Hi,

I am trying to simulate a roll tank in CFX. I firstly want to discover the natural frequency of the tank. To do this I was going to excite the tank and record the time of the cycles.

Is this a possible approach and how would I go about it? I have modelled the tank etc.

I would greatly appreciate any help

Regards, Sam

I would use a structural package to do this... do you happen to have the structural package of ANSYS?

Hi,

What is a roll tank? Is it the fluid or structural (or coupled fluid/structural) natural frequency you are looking for?

Glenn Horrocks

Hey Guys,

thanks for help. They use roll tanks in ships it is a tany in a u-shape half field with fluid they are designed so that when the ship rolls the fluid will roll 90o out of phase and dampen the motions.

I am not concerned with the sturcutre of the tank at all I just want to know the frequency at which the tank will ocillate about it longitudinal axis.

i.e. if the tank is inclined and restrained on a kknife edge at the bottom middle of the u-shape what frequency will it roll at

I have setup the problem in CFX I just don't know how to set me inital condtion to be at an incline? I have defined a local coord and the local z axis is what I want the tank to pivot on.

Regards,

Sam

If you're after the frequency of the tanks in roll (motion about the longitudinal axis), then CFD is overkill - have a look at 'Seakeeping: ship behaviour in rough weather' by Adrian Lloyd - specifically the roll stabilisation chapter.

Hope that helps, latslosh

Hi,

You can model this simply by starting with the tank with the free surface offset and modelling the flow from there. You cannot model in the frequency domain as you can in FEA solvers so you are forced to do a full transient analysis and extract the frequency from that.

You can also use the moving mesh or rotating frames of reference approach to more precisely model your motion, as it is actually a rotation and so will have centrifugal and coriolis components. Whether these components are significant will depend on the geometry.

Glenn Horrocks

Thanks very much for everyones help,

I realsise there are other ways to get the natural roll period how ever I would like to extend this to more complicated geometries. The main reason I am doing this however is to discover the moment generated at any isntance in time this I believe I need to use CFD for.

Thankyou Glenn I will try to each of those approaches, is there one you suggest will work better than others? I was attempting to simulate an oscillating gravity to replicate the movments of the tank however it hasn't worked at this stage.

Does anyone know of any tutorials or examples of the methods listed by Glenn?

Once again thank youe veryone for your help, it is great that a site liek this existis!

Regards,

Sam

Sam,

In that case finding resonance is standard experimental procedure - only that you're replicating it in CFD.

With respect to finding the moment histories: Rotating frames of reference work - I have used them for sloshing - but you need to be careful that the unsteady term (euler force) is included in the simulation. RFR is faster than having a moving mesh (no mesh displacement to be solved) and, in my opinion, easier to set up. However, the initialisation can be a bit tricky.

Good luck, latslosh

Thank you very much for your help latslosh,

I searched the ansys help file on RFR and found very little on how to set up a problem. I opened up my domain settings and in general option set the domain motion to rotating. I inserted a local axis and set the rotation about this axis.

Is this correct? How do I specify a rotation of say +/- 10 degrees rathere than having it do a full 360. I just want it to go back and forth.

I don't know how this normally works but it would be great if someone could send me a file on the set up?

Once again thankyou everyone for your help

Regards,

Sam

Hi Sam,

In a RFR simulation you specify the rotation speed. So you need to differentiate your angular displacement function to get a angular velocity function and use that as the speed of the RFR.

Glenn Horrocks

Thanks Glenn,

I will try that today. I have been so far just trying to simulate it using an occilating Gravity term which has not worked however I think it has not worked due to to larger time steps.

Regards,

Sam

Thanks everyone!

I have got the frame of reference function working so I'm very excited. I did as you said Glenn and derived an equation for angular velocity however it does not seem to work. When I specify a standard andualr velocit i.e. 0.8rad/s everything works as it should. However when i input the function the fluid goes everywhere!

The function I am putting in is

Av=514.29pi/180*cos(t*51.429*pi/180)

I have no clue what I am doing wrong but the fact that everything seems to work when I have a standard AV in must mean there is something wrong with the function

Regards,

Sam

The function is suppose to define a roll amplitude of 10 degrees and a roll period of 7 seconds

Regards

Sam

Sam,

Are you moving your gravity vector according to the specified angular displacement; and you may want to check the amplitude term in your expression for angular velocity - it does seem a little large (remember that CFX likes angles to be specified in radians...)

Cheers, latslosh

Thanks all,

I have got it to run succesfully. Latslosh that was my problem I was using degrees in my amplitude silly silly!

Once again thankyou very much all your help is much appreciated!