CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Translational Periodic Boundary Conditions (http://www.cfd-online.com/Forums/cfx/105659-translational-periodic-boundary-conditions.html)

 HeatTransferFan August 5, 2012 22:55

Translational Periodic Boundary Conditions

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

 bratzinger August 6, 2012 05:51

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

 ghorrocks August 6, 2012 05:57

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.

 bratzinger August 6, 2012 07:25

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"

 HeatTransferFan August 6, 2012 14:46

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 (Post 375560) 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 (Post 375557) 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

 ghorrocks August 6, 2012 19:01

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.

 bratzinger August 7, 2012 03:29

Quote:
 Originally Posted by HeatTransferFan (Post 375647) 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 (Post 375647) 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)

 rasko August 29, 2012 07:57

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.

 HeatTransferFan September 11, 2012 22:25

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

 hesamking September 19, 2013 12:08

Translational or general connection?

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

 ghorrocks September 19, 2013 18:05

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.

 hesamking September 20, 2013 13:12

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

 ghorrocks September 21, 2013 06:20

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.

 hesamking September 21, 2013 16:49

2 Attachment(s)
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 picsAttachment 25516

Attachment 25517

 ghorrocks September 22, 2013 07:15

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?

 hesamking September 23, 2013 11:31

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

 ghorrocks September 23, 2013 18:41

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.

 Shamoon Jamshed March 2, 2016 15:18

Hi Horrocks,

Can you help me with Fluent? Do you have experience with peridic flows in Fluent?

 ghorrocks March 2, 2016 18:12

Try the fluent forum: http://www.cfd-online.com/Forums/fluent/

 All times are GMT -4. The time now is 12:04.