Showing results for 
Search instead for 
Do you mean 
Reply
Solved! Go to solution

Frequency dependent damping in response simulation

I want to run Sol 103 Response simulation with frequency dependent damping data. GTAC informs me this is possible in Resp Sim with CBUSH element, so I created a spring and added a lumped mass to test this in a simple example. The physical property (pbush1) table has a 'Dependent properties (pbusht)' tab which I thought would be the place to define my freq dependent viscous damping data as a field, which I did. I left the viscous damping field in 'Nominal Values (pbush)' tab blank, as I already put the freq dependent data as mentioned. I just populated the stiffness tab in the nominal values tab. The resulting FRF from the analysis does not make sense. Very sharp peak, as if there is no damping in the sytem. It almost seems like the freq dependent damping is ignored. Do we know what the problem might be here ? If dependent properties tab is already populated with fields, does one still need to fill the nominal values tab ? i.e in one test case I put freq dependent stiffness and damping data in the dependent tab as fields and left nominal tab completely empty, it did not even run analysis, complaining that 'no stiffness' value was found. A bit confusing. Also, what is the function of the 'nonlinear' field in the 'dependent properties' tab ? Sim, fem files attached. 

 

Thanks

 

Bulent 

6 REPLIES
Solution
Solution
Accepted by topic author Bulent_Goksel
‎05-27-2016 02:39 PM

Re: Frequency dependent damping in response simulation

Hi Bulent,

 

I've got some news for you. Response Simulation doesn't support frequency dependent damping. So, for the solves where you defined no nominal damping on the PBUSH, but frequency dependent damping on the PBUSHT, Response Simulation acted as if there was no damping. Frequency dependent damping support is a good enhancement request for Response Simulation.

 

NX Nastran modal frequency response (SOL 111) does use frequency dependent damping. There you do not have to define a nominal value for the viscous damping if frequency dependent damping is defined. NX will write the following for both physical properties set ups:

 

No nominal damping, frequency dependent damping

$* NX Property: PBUSH1
PBUSH 1 K 1000.00 +
+ B 0.0000
PBUSHT 1 B 1
TABLED1 1 +
+ 10.00001.897500 20.00001.802625 30.00001.707750 40.00001.612875+
+ 50.00001.518000 60.00001.423125 70.00001.328250 80.00001.233375+
+ 90.00001.138500100.00001.043625 ENDT

 

Nominal damping, frequency dependent damping

$* NX Property: PBUSH1
PBUSH 1 K 1000.00 +
+ B 1000.00
PBUSHT 1 B 1
TABLED1 1 +
+ 10.00001.897500 20.00001.802625 30.00001.707750 40.00001.612875+
+ 50.00001.518000 60.00001.423125 70.00001.328250 80.00001.233375+
+ 90.00001.138500100.00001.043625 ENDT

 

Both setups produce the same frequency (damped) response.

 

Regards,

Mark

 

Mark Lamping

Simulation Product Management

Simulation and Test Solutions

 

Siemens Industry Sector

Siemens Product Lifecycle Management Software Inc.

mark.lamping@siemens.com

www.siemens.com/plm

Re: Frequency dependent damping in response simulation

Hi Mark,

 

Thanks for the quick and detailed response. I tried it, it worked. Very helpful, as usual.

 

Few questions / comments to make sure I got my facts straight.

 

1) Only Sol 111 supports freq dependent damping in phy properties for cbush, but not sol 103 Response Simulation or sol 108 direct FR ? 

 

2) For elements other than cbush (i.e shell, solid), even though it is possible to define a frequency dependent Structural damping Coefficient GE using fields in defining the material, my understanding is that NX CAE does not incorporate that to the input deck. One has to manually edit the input deck, with the freq dependent material data, to solve. And that is only available for Sol 108 but not Sol 103 Response Sim or Sol 111 ?

 

3) With Sol 103 response simulation, it is still possible to modify % viscous damping for each mode by right clicking and editing in the 'Response Simulation details view'.

