[ghorrocks]

It is because there is a bug in your simulation set up. And you should run using a fast, coarse, 1:1 aspect ratio mesh to debug it and fix it.

[Danial Q]

One more thing I came across (from previous document of model) is grid independent meshing in this case. So, still 1:1 aspect ratio will work? or that will be totally different.

[ghorrocks]

I do not understand your last comment - but I presume it means you have some previous work in this area which suggests for you to use a certain mesh. You can try their mesh once the basic simulation is working. So use a coarse and even mesh to debug, then refine the mesh.

[Danial Q]

Yeah..a document regrading previous work about this model which describes grid independent mesh of 20 cells per initial radius of drop (20 micron). So, i was thinking that where to set this number of cells for meshing? I mean what parameter sets the number of cells....

[ghorrocks]

Do the meshing tutorials, or ask on the geometry and meshing forum.

But I will say it once again - forget running on a fine mesh until your model is running reliably and converging on a coarse mesh. You do debugging on a coarse mesh.

[Danial Q]

hmmm got your point about making simulation work first. But how would i know that what is root cause to problem, say liqNi entrance in domain as mentioned above, while i think physics is alright and i don't see any wrong with that.So, is it problem because of meshing or physics. or it is experience thing only...

[ghorrocks]

You need a mesh fine enough to at least resolve the features you are working on. Accuracy can come later, but for now having the flow do what you expect it to do is step one.

A problem about fine meshes is they can lead to very fine time steps and that means things happen very slowly. So you may have simply not run the simulation long enough.

[Danial Q]

I have set opening boundary for liqNi entering into domain with opening press & direction option selected ,relative pressure set to zero and velocity set to 100 m/s, temp 2000 K. so, with these opening conditions, i cant see anything stopping droplet (flow) entering/moving into domain. Do you think something is missing?

[p.galimutti]

Originally Posted by Danial Q

Yeah..a document regrading previous work about this model which describes grid independent mesh of 20 cells per initial radius of drop (20 micron). So, i was thinking that where to set this number of cells for meshing? I mean what parameter sets the number of cells....

Ok you are saying 'radius of the drop', but your simulation looks like a rectangular domain. I don't understand that. Looks like the paper you're looking at is having a different domain. BTW, grid independence is same as the mesh sensitivity analysis we've been talking about!

I asked in my previous post 'where you got the mesh parameters' from. You said you set them 'yourself'. Now you're telling something else!

I don't know what to say but you need to learn some basics!

I seriously doubt your bcs too. A velocity of 100 m/s in a 10e-4(X) length and almost half temperature of sun (2000 k) for liNi seems ridiculous! You know what happens to liNi at 2000K?

[Danial Q]

Well, let me make you clear about few things,

First : it is simulation of thermally sprayed metal coating powder, for which a single droplet is being studied (impact on other metal piece) so obviously its temp will be as high as 3000C normally and speed will be 120 m/s or more than that. And individual particle size of that powder is always in microns e.g.(10 0r 20 microns). So, as a science student ,you should start believing things from now on.

Second: When you asked about the mesh, that was obviously set by myself where i used sweep method, and the parameter which i am talking about now(20 cells/initial radius) is from some previous work.

Third: a rectangular domain means " to consider the surface tension effects in the presence of atmospheric air as this particle travels through air and impacts on metal piece. So, a rectangular domain is set in which air is present already and droplet travels through until hits and hence free surface is resolved".

As far as learning basics is concerned, ofourse I dont know much about Ansys and CFd as it has never been my area but now I have to do simulation for my experimental results so have to jump into .I hope it is all clear now.

Thanks

[ghorrocks]

Have you worked out how far you expect a 100 m/s drop (or what ever the speed was) to travel in the simulation time you have elapsed so far?

Also - you mention you are using surface tension - this severly restricts the time step which will work well, so you will need a very small time step. But with your unstable numerics it will need to be even smaller.

Also also - I have done sensitivity studies on mesh quality versus surface tension accuracy and found that aspect ratios of worse than about 1.5 are bad news (ie inaccurate). So in this case you definitely need to make your fluid domain 1:1 aspect ratio hexas. Forget about any mesh grading at all if you want the surface tension to be accurate.

[Far]

is there any physical explanation that why surface tension requires perfect hexas?

[ghorrocks]

Look in the CFX documentation for how surface tension is applied. The resolution of surface curvature and the application of the surface tension force along that surface gets tricky as the aspect ratio gets higher. And a simple sensitivity study of pressure inside a spherical drop versus mesh aspect ratio shows that even gently biased meshes (ie aspect ratios above 1.5) start getting significant errors in the Laplacian pressure of a drop.

It is a simple study to do and if you are using he surface tension model I strongly suggest you have a look at this issue so you understand it - it is a major restriction on surface tension models.

[Danial Q]

Have you worked out how far you expect a 100 m/s drop (or what ever the speed was) to travel in the simulation time you have elapsed so far?

Also - you mention you are using surface tension - this severly restricts the time step which will work well, so you will need a very small time step. But with your unstable numerics it will need to be even smaller.

Well, I did not perform my experiment yet but from the old document available, it is clear that after 1microsecond it hits the solid domain at interface(solid/fluid) if same physics and domain sizes are used. As I am replicating the previous model first, so have to follow the old data.
While time step is concerned, that was the reason, I was using that less than nano second(1e-10) timestep by employing the timestep option rather adaptive stepping.
But the problem is solidification and phase change data is not available in those documents which is the real deal. And it is mentioned that phase chnage is employed through Thermal phase change model (that is the part I don't really agree).
Thanks

[ghorrocks]

Given the small time and lengths scales of your model have you considered whether non-equilibrium phase change is significant? That is sub-cooling and related issues. I suspect you will find it probably is, and that completely changes the underlying physics of the process.

[Danial Q]

Well, there is subcooling phenomena present in theory but as I already said that documents did not tell anything about it and no such thing(subcooling) is employed in modeling . Modeling equations just solve the conduction HT, Mass momentum and VOF along with CSF to resolve surface tension and curvature of the droplet.
Assumption made are; constt surface tension, laminar flow, zero solid domain velocity, neglected tangential stressses at free surface, no viscous dissipation.

[Danial Q]

So far what I have concluded is, with very small timestep such as nanosecs, RMS/MAX courant number shows some value only for the very first iteration and then for rest of the simulation, it remains zero. It has some values through out the simulation only when the mesh is very fine containing more than 0.3 million elements/nodes.

Three Monitor points have been defined for all these simulations but simulation shows only two mostly but third ( which in all cases is solid Ni droplet bottom side temp, while thickness of solidNi droplet is 1um) remains invisible in solver. It only appeared when mesh was fine like 0.3million elements.

In all cases, Ni mass and volume fraction remained almost zero while monitor points showed reasonable and sensible behavior of temperature change in system.

Could you please comment that if it is just debugging to be seriously dealt or some other areas are root cause. Because i have tried almost everything I know by now.

Thanks

[Danial Q]

Any suggestions please???

[ghorrocks]

I have already said my suggestions many times on this thread and I will not repeat them again. I have nothing further to add.

[Danial Q]

hmmmm. thanks glenn. I appreciate your support. Do you see any contradiction in past few comments;

1. You need a mesh fine enough to at least resolve the features you are working on.
2. But I will say it once again - forget running on a fine mesh until your model is running reliably and converging on a coarse mesh. You do debugging on a coarse mesh.

Is debugging for surface tension and phase change possible with the coarse mesh??