How to define a Timoshenko beam

[lukeme]

Dear members,

I need to do modal analysis of simple beam.The beam is of Timoshenko beam.

I am new to the Ansys. I did some examples through tutorials I could find on the net.

But I could not define Timoshenko beam (Beam 188 or 189). When I need to define Real Constants for the beam,
it gives "BEAM188 does not require real constants".
So how to define the real constants: Area, Izz, height for the beam?

Please help me.

 

[Drej]

Beams 188/9 don't use real constants. See the SEC#### series of commands in the help file to define the geometry of the beam, specifically SECTYPE and SECDATA.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[cloche]

Beam188 (linear element) and Beam189 (high-order "parabolic" variant of 188) do not require real constant because their section is defined by sketch. Use the Sections tools in order to accomplish that.

0) if your beam section falls into one of the typical standardized categories (I-shaped, U-shaped, L-shaped, square, circular,...), then you can choose the appropriate one by Sections -> Beam -> Common Sectns
1) if not, sketch the area representing the section of your beam, just like you would do for a normal model (use kpt, lines, etc, whatever you want).
2) you don't have to mesh the area, but you have to set LDIV or LESIZE for auto-mesh to respect your intent
3) Use Sections -> Beam -> Custom Sectns -> Write from Areas and select the area previously defined
4) when prompted, give a filename for the section data to be stored
5) then, call Read Sect Mesh, set the section ID number as you like, give it a section name (max 8 chars), set the location of element origin (depending on the analysis you are performing and the effects you want to take into account or discard; in case of symmetrical sections, this has of course no importance; but when centroid doesn't correspond with shear center, you have to carefully decide); the "coordinates" apply only when you choose "chosen location". Select the section file you previously saved.
6) you're done! now you can specify your section ID number when you set the Attributes for the elements Beam188/189. If you want to review the section's properties, simply go to Sections -> Beam -> Plot Section -> <ID number>

Bye, have fun with Ansys (I'm not ironic)!

Claudio

 

[lukeme]

Dear Claudio or drej,

Thanks so much for your reply but I could not really understand this Ansys and have not been able to find the frequencies of a simple Timoshenko beam. I am also trying to find them by hand but the results
are contradictory. I am realy desperate.


Would you please find the frequencies (the first two or three would be ok) for me, it would take just a litte time of yours, couple of minutes maybe??

Beam ---> -----------------
/\ /\

it is simple beam with a pinned support at left
and roller support at right end.

Geometrical properties:
L=5 m (length of the beam)
b=0.5 m (width of the beam)
h=1.0 m (height of the beam)
hence, I=4.17e-2 m4 and A=0.5 m2.
k=0.83 (shear correction factor)

Material properties:
E=2.1e10 N/m2 (modulus of elasticity)
G=7.0e9 N/m2 (shear modulus)
rho= 2400 kg/m3 (material density)

Please help me??

 

[Drej]

You must do this job and understand it yourself. If not, how are you going to explain the results to someone else? If you need only to analyse the modal response then shear deformation is negligable and you can do the analysis with beam4 - or even beam44 elements and switch the keyopt for shear deformation. Here is some sample code which builds your model, but it is incomplete. You'll need to add in the solution items (boundary conditions, modal options, etc.) and then you must understand the results.

fini
/cle

/title,Modal Analysis of a Simply Supported Beam
/filnam,beam_modal

/prep7

k,1,0.,0.,0.
k,2,5,0.,0.

l,1,2

et,1,44
r,1,0.5,4.17E-2,10.42E-3,0.25,0.25

mp,dens,1,2400
mp,ex,1,210e9

lesiz,all,5/20
latt,1,1,1

lmesh,all

alls

/solu



------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[lukeme]

Dear Drej,

I have been investigating the effects of shear def. and rotational inertia on the frequencies of a beam, that s why I need to use Timoshenko beam.

I did some analytical work and got the results. However, the results seem incorrect and need to compare them with true/actual values.

I am an stuctural engineer. I know how to use SAP2000, ADINA .. but they are incapable of modeling this beam. The philosphy/methodology of Ansys is really hard to grasp (for me).

That s why I am needing your help if you can.

Best regards,
Luke

 

[Drej]

It would be useful if you could describe why you are investigating the effects of shear deflection. So please give details. Give details of the hand calculation you have done as well and the results you obtained. You say you did some "analytical work". Can you describe this. Can you also describe the "true/actual" values. How did you obtain these? Are they frequencies?

All ANSYS beams can account for the shear deflection of a beam. You will find that the higher order modes (and the corresponding frequencies) will be affected by this. The differences between your system with/without shear deflection is subtle but evident. Rotational inertia will do nothing for the system you describe (it is irrelevant given your description).





------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[lukeme]

Dear Drej,

The analytical work I have been doing is to drive the equation of motion of a Timosheko beam governing the transverse osccillation of the beam. Then imposing the initial conditions (support conditons), I try to find the modal response (frequencies, mode shapes etc.)

I need to compare the hand calculation with a FE or anything else that is capable of simulating Timoshenko beam. I assume that FE programs yield true or almost true results. Or somehow I need to make sure that what I have been doing is correct/ at least reasonable.

Am I clear, dear Drej?
Thank you so much for your input and interest,

Regards...