HeatTransferFan View Post
Thank you for the help.


The point is that if you have a heat flux condition at the bottom of the heat sink and a periodic boundary condition in the fluid and solid, now the temperature in the system is not set and will depend on where in the actual heat sink you are (the overall behaviour is determined up to a constant). With a constant bottom temperature the temperature in the system is actually set. I tried both but it did not make much of a difference in term of convergence.

I am not sure how to set a specified temperature increase in the system. I can use Q=m_dot*cp*DT to calculate the temperature increase DT in the system, however I am not sure where I can input that. I set periodic boundary conditions on the solid part (as a solid solid periodic interface) but that's it. How can I specify the DT?

Krsto
  • i guess u already calculated what dT the fluid should have as it flows from "inlet" to "outlet" (side 1 and 2/const heat flux)
  • fluid domain boundary conditions:u can create global variables that reference to all cells -> heatsinkvar(add variable with unit W m^-2/tensor scalar and defined in fluid as->)= Velocity u * cp * rho *(DT+(DT:MassflowAve(Temperature)@Inlet-desiredTinlet)*RelaxationFactor) and then this variable is your heat-sink-flux-expression in periodic side 1 (or 2 )
  • solid domain boundary conditions: got problems with modelling these in a very short periodic model with my geometrie(tried serveral things). so i made them adiabatic, "said"/guessed that heat convection is dominant to heat conduction, created 2 or more periods(e.g. mirror the mesh in pre ) and then evaluated the middle one(its still way faster than simulating the hole geometrie). after a first run i checked if i was right and checked the gradients(->variable) and temperature profiles by hand, i mean eye ^^, through looking at there contour lines who should also be periodic(if there is a DT u can create a relative temperature via expressions that is displayed by the contour)
Quote:
Originally Posted by HeatTransferFan View Post


Also, I get a warning "In Analysis 'Flow Analysis 1' - Domain Interface 'Fluid Periodic': A Mass and Momentum model is only valid for periodic interfaces if all fluids have constant density" that I am not sure how to deal with. I don't have a problem with this because the flow is incompressible. Should I just not worry about it or could it affect my convergence? Can I set the flow to be incompressible?

Krsto
in: materials -> thermodynamic state=liquid/the material only got a constant density
-> stil got the msg so i ignored it (havent found anything else)

Last edited by bratzinger; August 7, 2012 at 07:45.
bratzinger is offline   Reply With Quote

Old   August 29, 2012, 07:57
Default
  #8
New Member
 
Nils Schueler
Join Date: Jul 2012
Location: Munich
Posts: 11
Rep Power: 4
rasko is on a distinguished road
Hello Krsto,

did you already manage to get your solution converging? If not you might try to adjust the Pressure Update Multiplier (you can find it at Outline -> Interfaces -> periodic (or whatever might be the name for your periodic BC) -> Additional Interface Models). My solution didn't converge until I set a much smaller value (for me: 0.02) than the default one. But that probably depends strongly on the problem. For more informations you might search the documentation for Pressure Update Multiplier.
rasko is offline   Reply With Quote

Old   September 11, 2012, 22:25
Default
  #9
New Member
 
Join Date: Jul 2012
Posts: 11
Rep Power: 4
HeatTransferFan is on a distinguished road
Rasko,
I ended up giving up on the heat transfer part and just simulating isothermal periodic flow with a fixed mass flow rate. It worked really well and converged fast. I moved on to something else but I plan on coming back to the heat transfer part. I think using a heat source in the solid would be the best way but I haven't tried yet. I'll keep you posted.
Thank you everyone for your help,

Krsto
HeatTransferFan is offline   Reply With Quote

Old   September 19, 2013, 12:08
Default Translational or general connection?
  #10
Member
 
Hesam Moghaddam
Join Date: Mar 2012
Posts: 49
Rep Power: 5
hesamking is on a distinguished road
Hi all,
I am trying to simulate a blast-like situation by using two domains connected through an interface.
The first domain is initialized with 100 psi pressure and the following (low pressure) one is initialized with ambient pressure (14.7 psi). When the transient simulation runs (for 5 ms), the pressure releases from the high pressure domain and goes into the other one. I have a head model in the low pressure domain and I want to see the flow around head.
My question is that for such a situation, do you recommend general or translational connection between the two interfaces?
by the way, should i make my domain large to remove the effects of the wall? because I have tested both small and large domains (where the walls are close to the head or far away from the walls)
Thanks,
Hesam
hesamking is offline   Reply With Quote

