[butterflymuzzy]

Hello to everyone,

My name is Mustafa from istanbul. Im naval architect engineer and ı have been using cfx for calculating free surface model ships for 1 year. but ı havent reached the true answer yet. I m calculating 1/25 scale size of a 100 m lenght ship. the speed is 3 m/sec. I m using vof model with the help of ansys cfx free surface rigid body solution. ı m using steady state situation. ı used many type of time steps especially from 0.0025 sec to 0.01 sec . and ı used many type of mesh size for the surface of the ship from 30 mm to 6 mm. my domain sizes are ok. 5 ship lenght from back. 2.5 ship lenght from forward and side. inflation thickness of the ship 20mm, the sea and air is 30 mm. and 1 ship lenght from bottom and top. my wxpressions are airini, watini, hydpres and draft of the ship. inlet outlet, top side bottom (free surface), half ship side symmetry. rigid body mass moment of inertias and position of the 6 dof are ok. trasnverse movement form z axis, rotational movement from y axis. when ı started the solution and following the drag of the ship from monitor. from 1 to 700 th itearition everything was ok. the force was ossilating and going to the right value. but after 700th and 800th iteration directly go to the up up up up. ı couldnt control it with many type of mesh and time step sizes after 700 th or 800 th iteration .

ı know may be you can say me this is because of the stady state situation use the transient one. but is there any clue for steady side for calculating the resistance.

Thanks so much for your helps.

[ghorrocks]

This question seems to be related to this FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

In free surface models which run fine but then diverge, it is often caused by a surface wave finally reaching a boundary and the boundary is unable to properly handle the approaching wave. This can be linked to poor specification of boundary condition which does not allow the water level to move around properly. Can you check whether a surface wave has hit a boundary around the 700th iteration?

[butterflymuzzy]

So you mean nd suggest that increase of your inflation thickneses?

ı m gonna show the pictures of my cfx free surface work this evening.

[ghorrocks]

No, that is not what I mean. The vessel will create waves, and these waves take time to propagate out. This means after a while the waves will hit the boundaries. If your boundaries can't handle waves it will crash. This can cause free surface simulations to run OK for a while but diverge later on.

[butterflymuzzy]

So how can my boundaries handle with waves those are the todays picture of my running.

You can see the mommentum, mass, turbulence and resistance graphs of my ship. Now 1750th iteration finished. İt is still continuening. Are those graphs normal ?

Trim and sinkage hasnt converged yet. I m using physical timestep 0.01 sec

Thanks.

[butterflymuzzy]

Mass and momentum graphs

[butterflymuzzy]

Turbulence (KE) graphs.

[butterflymuzzy]

Ghorrocks hello,

We talked about my situation 2 weeks ago,

I m still working on my cfd free surface rigid body ship resistance in cfx. i m using steady state situation.

For controlling the resistance force ı did everything. ı changed the time step from 0.01 to 0.0025 sec, ı changed the mesh size from 30 mm to 6 mm but ı could not control the resistance force. for example for 30 mm mesh size and 0.01 time step after 700th iteration the resistance is going up up up, if ı change the physical time step from 0.01 sec to 0.002 sec that resistance force divergence is starting from 2400th time step.

On the other hand for the rigid body side, ı entered mass moment of inertia of the 1/24 scale ship ixx iyy izz (kg/m^2). and i entered the LCG of the ship . I entered the advanced solve functions of mesh,force and torque relaxetions as 0.5, 0.5 and 0.25 for rigid body. I made also advanced controls(coupled, volume weighetedi high resolution ). but like the resistance, when i control the rigid body movement euler y trim and position of z sink, after a while sink is going bottom then goes up up up then the solution crashed in 1800th iteration.

I will share the pictures of my projects solution data (pre setup and mesh steps) in here.



today ı m changing inflation layer thickneses, ı was using 30 mm 12 layers total thickness in free surfaces air and water. but my wave's height from the bottom of the ship (zero point) is 270 mm. under sea height is 170 mm. so the wave height is 100 mm. this height is longer then my inflation thickness. so ı changes the thikness height of my free surfaces.

Do you suggest anything for fix this resistance and rigid body problem?

Best,

Mustafa

[butterflymuzzy]

And also from this topic ı want to learn from you many things. and ı want to share my cfx ship resistance knowledge with other members.

I will share every solution setup details(with expressions) from here with pictures.

Best.

[ghorrocks]

I would recommend you do some simpler simulations to guide you on how to set good accuracy. I would recommend:
* Do a single phase, fixed mesh (no rigid body) simulation over the boat hull and do sensitivity analysis on the mesh size and convergence criteria until you get good wall friction accuracy.
* Using the mesh from the previous step as a starting point, then do a free surface, fixed mesh (no rigid body) sensitivity analysis on mesh size and convergence tolerance. Your mesh from the first step should be good for the skin friction, but you might need refinement around the free surface to resolve the surface waves.
* Only then do the full model with a rigid body model.

Also - you have not made any comments about whether the surface waves have reached the boundary. In my experience this is very important and a common source of problems. Please have a look at the surface waves near the boundary and see whether they are behaving realistically. You will probably have to apply wave absorbing boundary conditions.

