Modal Analysis of Tension Cable Connected Structure 1

[generaluday]

Hello!

I'm trying to solve a problem comprising of a simple fuselage with pre-stressed tension cables connecting the arms of the fuselage. I'd like to conduct a modal analysis on this setup. Let's assume that the fuselage comprises of an X-shaped structure with 4 tension cables connecting the arms, and is tethered to the ground along it's center point. I've meshed the arms with simple Beam elements, and I tried using DOF Spring elements with a certain stiffness for the cables, but the modal frequencies seem to remain the same regardless of the changes in the stiffness values.

It has been well established that the tension in the cables is critical in determining the natural frequencies of such structures, for instance, those of cable-stayed bridges, etc. What is the best way to simulate this type of scenario in Femap?

Thanks.

 

[BlasMolero]

Hello!,
You will need to pre-stress the model using a Subcase:

1.- First you will need to setup & run a Linear Static Analysis (SOL101) of your model.
2.- After that Set the Analysis Program to 36..NX Nastran and the Analysis Type to 2..Normal Modes/Eigenvalue
3.- Click OK to create the Normal Modes analysis set.
4.- Expand the newly created analysis set so that you can see the options for Bulk Data Options, Modal/Buckling and the entire tree under Master Requests and Conditions.
5.- Before running the Normal Modes, preload the model by creating a Subcase for the linear static loading:
• In the Analysis Set Manager dialog box, select Master Requests and Conditions then the New button.
• Click OK to create the subcase
• Expand Case: 1.. and its Boundary Conditions tree
• Select Boundary Conditions then click Edit.
• Set the Constraints to the existing one.
• Set the Loads to the existing one as well.
• Click OK to apply the changes

And Run Normal Modes analysis. If you compare with the results obtained without performing a pre-stress you will see that now your frequencies are bigger, because your structure is stiffer, is pre-stressed, OK?.

Now you know how to run a preloaded modal analysis, this is simply.

Best regards,
Blas.


~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

 

[generaluday]

Hello Blas,

Thanks a lot for the instructions and ideas. I used to do pre-stressed modal analyses in ANSYS, but I wasn't sure how to do that in Femap. I got in touch with someone in Siemens, and he pretty much gave me the same instructions.

I pre-stressed the cables using a bolt preload, and ran the pre-stiffened modal analysis, and that worked. Is this the strategy you would use in case of cables?

I'm trying different ways to pre-stress the cables, and I'll post it on here if I find a better way to do it.

Thanks!

 

[jacksonfem]

Is there any other way to simulate cable elements in Femap except nonlinear springs or a truss element with a stess-strain material behaviour with almost zero compression stifness?

At rod element exists a "cable" option. Is it working only with NeiNastran solver??

Thanks!