Robot Structural Analysis Forum
Welcome to Autodesk’s Robot Structural Analysis Forums. Share your knowledge, ask questions, and explore popular Robot Structural Analysis topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Eigen Values / Natural Frequencies

12 REPLIES 12
Reply
Message 1 of 13
greg.parent
3997 Views, 12 Replies

Eigen Values / Natural Frequencies

I am reviewing the design of a guyed transmission line tower and I need to calculate the periods/natural frequency of this structure.  I can model it in Robot but I was wondering how to analyze the structure to obtain the 1st and 2nd mode of the natural frequency of this structure. 

 

I have searched this on the Robot user manual and found related topics under: Table Columns/Eigenvalue.  However I am having no luck getting the Eigenvalues tab to appear.  I need some direction on how to do this.

 

Any advice?

 

-Greg  

12 REPLIES 12
Message 2 of 13
tony.ridley
in reply to: greg.parent

Hi mate,

 

You need to run a modal analysis. 

Set up number of modes, and add load to mass conversion if necessary. 

 

After analysis go to results----------->advanced------------->modal analysis.  This will give you the frequencies and associated eigenvalues etc.

 

Tony

Message 3 of 13
Pawel.Pulak
in reply to: tony.ridley

Greg,

If you run this modal analysis for a guyed transmission line tower with cable elements pay attention to loads in static load case directly preceding the modal load case.

Modal load case will use cable stiffness from this case. It means that changing static loads in preceding load case (and thus changing stiffness of cables) you will receive different frequencies of vibrations.

 

More details in:

1/ Rafal's answer in this post: http://forums.autodesk.com/t5/Autodesk-Robot-Structural/Barre-de-treillis-traction-compression-vs-s%...

2/ my answer in this post: http://forums.autodesk.com/t5/Autodesk-Robot-Structural/Seismic-load-combinations/m-p/3495432/highli...

 

Regards,

 


Pawel Pulak
Technical Account Specialist
Message 4 of 13
greg.parent
in reply to: greg.parent

Thank you for your reply, it definitely got me going in the right direction. 

 

Had another question however,  I set up the modal analysis to check 5 modes.  The first two modes had the exact same natural frequency and period.  The third mode was much higher and the fourth and fifth modes did not calculate a natural frequency or period it just gave a value of “N/A” for everything.

 

It seemed odd to me that the first two modes would have the exact same frequency and period.  Shouldn’t the second mode have a much higher natural frequency?  (See attachment)

 

Also my structure is not supported symmetrically, there are guy wires supporting the lateral load in only one direction.  Does this modal analysis analyze natural frequencies and period in different directions?

 

Thank you

Message 5 of 13
Romanich
in reply to: greg.parent

First natural frequency is always lower than second, second lower than third and etc.

Do you find the posts helpful? "LIKE" these posts!
Have your question been answered successfully? Click 'ACCEPT SOLUTION' button.

Roman Zhelezniak

Robot Evangelist & Passionate Civil Structural Engineer

LinkedIn | Robot & Хобот | App Store for Robot
EESignature


Message 6 of 13
Rafal.Gaweda
in reply to: greg.parent

Send us model to check



Rafal Gaweda
Message 7 of 13
tony.ridley
in reply to: greg.parent

The first two modes had the exact same natural frequency and period.  The third mode was much higher and the fourth and fifth modes did not calculate a natural frequency or period it just gave a value of “N/A” for everything. 

It seemed odd to me that the first two modes would have the exact same frequency and period.  Shouldn’t the second mode have a much higher natural frequency? 

 

Just be careful with how you understand modal analysis.  The term "natural" frequency is not applied to every mode.  Every mode has a frequency associated with it.  That may not be the "natural" one for the structure.  If you only get three modes this could be OK for a simple structure, depends on a lot of things.  

 

 

Also my structure is not supported symmetrically, there are guy wires supporting the lateral load in only one direction.  Does this modal analysis analyze natural frequencies and period in different directions?

 

Check Pawels post from earlier.  If you are using cables as guy wires they may not activate in the modal analysis depending.  Frequency and period are essentially the same thing reported in a different way, but neither depend on X, Y, or Z global directions.  The mode shape is what it is regardless of xyz direction.

 

Message 8 of 13
greg.parent
in reply to: Rafal.Gaweda

I am having an issue attaching the Robot Structural analysis Professional 2011 file.  It gives me the following warning:

 

Please correct the highlighted errors and try again.

  • The file does not have a valid extension for an attachment. doc,pdf,dwf,dwg,dxf,dst,gz,gzip,zip,bm,bmp,gif,jfif,jpe,jpeg,jpg,psd,tif,tiff,png,htm,html,xml,xls,lsp,svf,3ds,vcf,png,text,txt,log,env,dcl,rvt,rfa,ipt,iam,ipn,dwfx,idw,csv,nwf,nwc,nwd,sdf,cfz,vtfx,vtf are the valid extensions.

I believe that the Robot extension is: ".rtd" but that is not one of the valid extension types listed above.

 

Please let me know how I should attach the Robot Structural analysis Professional 2011 file that I have created.  Thank you,

 

-Greg

Message 9 of 13
Romanich
in reply to: greg.parent

Use *.zip format file

Do you find the posts helpful? "LIKE" these posts!
Have your question been answered successfully? Click 'ACCEPT SOLUTION' button.

Roman Zhelezniak

Robot Evangelist & Passionate Civil Structural Engineer

LinkedIn | Robot & Хобот | App Store for Robot
EESignature


Message 10 of 13
greg.parent
in reply to: greg.parent

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.

Message 11 of 13
greg.parent
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.

Message 12 of 13
Pawel.Pulak
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 🙂 )

 

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

 

Regards,


Pawel Pulak
Technical Account Specialist
Message 13 of 13
aghdaapr
in reply to: greg.parent

Hello!

 

As you know, a robot is a multi-body system and there is not specific natural frequency in general. It means that for a specific joints' configuration, there is a unique eigenfrequencies, however, they alter as soon as the joints' configuration change. I have written a book and instructed how to extract the natural frequencies through model-based as well as Inventor. I recommend to read it and let me know if you have further problem.

 

Best regards

Amirhossein Aghdasi

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report