Discussion Groups

Robot Structural Analysis

Reply
Member
greg.parent
Posts: 5
Registered: ‎06-26-2012

Re: Eigen Values / Natural Frequencies

07-05-2012 04:59 PM in reply to: Rafal.Gaweda

One thing I have not been able to model is the material of the conductor or of the guy wire.  For example the guy wire material is extra high strength steel and has a yield strength close to 175ksi.  I can't seem to input this material into robot.  Right now the guy wires are modeled as a 70ksi steel that was already in the material drop down list.  However, this may have no effect on the structures natural frequency or period.

 

I have noticed that if I apply the wind loads in different directions I get different values in the frequency and period.  I believe the best way to account for wind blowing in any direction is to modify the load case before the modal case.  I can modify this load case to represent the wind blowing in, say 8, different directions.  I can then run a modal analysis when load is applied in each different direction.

 

I am no longer getting the same Structural Frequencies for the 1st and 2nd modes, however they are very close.  For the short structure:

 

Mode 1: F1 = 0.92Hz

Mode 2: F2 = 0.98Hz

 

I would have expected a larger gap in Frequencies between the 1st and 2nd Mode.  Does anyone know why they are so close?

 

Also the guy wires were installed with an initial pre-tension.  Is thre any way I can model that?  Likewise the conductor was strung with a particular tension.  Is there any way I can model the cable elements to have these initial tensions?

 

I would appreciate it if someone take a look at these models and see if I am on the right track.  Thanks.

Please use plain text.
Product Support
pp2008
Posts: 529
Registered: ‎06-23-2008

Re: Eigen Values / Natural Frequencies

07-09-2012 12:43 AM in reply to: greg.parent

Hi Greg,

explanations concerning various topics raised in your post

 

One thing I have not been able to model is the material of the conductor or of the guy wire.  For example the guy wire material is extra high strength steel and has a yield strength close to 175ksi.  I can't seem to input this material into robot. 

 

        You can define and add new material to the database in Job Preferences - see the screen captures below. One note: it may be necessary to close Robot and start it again to make the new material available in all dialogues.

new_material.png

 

 However, this may have no effect on the structures natural frequency or period.

 

     Yes, the properties which influence the natural frequency or period are Young's modulus, Poisson ratio, unit weight.

 

I have noticed that if I apply the wind loads in different directions I get different values in the frequency and period.  I believe the best way to account for wind blowing in any direction is to modify the load case before the modal case.  I can modify this load case to represent the wind blowing in, say 8, different directions.  I can then run a modal analysis when load is applied in each different direction.

 

      Yes, repeating modal analysis after appropriate static load cases is the best approach in case of nonlinear models. In such case each modal analysis will use different linearized model from preceding static load case - already mentioned by me earlier in this thread.

 

I am no longer getting the same Structural Frequencies for the 1st and 2nd modes, however they are very close.  For the short structure:

Mode 1: F1 = 0.92Hz

Mode 2: F2 = 0.98Hz

I would have expected a larger gap in Frequencies between the 1st and 2nd Mode.  Does anyone know why they are so close?

 

    The frequencies for short structure attached by you are F1=1.44 Hz and F2=1.95 Hz.

But independent from these values have you looked at vibration shapes corresponding to these modes? It is a 3D model and they can correspond to different directions of vibrations. Previously you have mentioned precisely equal frequencies of the 1st and the 2nd mode. It is a correct solution in case of for instance 3D model of cantilever where the bending stiffness about "strong" and "weak" axis is the same - for instance circular or square section. In such case mode 1 and mode 2 correspond to the same shape of vibrations but in perpendicular directions. The same equal frequencies can be observed for modes 3 and 4. Here also shapes are analogous and only directions are orthogonal. See the screen captures made for very simple model:

frequencies.png

 

Also the guy wires were installed with an initial pre-tension.  Is thre any way I can model that?  Likewise the conductor was strung with a particular tension.  Is there any way I can model the cable elements to have these initial tensions?

 

 

          It is possible to define cables in Robot by tension. But if all cables are defined this way Robot will try to obtain required tensions in all cables  (by changing length of each cable) SIMULTANEOUSLY for assembling load case and then to fix cable lengths for all consecutive load cases and load combinations. In practice obtaining convergence for such model is impossible - see some remarks in Help:  

http://docs.autodesk.com/RSA/2013/ENU/filesROBOT/GUID-DCDD6D6E-D1BA-4535-9A21-AA28C9277CF7.htm

In reality the assembling of cables  is usually made in SEQUENTIAL way:

1/ one group of cables is assembled with some pre-tensions and if required tension forces are obtained these cables (cable lengths) are fixed

2/ then another group of cables is asembled  with some pre-tensions and if required tension forces are obtained these cables (cable lengths) are fixed too. Usually the assembling of the second group results in changing tension forces in cables of the first group comparing to their original tension forces (from point 1).  So it is different than simultaneous assembling of all cables

3/ then another group of cables is assembled....

....

 

The practical approach may be sequential creation of the model like below:

a/ adding cables corresponding to step 1/ above  defined by tensions and running analysis

b/  checking regulations of cables added in step a/  (see the description of cable regulation in help:  

http://docs.autodesk.com/RSA/2013/ENU/filesROBOT/GUID-0F586BFB-4CFD-4D6F-8DFB-322CEC428E76.htm) and replacing tensions in definitions of these cables by their regulations (input as positive or negative absolute elongations)

c/ adding cables corresponding to step 2/ above  defined by tensions and running analysis

d/ checking regulations of cables added in step c/  and replacing tensions in definitions of these cables by their regulations (input as positive or negative absolute elongations)

e/  adding cables corresponding to step 3/ above ...

... 

 

In the final model only the last assembled group of cables would be defined by tensions - all the previously assembled would be defined by elongations but these elongations would correspond to tensions from previous stages of assembling.

 

I hope these explanations will be useful (and that the last part is clear enough :smileyhappy: )

 

---------------------------------------------
If this post answer your question please click "Accept as Solution". It will help everyone to find answer more quickly!

 

Regards,



Pawel Pulak
Please use plain text.