[ghorrocks]

Yes. If your full domain is too big then just cut out a section and model a single drop. So if a coarse is no good then use a fine mesh but of only a small region. Anything so you can get it to run fast, but model the necessary physics.

[Danial Q]

Thanks again. So, "cut a section" means by using geometry module or meshing/solver offers you option to model only a section of whole model. Sorry for stupid question but I cant help it; its learning nad time saving.

[ghorrocks]

No problem.

So if your full simulation has 100 drops in a domain 100um x 100um, then maybe model 2 drops in 5um x 5um. Use DesignModeller (or any other modelling package) to chop out a relevant bit. That will run nice and fast.

[Danial Q]

aaaaah, I told you that I am already modeling a single drop.
And could you please point out any wrong in this settings for surface tension and free surface/vol.fraction;

liquid = step((rdrop-dist)/1[mm])
dist = sqrt((x - (5e^-3) [mm]) ^2 + (y - (5e^-3) [mm]) ^2 + (z - (3e^-2) [mm]) ^2)
rdrop =(20e^-3) [mm]
surface tension = 1.78N/m^1 (CSF MODEL), Vol weighted smoothing type, 0.25 relaxation factor
Vol fraction of liquid = liquid (shown above)
Vol fraction of air = 1-liquid
opening initial BC >> Vol.Fraction (Air) = 1, Vol Fraction (liquid) = 0
I could not find any wrong so far but Avg scale values for V.fraction of liquid is still zero.

[ghorrocks]

Sorry, I forgot that. I am running too many conversations at once to remember all the details.

If you are running a single drop then try a smaller single drop Anyway which makes it smaller.

But I think I see a problem. Your dimensions are all in the form (5e^-3)[mm]. I do not know what CFX resolves that too but i suspect it is nto what you want. Specify your dimensions in the form 5 [micron] or 0.005 [mm] to be absolutely sure.

Am I correct in saying that you have specified an initial condition with a big blob in the middle of the domain, but the blob does not appear? If you have said that before then I apologise for missing it but that completely changes things. In this case it simply means you specification of the initial conditions is wrong - and I think the units bug I mention above might explain it.

[Danial Q]

"Am I correct in saying that you have specified an initial condition with a big blob in the middle of the domain, but the blob does not appear? In this case it simply means you specification of the initial conditions is wrong - and I think the units bug I mention above might explain it."

I will correct the expression as you mentioned and check if it makes some reasonable difference. No, I have defined droplet near symmetry boundary (not at wall and not even at centre).


Thanks

[Danial Q]

Could you please explain that how does it make a difference to set up physics when blob is defined at centre of domain or away from centre somewhere?? Because what parameter defines its coordinate position? I did not find any in cfx pre. Sorry, in last post where I mentioned symmetry plane, i defined monitor points on it.

Secondly, I tried simulation with mesh aspect ratio 1 with 0.2 million elements and time steps so small as 1e-10 s. But still that cliping and temp out of range NOTICES showing up. Should i decrease timestep more and more untill warnings dont show up naymore or at some point try to refine mesh a bit more.
Any suugestions...

Thanks

[ghorrocks]

After seeing your CEL I think you have just incorrectly specified the initial conditions. Your numbers of the format (5e^-3) [mm], which I suspect you intend to mean 5 micron could evaluate to a strange number - maybe 5^-3[mm] = 0.008[mm] or 8 micron. Not sure if this is how CFX will evaluate it, but it looks like a mistake waiting to happen to me.

So re-write your CEL in the tradition format before doing any further simulations. If you want it to be 5 microns, then use 5[micron] as the unit. That way there is no possible confusion.

[Danial Q]

I have already corrected it to 5* 10^-3 [mm]. I think this format should be OK.

Thanks

[ghorrocks]

But what does that resolve to? If your initial condition still does not appear correctly I think it is still wrong. Just directly specify it as 5 [micron].

[Danial Q]

Yep this time, it is directly mentioned in microns and initial coordinates for droplet have also been set near symmetry as "dist" expression. Thanks for the hint though...Well, how would it change the physics setup except the dist expression if droplet is defined at centre, any physcis change seems unnecessary to me, m i right??
well this time it started well, otherwise it gave me notices from very beginning..I hope it goes well now and resolves to some reasonable value..

