I have a following question concerning NX 8.5-12 (SOL103 Response Dynamics): is it possible to introduce different damping coefficients for the different properties (shell/solid) when you evaluate FRF in SOL103?
For example, it's possible to do it using SOL111 (specifying both different Damping Coefficients for the different properties and PARAM,W4),
but as I got SOL103 Response Dynamics ignores the damping coefficients specified in the properties cards and considers only a damping factor for a whole model (Response dynamics -> Natural Frequencies -> Modal Represantation -> Normal Modes -> Edit Damping Factor).
Solved! Go to Solution.
For Frequency and Transient events, you can include in your Response Simulation evaluations the physical viscous and/or hysteretic damping calculated by NX Nastran. Before solving the model, add the appropriate elements (such as dampers, bushings, or springs) or material damping in your FEM as listed below. You can also define global structural damping in the G parameter for the solution.
To define viscous damping:
To define hysteretic (structural) damping:
After you solve the model and create the Response Simulation solution process, use the Physical Damping Settings dialog box to enable the physical damping in your response evaluations and optionally enter a Scale factor.
You can view the percentage of the damping ratio for each mode in the Response Simulation Details View in the %Phys Visc and %Phys Hyst columns. The values displayed are the diagonal terms of the viscous damping matrix or hysteretic damping matrix multiplied by any Scale factor you defined
Thank you for your reply, Steve!
I did as it's advised:
1. Specified a material damping GE using GUI (then checked - it's printed in the input .dat file automatically - didn't get why you advised to add it to the input file manually);
2. After I had solved it and created the Response Simulation solution process I checked in the Physical Damping Settings dialog box that the physical damping in my response evaluations is enabled.
3. But still both %Phys Visc and %Phys Hyst are 0%.
I checked it either for PSHELL or PCOMP - still it doesn't work in both cases (basically, I need a damping model for PCOMP type).
I managed to get %Phys Visc or %Phys Hyst greater than 0% only when I specify the damping using "Edit damping Factors" dialog box, but it introduces the specified damping for a whole model - but I don't need it at all, cause for some properties I need a damping equal to 0%.
Looking forward to your reply!
Yes, you are correct about not needing to add the GE value manually. That was for an older version where it wasn't yet supported in the UI. I created a simple shell model using a PSHELL and set the GE value to .2 for the material. The damping showed up as 20% in the % Phys Hyst column of the Response Dynamics Details view. However, when I tried using a PCOMP, I do not seem to get the damping either. If you want to send me your dat file for the PSHELL case, I can check it. I'll have to see why the PCOMP doesn't seem to work.
I found the reason why it didn't work (I think it would be a useful information for other users):
The point is that I launched SOL103 Real Eigenvalues (in conjunction with dynamic response) and if I specified PARAM,OUGCORF,GLOBAL either by GUI or manually - anyway solver deletes this parameter - probably that's a reason why I didn't get the physical damping.
To cut the long story short, you don't even have to specify that PARAM with SOL103 Response Dynamics - with that solver everything works well.
Ok, yes, you must use the "SOL103 Response Dynamics" Solution to be be able to get the damping back to Response Dynamics. This solution outputs the necessary damping information for RD that the plain "SOL 103 Real Eigenvalues" solution does not.
Glad you got it working now. If yo uneed anything else, let me know.