[Danial Q]

But when i was using the previous small timesteps (5e-10 s) , i did not have any error like this. So for adaptive timestepping,problem reveals, how can it be improved (make stable) while using adaptive??

[ghorrocks]

In that case your setup with step changes in material properties requires finer time steps than the normal solver so you will have to work out what time steps it needs. Obviously you need finer time steps then adaptive is trying to give.

Any don't forget you may need tighter convergence.

[Danial Q]

This time i have chosen these adaptive time step settings and it looks good so far but would need your say on this, if it is going good or should start over;

total time = 2e-6s
initial time = 5e-10s
Max time step = 5e-8s
Min time step = 1e-20s
Max/Min loop = 9/4
Time dec. factor = 0.5
Time Inc. factor = 1
Residual Traget = 1e-4
AND
Adaptive Timestepping Information |
----------------------------------------------------------------------
| Direction | Ratio | Last Value | Next Value | RMS Co | Max Co |
+----------------+-------+------------+------------+--------+--------+
| Unchanged | 1.000 | 6.2500E-11 | 6.2500E-11 | 0.00 | 0.00
TIME STEP = 489 SIMULATION TIME = 3.1250E-08 CPU SECONDS = 7.119E+04
----------------------------------------------------------------------
COEFFICIENT LOOP ITERATION = 1 CPU SECONDS = 7.119E+04
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk | 1.00 | 4.4E-08 | 2.6E-06 | 2.1E-03 OK|
| V-Mom-Bulk | 1.00 | 4.6E-08 | 3.7E-06 | 2.1E-03 OK|
| W-Mom-Bulk | 1.00 | 7.3E-08 | 2.9E-06 | 1.3E-03 OK|
| Mass-liquidNi | 1.00 | 4.3E-18 | 2.1E-16 | 4.0E-05 OK|
| Mass-Air at25C | 1.00 | 9.6E-12 | 1.5E-09 | 8.5 9.5E-03 OK|
+----------------------+------+---------+---------+------------------+
| H-Energy-liquidNi | 1.00 | 4.1E-12 | 1.9E-11 | 1.3E-16 OK|
| H-Energy-Air at25C | 1.00 | 3.4E-04 | 1.6E-03 | 5.7E-17 OK|
| T-Energy | 1.00 | 2.5E-08 | 1.4E-07 | 9.4 1.3E-16 OK|
+----------------------+------+---------+---------+------------------+
COEFFICIENT LOOP ITERATION = 3 CPU SECONDS = 7.129E+04
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk | 0.42 | 1.2E-09 | 8.1E-08 | 3.1E-02 ok|
| V-Mom-Bulk | 0.41 | 1.1E-09 | 5.1E-08 | 3.1E-02 ok|
| W-Mom-Bulk | 0.57 | 6.2E-09 | 9.5E-08 | 8.4E-03 OK|
| Mass-liquidNi | 1.00 | 1.7E-18 | 9.2E-17 | 2.8E-05 OK|
| Mass-Air at25C | 0.59 | 2.0E-12 | 3.9E-10 | 12.3 9.9E-03 OK|
+----------------------+------+---------+---------+------------------+
| H-Energy-liquidNi | 0.02 | 2.0E-10 | 9.3E-10 | 4.2E-17 OK|
| H-Energy-Air at25C | 0.02 | 1.2E-10 | 5.8E-10 | 3.5E-17 OK|
| T-Energy | 0.50 | 7.5E-09 | 4.1E-08 | 9.4 4.2E-17 OK|
+----------------------+------+---------+---------+------------------+

Thanks

[ghorrocks]

Why min 4 loops? Then the adaptive time steps can never reduce the time step.

Why an increment factor of 1.0? Then the time steps never increase.

You need to do a sensitivity study on your convergence criteria.

[Danial Q]

I have set min loop to 4 as If I set min coefficient loops '3' for solver control. And if I set less than 3, CFx gives error to be set it more than min solver target loops.
And i decreased the increment factor to capture the changes in short time step. I thought it would help to tighten the control.

Do you think, I should change coefficient loops in solver settings?? I will have to set it min 2 to get min 3 loops in adaptive time stepping.

Thanks

[ghorrocks]

At the moment your setting of the minimum coeff loops and increase factor of 1.0 means that adaptive time stepping will not work.

[Danial Q]

I tried another run with default settings of adaptive time stepping, with min 5 and max 10 loops while min timestep was 1e-20s and max was 5e-7, initial 5e-10s. BUt again same numerical unstability error.

[ghorrocks]

As entertaining as this conversation is, I fear it will go on forever. The approach you have chosen is numerically unstable - you are always going to be getting numerical errors as it is a very poor approach. It also misses essential physics (ie latent heat) and that is almost certainly important as well.

You need to work out an approach which actually models the physics of the solidifcation phase change in a fashion which is numerically stable. There is no easy way of doing this in CFX, that is why it is not in there already. You are going to have to get some tips from support on how to do this as I do not know.

