topic Re: How can model hydrodynamic pressure on RSA in Robot Structural Analysis Forum

How can model hydrodynamic pressure on RSA

Anonymous — Sat, 03 Oct 2015 01:40:50 GMT

Dear all

For the Seismic Analysis of Liquid-Storage Tanks, refer eurocode 3 and other documents, Hydrodynamic pressure have been modeled like convective mass with spring having stiffness.

As picture bellow

Anyone tell me, how can i model convective mass on RSA with spring (kc)

Thanks in advance

Re: How can model hydrodynamic pressure on RSA

Anonymous — Sat, 03 Oct 2015 07:38:45 GMT

No reply, anyone help me...:(

Re: How can model hydrodynamic pressure on RSA

Rafacascudo — Mon, 05 Oct 2015 17:04:42 GMT

never done it but Probably you can can try very rigid bars with no mass and use bar elastic release to simulate the kc spring

Re: How can model hydrodynamic pressure on RSA

Anonymous — Tue, 06 Oct 2015 03:40:02 GMT

Dear Rafa

I've model as that, but, have a problem as bellow

could u check it for me

Re: How can model hydrodynamic pressure on RSA

napooil — Tue, 06 Oct 2015 05:52:18 GMT

You have to check box as picture.

Re: How can model hydrodynamic pressure on RSA

Anonymous — Fri, 09 Oct 2015 03:56:32 GMT

Dear all,

i've modeling as this method

however analytical results have been problem, as bellow

i've att my model, anyone can be help me again

Re: How can model hydrodynamic pressure on RSA

Rafacascudo — Fri, 09 Oct 2015 14:30:29 GMT

Hard to say without further information.

Which load case?

"supposed like this" is vertical or horizontal displacement ?

If it´s modal analysis ,modes 4 and 5 show similar displacement to your picture

Re: How can model hydrodynamic pressure on RSA

Anonymous — Sat, 10 Oct 2015 01:10:20 GMT

Dear rafa
it's horizontal displacement
i'll be check again... thanks u somuch...

Re: How can model hydrodynamic pressure on RSA

Pawel.Pulak — Tue, 13 Oct 2015 17:58:07 GMT

If you mean the deformation in the horizontal direction you may refer to vibration modes 4 and 5, mentioned by Rafael.

Below are some screen captures showing top view of them for bars made of LINK-1 section.

Looking at these modes 2 observations can be made:

deformations related to these modes are not only in global X or only in global Y direction but in both of them - like "oblique". It is so because of the symmetry of the model - both modes have the same frequency and from the theoretical point of view any mutually orthogonal vibration modes are correct
shapes of vibration modes and types of releases used for bars with LINK-1 section correspond to using not only the elasticity of springs defined in releases but also elasticity (longitudinal and transversal ) of the bars themselves and moreover the elasticity of releases is duplicated as longitudinal (for local UX) and transversal (for local UY). It makes it sophisticated and the full control of stiffness defined this way is rather difficult.

The screen capture in your first post and the document attached to it suggest that the convective mass should be connected to the walls of the tank by the set of simple longitudinal springs, acting in horizontal directions. The simplest approach for it in Robot seems using weightless truss bars with length, section and material corresponding to required stiffness. In your model the length is 5 meters (radius of tank), stiffness defined in releases is 1000 kN/m, "Nomass" material defined by you has Young's modulus E=2e5 MPa. In such case the section area corresponding to these parameters is 1000*5000/2e5 = 25mm2

It means that the truss elements to model the springs can be made of 5x5mm square sections. I have defined such section with label "spring", assigned it to bars 3to6 or your model, declared them as truss bars (Geometry>Additional Attributes>Advanced Bar Properties), deleted now unnecessary releases and defined additional support to prevent the node with convective mass from vertical displacement and rotations.

I have attached such model to this post. You can see the change of vibration frequencies of modes 4 and 5 for it comparing to the original model (3.57 Hz instead of 4.47 Hz)

For this model also the effect described by me in point 1. can be observed - the vibrations shapes related to convective mass are not along global directions but 2 mutually orthogonal oblique directions.

Best regards,

Re: How can model hydrodynamic pressure on RSA

Anonymous — Wed, 14 Oct 2015 01:40:03 GMT

Thanks you so much, i'll be check it....

Re: How can model hydrodynamic pressure on RSA

Rafacascudo — Wed, 14 Oct 2015 12:35:52 GMT

Hi Pawel,

That´s also a good way!

I just prefer rigid bars and elastic releases because there´s no need to create new supports and calculate new section properties. In his original model just a bar like in the picture below , would give the same results as your model alternative!

On my almost total ignorance in dynamics , I just keep thinking, why not link this mass to all tank nodes ?

At least 4x90 degrees ,but to the nodes in the whole height lenght

Wouldn´t it be more realistic?

Re: How can model hydrodynamic pressure on RSA

Pawel.Pulak — Wed, 14 Oct 2015 13:20:20 GMT

Hi Rafael

"there are many ways to skin a cat"...

I prefer avoiding "rigid bars" because it is not quite clear and precise when explaining to others. You have defined a "rigid bar" with Ax=1000cm2 and Ix=Iy=Iz=1cm4 - it resulted in frequensies as in my model. But using "rigid bar" with the same Ax=1000cm2 but for instance circular or square shape would result in different results - because it would be "rigid" not only in longitudinal direction..

Not all nodes are linked because it is easier to model it this way - the number of springs is limited and their stiffness can be simply derived from stiffness related to convective mass.

In case of linking all nodes it would be more difficult to calculate the tributary stiffness corresponding to single link - especially in case of non-uniformly distributed nodes.

Regards,