 

4) For the cases where defining a frequency based damping is allowed (either in material or phy prop creation) but not recognized and ignored by the solver, it would really be helpful if NX raises a flag and warns the user, either in info window, solution monitor or in f06 file but definitely somewhere.

 

5) In the dependent properties (pbusht) portion of the phy prop table for cbush, there is a 'Nonlinear' field. What is its use case ? The reason I am asking this is because, as the next phase of this investigation, I want to make the spring nonlinear (hardening). i.e 'Duffing equation' type of problem. I was wondering if that would be the field to enter this nonlinear F vs x relationship. I suppose I will also have to switch to sol 129 or sol 601,129 types as this now beomes a nonlinear problem.

 

Regards

 

Bulent

Re: Frequency dependent damping in response simulation

Bulent,

 

Here's my attempt at answering each question. I can't guarantee this is all correct as I'm getting into some deep water.

 

1. Correct, correct, incorrect. SOL 111 and SOL 103 both perform normal modes calculations. Normal modes calculations don’t take damping into account, but modal damping is output. To be safe, I’m not sure if there’s a difference between the modal damping calculations related to SOL 111 and 103 response simulation. For certain, the frequency dependent damping of the CBUSH is taken into account during the response portion of SOL 111. The response portion related to SOL 103 response solution doesn’t take place in NX Nastran. It takes place in NX Response Simulation. For certain, NX Response Simulation does NOT take into account frequency dependent CBUSH properties. SOL 108 direct frequency response does indeed support frequency dependent CBUSH properties. 

 

2.  Incorrect and correct. Damping can be exported as a real value. NX does export the material damping coefficient as the GE field on the MATi bulk data entries. You have to define it as a REAL value since NX Nastran doesn’t support GE as a table (i.e. cannot be frequency dependent). If you define it as a frequency dependent table (perhaps other solvers support this), the export to NX Nastran will skip the export of GE. If the material doesn’t support frequency dependent material damping coefficients, the different solutions certainly won’t either.

 

3. Correct

 

4. Yes I agree. This would be best caught during export to the solver. It’s a good enhancement request.

 

5. The Nonlinear portion of the dialog addresses the PBUSHT’s ability to represent a nonlinear force-deflection spring. The PBUSHT quick reference guide entry states that it can have frequency dependent or displacement dependent representations. If you define a new field for one of the stiffness components in PBUSHT’s main dialog, you will see that it only allows frequency dependence. Under the Nonlinear portion, it will only allow displacement dependence. The displacement dependence representation is only used in nonlinear solutions.

 

Regards,

Mark

Re: Frequency dependent damping in response simulation

I would like to point out that in case of Modal Frequency Response analysis the PBUSHT entry is correctly written in dat file while exporting from Femap 11.2.1, but unfortunately in case of Random Response Analysis this entry is not present in the input file. Both analysis use the same solution SOL111. This entry need to be add manually and NX Nastran will take it into account during solution.

Re: Frequency dependent damping in response simulation

That's not correct. Response Simulation does not use SOL 111. For instance, never will you see SOL 111 in an input file generated from an NX solution that is created as SOL 103 - Response Simulation. Response Simulation uses SOL 103 to calculate modes and other data, but the responses are calculated by Response Simulation and not NX Nastran. Frequency dependent dampers aren't supported by Response Simulation, whereas they are by SOL 111.

 

Regards,

Mark

Re: Frequency dependent damping in response simulation

I drew my conclusions based on two simulations. I performed Random Vibration analysis with PSD function defined:

 

=====================================

SOL SEMFREQ

RANDOM = 200

RANDPS       200       1       1      1.      0.      11

=====================================

 

In the first model I defined only the PBUSH entry:

 

=============================================

PBUSH    5000003       K      6.      7.      7.      8.      9.      9.+      

+                      B     10.   

=============================================

 

, and in the second I added the PBUSHT entry with frequency dependent tables:

 

==============================================

PBUSHT   5000003       K       6       7       7       8       9       9+

+                      B      10

TABLED2        6 …

TABLED2        10 …

=============================================

 

The normal mode frequency increased and the response of the node on the structure significantly decreased. These results make me confused. What can cause these differences?