[Danial Q]

I consulted with them and this is what they suggested, properties as a function of Temp. So for latent heat , I checked the literature and employed the approach. So i dont know what loopholes ,u think are in this approach. Latent heat is added in specific heat for phase change in certain range, so did i.
if(T<1725.5[K],595[J kg^-1 K^-1],if(T>1725.5[K] && T<1726.5[K],145067[J kg^-1 K^-1],620[J kg^-1 K^-1]))
This red expression defines the range and adds latent heat for phase change or removes it depending on temp.

[ghorrocks]

That might account for the latent heat but will be very numerically unstable, which takes us back to square 1.

So if you want to do this model you should forget the normal rules of thumb (eg the normal settings in adaptive time steps and general comments on convergence). To get this to converge you are going to have to be very gentle with it - an excellent quality mesh, small time steps, double precision numerics.

[Danial Q]

Hmmm... though I am using double numerics atleast for my last two runs and timesteps has also been reduced to less than nanos. Now "Excellent quality Mesh" is what I am looking for. I have tried sweep method with edge sizing but it looks like my system has forgotten, how to mesh. I mean, is it usual that meshing takes days even for micron size bodies, which has element size set to 5e-3 micron??
I have attached pics if you could kindly look at set parameters and advise.

Thanks

[ghorrocks]

This question is best asked on the meshing and geometry forum.

But I will say that with a simple geometry like you appear to have a perfect hex mesh should be possible - 1:1 aspect ratio elements, perpendicular faces. This will give you the best chance of convergence. Is this what you have for your current mesh?

Also use the mapped mesh gizmo to force it to do a hex mesh. If it is taking ages then make sure you have the settings right on a coarse mesh which completes in seconds before refining.

[Danial Q]

Infact I used Hex dominant mesh for the model (for last couple of runs) and just for assurance posted it on that Meshing Forum. Some one there advised me to do sweep mesh with edge sizing. But this sweep method is taking tooo long.

[ghorrocks]

Use a mapped mesh gizmo with the sweep and start with a coarse mesh to get it working.

[Danial Q]

But another thing which is mentioned in literature that Hex dominant mesh is not suitable for sweepable bodies and my domains are also sweepable. did i get it right?

Thanks

[Danial Q]

Alright, I will give it a shot and i hope it would take less time with default values.

Thanks

[ghorrocks]

You don't want hex dominant for a body like this which should be easily sweepable/full hex mesh.

[Danial Q]

Originally Posted by ghorrocks

You don't want hex dominant for a body like this which should be easily sweepable/full hex mesh.

was taht question or advice?? din't get your point.

[ghorrocks]

It was advice, but a little incoherent I guess

To write it more clearly:
Do not use hex dominant for a body like this. You might still get some weird elements with hex dominant. This body should be easily sweepable so use that option.

[Far]

Originally Posted by Danial Q

Infact I used Hex dominant mesh for the model (for last couple of runs) and just for assurance posted it on that Meshing Forum. Some one there advised me to do sweep mesh with edge sizing. But this sweep method is taking tooo long.

Here is reply from Simon:

Originally Posted by PSYMN

In reverse order (since your first was best).

3) the Cartesian method does not work if you bend the blocking. Everything must remain Cartesian. We are releasing a cutcell mesher with ANSYS Meshing and/or TGrid at 13.0 (mid Nov 2010) that should do nicely for you. It does support baffles, inflation, etc. If you contact me privately, I would love to get your test case and run it thru that mesher.

2) The Hexa Dominant mesher is really intended for FEA users. I am not sure if it even supports baffles, but I know it doesn't support inflation.

1) Tetra Prism is the way to go for this sort of problem. Orthogonality of 90 degrees for Prism is good, so not sure what your problems really are. I would suggest going back to this approach and we can try to sort out your issues thru better settings, etc.

The first thing to look at will be if you have stair stepping on or not... Or you could create a baffle that extends beyond your actual sail (in a different "construction" part) so that the stair stepping can happen there, then you delete the shells in the construction part.

Here are a couple images to illustrate stair stepping on or off.
Attachment 4764

Attachment 4765

Later we can discuss how you will merge this with the hexa going on below the surface.

Originally Posted by PSYMN

Hexa Dominant was never intended for CFD. It puts isotropic hexas near the walls and junk in the middle. It doesn't work with prism, etc. Only use it for FEA (mechanical) applications. We should probably just hide it if you set the physics to CFD...

What you want is "Assembly Meshing" "Cutcel". You can use global inflation with Named selections to control where the prism is applied. It works very well at R14.0, but is different from the other "methods" in how you apply it. Look it up in the Help to find it.

The catch is that it produces a mesh with haning nodes and some poly's so it is only good for Fluent, CFX doesn't like it.

You can try ICEM CFD Hexa.