Domain interface: translational periodicity for Multiphase flow
Hello
Does anybody know if the translational periodicity is properly implemented in ANSYS CFX 13.0 for Multiphase flows? Thanks in advance Milan 
I know of no limitation in translational periodicity. Periodicity is numerically implemented by simply mapping the variable values at one side of the periodic boundary to the other, so numerically it is very simple and adding things like multiphase does not complicate things.

Sounds logical...
I was asking because I read a post in a forum (unfortunately I don't remember where) that a guy was having problems with mass imbalances in multiphase flow using periodic interfaces. He/she contacted CFX technical support and they told him/her that periodicity is not supported for multiphase flow. Thanks Milan 
I am not sure about lagrangian particle tracking and periodic interfaces  I think they work but I am not sure.
But I am pretty confident eularian multiphase is OK with periodic interfaces. There might be some unusual case I have not thought of but in general it should be fine. 
hmm. interesting.
wonder if this is 1:1 periodicity or a GGI on the periodic. 
1:1 or GGI should make no difference. 1:1 just means it can be directly mapped over and GGI means it needs an intermediate interpolation step, but conceptually it is the same.

it used to be multiphasecht was not supported by the GGI interface, but the 1:1 was ok. I checked the v140 solv doc and it is fully supported now (don't have v130 docs)
there are always some type of GGI issue in the errata for most of the advanced models, mostly due to the discretization. CFX201023 is a good example. 
Thank you all for your feedback
I am performing a transient "2D" simulation of an oil droplet in water through a rectangular channel, using translational periodicity on the inlet and outlet, symmetry conditions on the side walls, and no slip wall in the upper and lower walls. I impose a pressure gradient on the domain and an initial velocity distribution and volume fraction (to model the initial position of the droplet). This is to model the deformation and breakup of the droplet. While doing that I got some basic questions (maybe trivial?) about the general modeling of twophase flow with CFD methods (not strictly related with the problem mentioned above): 1.The use of an homogeneous model with free surface and a very fine mesh should capture properly the physics of the problem as good as the use of a mixture model with free surface with a coarse mesh?. According to my understanding the mixture model uses separate conservation equations for each fluid and specifies for a cell with two fluids a momentum exchange between them. For a very fine mesh (where the volume fractions of a phase in an element are very close either to 0 or 1) is this equivalent to using a homogeneous model where the momentum exchange between them is computed by the tangential and normal stresses on the elements boundary? 2.When using the particle model: what happens when the diameter of the particle is greater than the size of the element?. According to my understanding, the particle model assumes that one of the phases is organized in a particle shape and it calculates the momentum interfacial terms by using pre built correlations. What happens then when for example there is a big droplet that encircles e.g. a lot of elements? (Might be a fairly common case close to the walls where we have inflation). 3.When converting a problem of twophase flow in pipes (3D) to a 2D simulation. Assuming for instance stratified oil and water flow. I am simulating a plane that cuts the pipe vertically, passing through the axis along the flow. The content of oil and water of the 2D simulation is different than in the real 3D case. How good is this assumption?, for example for predicting layer height, phase velocities, etc. In 1D mechanistic models, or quasi 3D models it is possible to include the effect of the additional fluid in the integration of the cross section. Sorry for the long post. If anyone thinks that these questions should be posed in a different post/section, please notify me and I will move them. Milan 
1: You have to remember the basic assumptions behind the models. A homogenous free surface models assume the free surface can be resolved by the mesh. The inhomogenous mixture model assumes that there is bubbles/droplets at the subgrid length scale. You choose the model which is most appropriate for what you are modelling.
2: Mathematically, not much happens. Again, the fundamental assumption of the particle model is that the particle can be represented by a applying its momentum, temperature and any other affects at a point. If the actual particle is bigger than an element that is no importance at the macro scale, but obviously you won't have the micro scale flows (eg the flow around the particle modelled). 3: The accuracy of the assumption is problem dependant. Without further details we cannot say. 
Thank you Glenn for all your comments, now it is more clear
Going back to the 2D approximation of 3D multiphase flows: For Example I want to model stratified flow in a pipe, I have the volumetric flow rate of air (Qair) and the volumetric flow rate of water (Qwater). If I were using a 3D approximation: With these values I can calculate the non slip volumetric fractions of each phase at the inlet (assuming that the two fluids travel at the same speed). That would be alphaair=Qair/(QairQwater), and alphawater=Qwater/(QairQwater). The speed at the inlet would be Vmix=(Qwater+Qair)/Apipe. Now for a 2D approximation (a vertical cut of the pipe through its center along the axial direction), I would impose at the inlet the same mixture velocity as calculated before, but what volumetric fraction should I impose for the water and air? Thanks for your feedback Milan 
Can you post an image of what you are trying to model and the 2D model you propose to simplify it to?

2 Attachment(s)
This is a sketch of the 3D problem I am trying to model by using a 2D approximation:
Attachment 24116 The Inlet is the boundary condition, the outlet is the (calculated) equilibrium condition. I want to solve this 3D problem by using a 2D approximation: Attachment 24117 and I am asking about the inlet volume fraction that I should impose. I think that I have to use a volume multiplier that will capture the variable area of the pipe at each vertical position. How to do this in CFX? Regards Milan 
This looks very similar to the CFX tutorial "free surface flow over a bump". Have you looked at this tutorial example?

1 Attachment(s)
Hello
Thanks for the suggestion but the tutorial addresses how to set up the simulation, but it doesn't discuss the 2D approximation of 3D two phase flow. What I am addressing (or trying to) with my discussion is the following: If one wants to make a 2D simulation of a 3D stratified flow in a pipe, you have to consider the pipe thickness for each position along the diameter. See the figure below: Attachment 24210 Each position of the pipe has a different "storage" capacity (volume) (minimum in the up and down positions and maximum exactly at the center. In a 2D plane simulation of single phase fluid we neglect this storage capacity and assume that the distribution of tangencial stresses and velocities in this channel is a good representation of the real situation in a pipe. This difference in volume storage for each individual cell is very important in multiphase flow. for Example: Going back to the stratified flow case, assuming that the height of the water layer is increasing along the axial direction (from inlet to outlet). This height should increase quickly when the height of the water layer is relatively close to the lower wall, but is going to increase slowly when the water level is close to the center. If we neglect the effect of the pipe width, a 2d simulation will not capture this phenomenon. My two doubts are about:  how to provide this difference in volume in cfx for every cell and Which volumetric fraction to impose in the inlet boundary condition to represent the adequate amount of fluid flowing in the pipe. I hope it is a bit clearer now. Milan 
I see  the answer is simple  what you describe cannot be done. CFX uses the mesh to model the geometry directly and does not have the capability to have some form of coordinate transform on top of that. Some other software might, but none of the major commercial codes have this either to my knowledge.
Your flow is not 2D so you cannot use a 2D assumption. Your flow does have symmetry however  so you can use a symmetry plane. 
All times are GMT 4. The time now is 23:10. 