[salvooch]

I am having trouble with the top wall moving in either direction w/ the flap. As it moves to the limit of motion, the mesh collapses and crashes the run.

I've fixed the top motion to be 0 in all directions, but this just causes the mesh to distort in the upper corner of the flap.

Anyone know how to fix this? Or do I have to re-mesh to a more coarse level of fidelity in the mesh?

Thanks

[ghorrocks]

Please post a drawing of your setup.

[salvooch]

Not much to draw; rectangle that is half full w/ water and I flap the right side to induce the waves. I've have attached the picture of the mesh collapsing on the upper left corner (opposite the flapping wall). Because the top boundary is moving, it collapses over itself and crashes the run.

The first is the time step before the run crashes, the second is a screen shot at failure:

BEFORE_FAILURE.pdf

FAILURE.pdf

I never had this problem when I was using a piston type wall movement, only here w/ the flap-type. I've since refined the mesh to be more coarse at the top corners in an effort to get around this, but I don't know why this way moves the top wall and the piston didn't. Any help would be greatly appreciated, thanks!

[ghorrocks]

The solution should be obvious - you need to make the top wall "unspecified" motion.

[salvooch]

That didn't work. It compressed the mesh from the middle when 'unspecified'; sagged down the same displacement provided, then crashed when the mesh collapsed.

[ghorrocks]

Can you post some images?

[salvooch]

Sorry, I found a slight error when inserting my ref coord frame for the rigid body (darn decimals...). I will be running it again today, should have a result by tomrw...

Thanks again for helping

[salvooch]

Thanks, worked like a charm!

Does anyone know how one of the earlier posters on this discussion was able to make this plot? I have been trying to make a plot of wave height like this, but my accuracy when compared to actually measuring it in Post Processor does not match. Does anyone know if this is through a function w/in CFX or how this was done?

I tried using pressure to calculate the wave height above a known point w/in the water, but again, it does not compare to the measured height. Does anyone know the best way to get the free surface height?

Thanks

Originally Posted by FluidH

Hi!

Here are a graph of my results:

[ghorrocks]

In CFD-Post draw a line parallel to the gravity vector which crosses the surface. Then calculate a line integral of volume fraction on the line.

A better way of doing it for transient runs is to define a monitor point, then it will be calculated for each time step. Define a plane parallel to the gravity vector or a long skinny volume and do an integral of volume fraction on it.

[salvooch]

You mean the lengthInt command in the post calculator set to water volume fraction, correct? Just want to be sure I am using the correct function in Post.

Also, is there a way to have Post step through and gather the values? I put the expression into the table but it only collects the data from the current time step. If I have to step thru each one and record the data, OK, it's not that bad; just wondering if there is an easier way to export the data to a table.

You mention a way to get this to work w/ a monitor point in Pre, but how does that input to an integral along a line to measure the volume fraction? Is there a way to input a 'monitor line' in Pre? Exporting the results would be much easier, but not sure how a point correlates to the line.

Sorry to ask so many questions, but I do truly appreciate the help you've provided so far! Thank you, again!

[ghorrocks]

You mean the lengthInt command

Correct.

Also, is there a way to have Post step through and gather the values?

Write a session file to do it for you. Use a perl loop to loop through all timesteps.

You cannot use a line as a location reference in the solver (to my knowledge). That is why I recommend you use a long skinny volume (which approximates a line) or a surface. Output the data using a CEL expression on a monitor point.

[salvooch]

Thanks, you've helped me out a lot!

[mystar]

Originally Posted by solimcfd

Hi, I am using CFX to model ocean waves using linear wave theory. I am using a multiphase simulation with air and water as the fluids. My results seem reasonably good but I would like to inject particles into the flow in order to see how they move in the field and to compare these particle tracks with theory. My problem is that I cannot add a particle transport solid if I already have two eulerian fluids, CFX doesnt allow it. Does any one have an idea of what I could do? Thanks

Hi ! Could you tell me how to creat wave boundary condition. I have tried many time but no result ...
Thank and Brg

[ghorrocks]

Simple waves can be generated by moving a boundary wall or imposing a simple sinuosoidal function. A much better way is by imposing a linear or non-linear wave equation on a boundary - but that is much more complex. There are some posts ont he forum on this, do a search to find them, or search google.

[belgacem]

Hi Friend
Can you more explain how to used the linear velocity filed at the inlet to generate the wave? how to set up this condition using the CEL.

[belgacem]

Hi Friend
Can you more explain how to used the linear velocity filed at the inlet to generate the wave? how to set up this condition using the CEL.

[Ahmed Elhanafi]

Hi All,

Id like to generate regular waves in Fluent. I successfully generated regular waves with laminar flow, but when tried to move to turbulent flow using either K-E or K_W and SST models, I got a problem with the results as you can see in the attachment.

Please, if you don’t mid helping me with this issue.

My Model Details are as follow:

Model details:
2-D model with 40m length 0.8m height and 0.5m water depth.
Free surface zone is 0.3m with 20 element/wave height and 100 element/wave length.
Mesh quality (Quad) 1.0.
I’m using open channel boundary conditions, Implicit solver.

Boundary conditions:

Left side: Inlet (open channel), Right side: no slip wall, bottom: no slip wall, top: outlet (open channel)

Solver settings:

Pressure-Velocity Coupling: PISO
Gradient: Least Squares Cell Based
Pressure: PRESTO! or Body Force Weighted
Momentum: Second order upwind
Volume Fraction: Compressive
For turbulence: Kinetic energy and dissipation: 1st and 2nd order upwind
Transient Formulation: Bounded 2nd order Implicit
Time step: 0.0025 sec.
No of Iterations: 20


Thanks.

[ghorrocks]

Try the fluent forum.

[pawl]

Originally Posted by solimcfd

Yeah, I am also using a physical beach, this does help with reflection but does not change the damping. What kind of grid are you using? Have you refined it in the region where the free surface is? What I noticed is that the damping gets worse when the cells are stretched quite a lot. There is a paper that has investigated all of these problems: http://www.ipen.org.br/Artigos-congr...NA2010-141.pdf. I am trying to reproduce their results, but for some reason I get excessive damping.

Hi. I know this is late.
Any update about how to prevent wave height damping along its propagation in wave tank?
Some say I need to run it in laminar model. But my work need it in turbulent model

[ghorrocks]

Firstly, have you confirmed you have a situation where the waves are not highly damped?

If the flow should not be highly damped but the simulation is then you have a problem with numerical dissipation. Have you done all the normal things to reduce numerical dissipation? Finer mesh, smaller time steps, high order space and time differencing. Also check the options for the free surface model as some of them are dissipative.