Thanks

[Danial Q]

How much courant number values ( Max & RMS) act as indicator for solution convergence. Because what i have concluded that it has nothing to do with solution convergence untill unless these values are too small.In my case, after 10 iterations these values become zero, does not matter what time step size is. Is it serious problem or I sould let the solver run while convergence criteria is obtained well.
second, well, i have tried different time steps as low as 1 *10^-12 sec, but instability remains at start for radius 20 microns while if radius becomes 10 microns even 1*10^-7[s] does not show unstability but gives courant number values zero. So, what is your opinion whether should i try more smaller time steps ??

Thanks

[ghorrocks]

I do not use the courant number options in CFX much. Often it does not mean much for a flow as CFX is an implicit solver and is not limited to a specific Courant number.

Can you post your CCL, an image of what you are trying to do and an image of your initial conditions? You might have done this already but that was long ago

[Danial Q]

As you remember, I am modeling a single droplet which hits a metal piece with high speed of 100 m/s ,1atm but temp 2000K. I have to track the shape of droplet after impact. Total time is 2 microsec (including spread of droplet after impact). Rest of the details you can find in "ccl " . Attached "ccl" contains basic physics information which i am using right now ,only time scheme changes.Just a good guess for my problem.

Thanks

[ghorrocks]

Some comments on your CCL:
* Why have you put all the expert parameters in there? I would remove them all and only put in the ones you really need. You can easily stuff things up with expert parameters and 99% the defaults are fine.
* Don't use a minimum number of coeff loops, if it converges quickly then just move on.
* You have buoyancy on. What buoyant effects do you expect? I suspect you can remove this option. In micro scale stuff gravity rarely does anything expect in very long time scales.
* You should use homogeneous momentum equation as well. That will simplify things. Have a look at the free surface flow tutorials for details on this.
* Often I have problems with the entrainment opening BC. Try other opening BC options.
* The CEL "liquid = step((rdrop-dist)/1[mm])" is bad practise - if you are non-dimensionalising then you should divide by 1[m]. But for the step function this should make no difference.

Can you post an image of your initial conditions from CFD-Post?

[Danial Q]

1. I am not using expert parameters anymore.
2. Don't use "minimum number of coeff loops", I did not get this point. Do you mean that I should increase the number of them e.g. from 3 to 4?
3. I will try with non buoyant feature.
4. I have tried "opening press and direction" condition for opening boundary rather "entrainment" option but it did not make any difference though. Right now, I am using opening press and direction option.
5. "Homogeneous momentum equation" details, I did not see any specifc in that tutorial.
6. In a CEL for "liquid", I used [mm] because I defined "dist" expression in [mm]. And this unit is used for making the STEP function "dimensionless" (mentioned in documents).So, you think it should be in [m] always?

Thanks

[ghorrocks]

2. No, remove the line. If it converges straight away then that is fine, proceed.
4. Often opening perss and dirn is more stable than entrainment. But sometimes it is the other way.
5. The free surface flow over a bump used homogeneous momentum/pressure equations.
6. When you non-dimensionalise by dividing by 1[mm] it is actually dividing by 0.001 [m], so it is being multiplied by 1000. This makes no difference to the function step() as that is only looking at the sign of the number, but for other functions it would ruin the calculation. That is why I say bad practise.

[Danial Q]

Sorry but I did not get your point about followings;

1. No, remove the line. If it converges straight away then that is fine, proceed. Because I dont know what are you asking me to do?? For transient scheme I have to set min and max coeff. loops.
2. How did they employ homogeneous momentum/pressure in free surface flow tutorial, I could not understand yet.
3. I will run cfx post and send you image but right now I tried to stop current run, it gave me exe error.

Thanks

[ghorrocks]

1. I remove that line of CCL so you do not set a minimum. It is very rare that you need to set a minimum.
2. Do the tutorial and see how they did it.
3. It is a good idea to output the initial condition by saving a results file at time step 0. This checks that the initial condition is what you intend it to be before spending all the time on a simulation.

[NewToAnsys]

Hi, could you please tell me how one performs a mesh sensitivity analysis without running the simulation for each different mesh?
I'm sure this is a basic question but I'm new to this.. could you maybe point me to some helpful literature/videos on the subject? Thanks in advance!