Droplets and CFX
 

Hello im new in this Forum and to begin with i want to excuse my bad english.
So now to the problem i would like Help with.
Im working with CFX for about 8 weeks, so im fairly new.
Im simulating multiphasic microchannel flows for my masterthesis.
My main problem is, that i want to simulate the formation of a Droplet on a microslot for benchmarking purposes. I choose the settings like it was stated in the Help and tutorials as well as it was stated in several papers.
So after 6 weeks of trying im at my wits end.
The simulation works, the interface between the two immiscible phases is created and the second phase flows into the first one,, but as soon as i activate the continuum surface force (the mainly active Force for this simulation) the flow that should be present stops as soon as the Interface between the fluids is established.
Hope somebody can help with my Problem

Is this what you are asking - your model works fine without surface tension, but as soon as you activate surface tension it does not accurately model the flow?

Also an image of what you are getting and what you expect would help to understand the problem.

OK how to explain ... the Model works neither way.
But if i do not use Surface Forces, the expectet Flow begins to form but it simply only fills the channel without forming a droplet/bubble what it should, but without using surface Forces that is to be expectet.
If i activate the Surface Forces the flow does not work, i already tried to use normal flor or mass flow, but for both there is no growth of a droplet, you only see a interface developing and then it stays this way.
My expectation is that there should form a droplet, and after a short time there should form a neck when it separates from the inlet channel.
As For pictures:
This is the starting condition, with Surface forces it simply stays this way, besides that there will develop an interface.
http://s1.directupload.net/images/130503/u2lxxcp3.jpg

As For without Forces the following is developing, but it simply grows in size where there should be a separation:
http://s14.directupload.net/images/130503/sx5labqa.jpg


Edit: For benchmarking Purposes i try to model the same as in the Following paper:
"CFD analysis of microchannel emulsification: Droplet generation process and size effect of asymmetric straight flow-through microchannels"
Authors:
Isao Kobayashi and Goran T. Vladisavljevic and Kunihiko Uemura and Mitsutoshi Nakajima

The Purpose is to show that we can get similar results with ansys so that i can use it for modeling purposes of my Ma.Thesis

Can you post your CCL?

Hope that it works with this, its the simulation im actually running, but this time im using static pressure at the inlet instead of a mass or normal flow.

Ps in cas the attachement did not work i have uploaded it to
http://www.file-upload.net/download-...oplet.ccl.html

You have modelled this as a eularian multiphase model, as sub-grid droplets in a continuous fluid. This is not an appropriate model for what you are doing - you should model this as a free surface model. Have a look at the tutorial Free surface flow over a bump for how to set up a free surface simulation.

Hmm ... thank you i will look into it... im pretty sure i lokked through that tutorial, well i always wondered why ansys wanted Droplet sizes for a simulation that should determine the size...

Still not working
 

Well i tried som Variations of the Analysistype you suggested me ... took some time.
There was a large pressure drop at the Connecting region of the meshes so i tried a one Domain Simulation.
And now here is my Problem, if i Use the flow rates specified in the paper nothing happens, so i used a mass flow with a much higher magnitude to see something happen, but still, the interface does not develop like it should and there are still no droplets to be seen, so im out of ideas for now perhaps you could help me again, if possible.

I have uploaded the CCL again, hoping that someone could again help me and may point out what has to be revised.

Here a link to the CCL
flow2.ccl

Why is you initial timestep smaller than youir minimum timestep? Make the minimum time step 1e-8s and the maximum 1e8s. Let it find its own time step without you prescribing limits (unless you actually know a limit exists - then please describe why).

If the phases have a distinct interface for the entire simulation then use the homogenous model.

Do not adjust the surface tension settings unless you know a better setting. But I strongly recommend you do a test of all key free surface parameters and a sweep of key settings. You can often find a better setting than the default for free surface modelling, but you need to do a careful analysis to find it.

Also have a look at the coupled volume fraction solver. It may help - but not always, you need to test it.

Thank you for your answer i will test it.
But one Question is there a Cause why the homogenous model works better?
Well it should have a distinctive interface but i do not really see why to use it, cause in my understanding if you use a homogenous model the cells will be seen as homogen so the movement of the fluids in both ways does not really seem to matter even tough i think it should...
Well or it is simply a problem of understanding on my side, as mentioned im still trying to grasp the basic princibles behind.

Read up about homo- and inhomogeneous. The difference is whether they have a shared velocity field or not. If the homogeneous model is approriate it will run faster (less equations) and with better convergence.

Ok ... i stopped the Simulation early, after 3 days of computing to see what happened and it seems that the Timestepping did the trick on that one ... so let me again thank you for your Help.