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 crossflow 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 
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 massFlowbased heat sink (update: the sum of the "cellheatsinks" 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 
Quote:
Other than that, try this FAQ: http://www.cfdonline.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. 
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"

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:
Quote:
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 
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:

Quote:
Quote:
> stil got the msg so i ignored it (havent found anything else) 
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,
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 
Translational or general connection?
Hi all,
I am trying to simulate a blastlike 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 
A few points:
1) There is no need to do this as a multidomain 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. 
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 blastlike (shock wave) situation I have done inside LsDyna. 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 
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. 
2 Attachment(s)
Ghoroocks,
Are you sure? Because I haven't found anything blastwise 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 LSDyna. 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 
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? 
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 LsDyna or Autodyne you can notice that although NavierStokes 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 
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.

All times are GMT 4. The time now is 00:57. 