Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!

How to simulate the effects of water 2

Status
Not open for further replies.
bisav

bisav

New member
Jul 2, 2014
22
0
0
IN
Hi everybody,

I have a doubt in PATRAN.
How to simulate the effects of water weight effectively.

My model is simple cylindrical tank, in fact a huge tank. Tank is completely filled with water. Now I want to run it for the modal analysis(Normal Modes). How do I give the weight of the water effectively to the container. If I create a mass element at the centre and attach it with all the nodes of the tank using RBE2 connection, the system becomes very stiff. And if I give non structural mass (value is calculated by total mass divided by the total surface area) in the element property of the tank wall, I think that either is not the correct way to simulate water. Because each wall will be carrying huge loads which I feel is not the correct way to do it.

Can anybody help me.?

Thanks
Bibin
 
Replies continue below

Recommended for you

Sort by date Sort by votes
Hi,

Hydrostatic pressure (P)?

P = Rho * g * h

Rho = fluid density , g = acceleration, h = fluid depth

Indeed the use of RBE2 is wrong and it will make the structure very stiff and cause numerical issues...

Here the variable is the water depth. With Femap it is easy to create such a pressure function of depth (so the element centroid, or node position) using data surface...Also I know that with Patran it is feasible too by creating spatial PCL function or tabular input. look at the attached pdf which explains how to create spatial and temporal variation of loads.


Hope this helps

Seif Eddine Naffoussi, Stress Engineer
33650 Martillac û France
 
Upvote 0 Downvote
Hai compsite curves,
Greetings for the day.

Thank you for the reply.
I have already applied this variable pressure by using spatial fields PCL function. That is for the stress analysis. Now that I want to do the MODAL analysis. This pressures won't be taken into account for modal analysis. But for modal analysis, I want to simulate the mass of the water effectively. I want to give the mass to the model in a correct manner. For this reason only in the modal analysis I removed the pressure function and created a mass element with the mass of the water at the center and attached it with tank using RBE2, but that is not the correct way, it makes the structure very stiff.

Bibin
 
Upvote 0 Downvote
If you have a parametric base plate mesh then you could extrude the plate elements in order to obtain SOLID elements (i.e HEXA).
Then you have to deal with MAT10 and PFLUID (field n° 8 in the PSOLID nastran card) to represents the water properties and assign this properties to the solid elements.
You will need to define some information like the mass density, speed of sound to calculate the bulk modulus...

Regards,

Seif Eddine Naffoussi, Stress Engineer
33650 Martillac û France
 
Upvote 0 Downvote
Hello compositecurves,

But how can we give the connection between fluid element(hex elements and the side wall) ?
Node connection or any other connection. Node connection seems to be difficult since it is a big structure, so there will be so many nodes. And if I didn't connect it with the side walls will it be the correct way to approach to the problem???

Regards
Bibin.
 
Upvote 0 Downvote
Inorder to give node merging nodes on the the wall should have its node positions similar to the hex elements right?
 
Upvote 0 Downvote

Hello
Good Morning

Node merging was not a problem. But while running it shows error. It seems like fluid elements can't be attached to structural elements.

The following is the error showing in F06,

USER FATAL MESSAGE 5419 (MODGM2)
STRUCTURAL ELEMENT QUAD4, ID = 1, REFERENCES FLUID GRID POINT ID = 1


And below is the error definition I found out,

*** USER FATAL MESSAGE 5419 (MODGM2) STRUCTURAL ELEMENT %1 ID =%2 IS ATTACHED TO A FLUID GRID POINT ID =%3



So is it not possible to attach a fluid elements with structural elements? If it is so how will we give the connection??

Regards
Bisav
 
Upvote 0 Downvote
Is that possible at all.............!!! REBE2 can have only one independent node. How can we create the entire connection like that. If we are creating a centre node and attaching all the other nodes its okay. But I feel that is not the correct way. Guide me If I am wrong.
 
Upvote 0 Downvote
coupling for FSI simulations in NASTRAN is achieved by the ACMODL bulk data entry. The user supplies a search tolerance which Nastran uses to find a fluid grids to be associated to a structure grids. At the end of the job, Nastran echoes the list of the fluid grids mapped to structure grids in the f06 file.

 
Upvote 0 Downvote
> how do I do that??

It is at this point that you need to pick up the patran users guide and read to find out how ACMODL is supported thro' patran.
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

Gabriel93
  • Locked
  • Question
Error 4521 (elements perpendicular to their coordinate system x-axis)
Replies
0
Views
18
Gabriel93
Gabriel93
lavecchiasignora
  • Locked
  • Question
Read or Import a set of nodes
Replies
1
Views
19
dmapguru
dmapguru
nmruble
  • Locked
  • Question
Bush Element /Spring Element, what is the difference? 1
Replies
1
Views
26
dmapguru
dmapguru
enghelp2806
  • Locked
  • Question
Importing BDF from Hypermesh to Patran and preserve property names?
Replies
1
Views
23
dmapguru
dmapguru
Emi.Cor
  • Locked
  • Question
Addition of 1D elements reduces Buckling Factor
Replies
0
Views
14
Emi.Cor
Emi.Cor
Back
Top