Old   September 19, 2013, 18:05
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
A few points:
1) There is no need to do this as a multi-domain simulation. A single domain with an initial condition sounds like it will do it. Then there is no need for an interface.
2) Do you need to model the high pressure reservoir? Why not just model a pressure boundary at the high pressure?
3) I assume for your comment you are looking to model the head being hit by a shock wave in a far field (ie far away from walls). In that case do a sensitivity study on boundary proximity to check your walls are far enough away to approximate a far field.
ghorrocks is offline   Reply With Quote

Old   September 20, 2013, 13:12
Default
  #12
Member
 
Hesam Moghaddam
Join Date: Mar 2012
Posts: 49
Rep Power: 5
hesamking is on a distinguished road
Hi ghorrocks,
Thanks for the ideas.
Actually I have used this approach but besides coming up with overflow error,
It gives out weird pressure distribution inside the domain and on the head...
When I use two different domains, the fluid flow and distribution inside the domain and around the head is much more similar to the real blast-like (shock wave) situation I have done inside Ls-Dyna.
I know that for now Ansys CFX can not simulate blast fluid flow but do you have anything in mind about simulating the blast situation via CFD so we can see the fluid flow?
Thanks,
Hesam
hesamking is offline   Reply With Quote

Old   September 21, 2013, 06:20
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
CFX certainly can simulate blast flows.

You would have to show me what you intend to model before I can comment on the best way to model it. Please post an image and a description.
ghorrocks is offline   Reply With Quote

Old   September 21, 2013, 16:49
Default
  #14
Member
 
Hesam Moghaddam
Join Date: Mar 2012
Posts: 49
Rep Power: 5
hesamking is on a distinguished road
Ghoroocks,
Are you sure? Because I haven't found anything blast-wise that have been done using CFX; no article, example, tutorial , etc.
The modeling is exactly what you describes. I am studying the brain injury due to blast loading. The main task is being done using LS-Dyna. But we are trying to see the blast flow field around head and also under the helmet. Hence, we need to create blast situation to have an exact assessment of the fluid flow.
The meshing and BC are provided in the attached picsmesh.jpg

BC.jpg
hesamking is offline   Reply With Quote

Old   September 22, 2013, 07:15
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
CFX can model flows up to the hypersonic regime (normally around Mach 5). I have done much work on shock wave flow and reflections and you can get the results within under 1% to analytical results if you are careful. So yes, CFX can do what you are proposing.

And by blast do you mean including the chemistry of the explosion, or "just" a shock wave?
ghorrocks is offline   Reply With Quote

Old   September 23, 2013, 11:31
Default
  #16
Member
 
Hesam Moghaddam
Join Date: Mar 2012
Posts: 49
Rep Power: 5
hesamking is on a distinguished road
Thanks Ghorrocks,
Actually that's the problem. I knew that CFX can model supersonic flows( flows around airfoils) but it's the chemistry and mechanics of blast and explosion which is different.
Using Ls-Dyna or Autodyne you can notice that although Navier-Stokes equations are solved, the equations are different for blast resulting from a detonation at a fixed distance.
That' s what i haven't seen any commercial CFD software can do.
Based on this, what do you think is the best way to model my problem?
Thanks,
HesaM
hesamking is offline   Reply With Quote

Old   September 23, 2013, 18:41
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I cannot say what is best. All I can say is it sounds like CFX can model this also if you wish. You will have to work out which is best.
ghorrocks 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
periodic boundary conditions fro pressure Salem Main CFD Forum 21 April 10, 2013 00:44
Periodic boundary conditions in 3D Eulerian granular flow simulations dsm FLUENT 4 March 2, 2012 20:04
Problem with using periodic boundary conditions Sun FLUENT 0 January 14, 2011 10:47
periodic boundary conditions mranji1 Main CFD Forum 4 August 24, 2009 23:45
How to apply a periodic boundary conditions ck1973 FLUENT 2 July 4, 2006 01:27


All times are GMT -4. The time now is 09:56.