[butterflymuzzy]

Also - you have not made any comments about whether the surface waves have reached the boundary. In my experience this is very important and a common source of problems. Please have a look at the surface waves near the boundary and see whether they are behaving realistically. You will probably have to apply wave absorbing boundary conditions.

Is this mean the height of the wave and thickness of my boundary(inflation) thickness ?

the height of the wave from the from the side of the ship is higher than of my inflation thickness ?

Do you have skype or facebook, ı want to talk with you this situation from skype of facebook with your permission

[dkmred]

@butterflymuzzy

I am working on a similar project. Can you give us a feedback how you could handle your issues and share your experiences or .def files?

Thanks

[butterflymuzzy]

Thanks so much Glenn

[butterflymuzzy]

Originally Posted by ghorrocks

No, that is not what I mean. The vessel will create waves, and these waves take time to propagate out. This means after a while the waves will hit the boundaries. If your boundaries can't handle waves it will crash. This can cause free surface simulations to run OK for a while but diverge later on.

Glenn Hello again. I have been working for 1 year after my last message for this toppic.

I tried many strategies. I used from 0.01 to 0.0025 sec time steps but the free surface flow didnt converge. it converged for a while then goes up up up too far.

Then i checked the water hight from result chapter, with iso surface and i added a longitudional section plane with mesh for checking the free surface height is up or below my inflation height. i saw that when the water passed from aft bottom side of the ship, it made a goose neck height. So that height passed my inflation layer thikness. So you mean that my inflation layer prsims could not handle with the free surface.

My time step strategy for steady side is 1/4 rule , like pseudo transient.

For example using the physical time step 0.01 sec for continuity, momentum and turbulence but using 0.0025 sec only for volume fraction time step.

Why am i using this strategy ? Because i m adding the rigid body solver to my steady work.

Because you know and always say use the transient strategy for free surface but if i add the transient strategy the solving time took too much time with rigid body.


I will share the pictures of the water height with inflation layer thickness in the next message.

You said that the problem might be mainly from the mesh inflation quality.

Especially i think the prisms inside my inflation thickness could not handle with the water speed of 3 m/sec or 4 m/sec .

My typical inflation total thickness is 90 mm with 1.2 growth rate and 12 layers each of air and water domain side.

So can the problem be solved with changing the layer number from 12 to 6 or growth rate 1.2 to 1.15 ?

And also changing the physical time step from (0.01/[0.0025vf]) to (0.002/[0.0005vf])

I love CFX and there is no problem one fluid resistance problems with cfx. So useful.

But for the free surface it is like a nightmare for me for 1 year

But I promise my self for solving this problem

If i solve this problem i will add rigid body motion with sinkage and trim.

Thanks so much Glenn

Best.

Mustafa.

[ghorrocks]

but if i add the transient strategy the solving time took too much time

Yes, transient simulations take longer. But I bet if you had done it with a transient simulation months ago when you first started looking at this you would have got a good simulation by now. So is a transient simulation really too long when it means you get a usable answer quicker than if you try to do it using "faster" methods?

[butterflymuzzy]

Originally Posted by ghorrocks

Yes, transient simulations take longer. But I bet if you had done it with a transient simulation months ago when you first started looking at this you would have got a good simulation by now. So is a transient simulation really too long when it means you get a usable answer quicker than if you try to do it using "faster" methods?

Thanks so much Glenn

I solved my problem. My problem is i forgot to change the density of water from materials.

I used the density of salt water 1025 kg / m^3 in hydpress expression. So the problem solved. I can do the free surface ship resistance with steady state condition.

My new problem is now with the new version of ansys. ı changed my ansys version from 16.2 to 18.

When i used 16.2 the rigid ship body's dynamic trim and sinkage can easily converged in 4000 iterations.

But when i open the 16.2 ansys file with ansys 18 cfx, all the spesifications are same (did not change anything) but the rigid body solution is stopping after 160 iterations because of the negative volume mesh.

Can ansys cfx change any thing in solver method in this new version ?

in 14-15-16 can easily converge but in 18 there is a problem

[ghorrocks]

They have changed the mesh motion smoothing parameters in recent versions. For most users this improves the resulting mesh but you may be a case where the old settings are better. So I would look into the moving mesh smoother options looking for something which has changed, or new defaults defined.

[butterflymuzzy]

Till to the 16.2 version every thing was great. my relaxiation factors of sinkage and trim were really good in the 14.0,15.0,16.0 and 16.2 versions.

But i tried today 17.0, 17.2, 18.0 and 18.2 versions the result was negatively same After 180 iterations it was crashed.

Especially the solution menu was changed from version 17.0

But the mesh quality was really good in the new versions.

So you suggest that continue to use 16.2.

I m still searching where this problem can easily be solved ?

I tried the mesh,set up and solution menus combinations but the result was same.

Best.

[ghorrocks]

As I said in my previous post, the change which is affecting you is in the meh smoothing options. So that is where to look. Hopefully doing some quick simulations looking at the effect of the mesh smoothing options will find the issue.

It would be better to be on the current version of the software as it has many improvements. But if you can't get it working then you may have to admit defeat and go back to the older version.

[butterflymuzzy]

I used the default model exponent 2 each of the increase near volumes and boundaries.

But now after your recommendation in this new version, i will try to change the model exponent value from 2 to 1 or something like that till to find the converge.