I am trying to analyze a forced excitation of a structure. The excitation node needs a 30Hz, 0-to-peak 0.050" input. From my understanding, this is a forced displacement problem. All I've been able to find is information on inputting acceleration. Does anyone have tips, guides, examples that I could follow? TIA
Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations JAE on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Frequency Response, forced displacement
- Thread starter Caleb_101
- Start date
Hi
From your question I assume that you want to do this in time domain (time-history analysis). And since this is the Femap forum I assume that you use Nastran. The approach is probably valid for other solvers also, perhaps with some modification.
A few suggested steps:
On the node you want to excite, apply a constraint for the DOF you want to excite. This constraint should be in addition to your general constraints for the structure.
Next create a sinus function in time domain, basically a time dependent function with amplitude as function of time (vs Time). I suggest that you use 1.0 as peak amplitude.
Then create a displacement load on the node you want to excite for the DOF you want to excite. Use you required amplitude value for the displacement and make it dependent of the time function you just created.
Now you have a displacement with a time dependent amplitude function, and the constraint will ensure the the node is forced to move as requested.
So, now you use the constraint set and the load set to set up the Time-History Analysis.
I hope you can make it work now.
Good luck.
Thomas
From your question I assume that you want to do this in time domain (time-history analysis). And since this is the Femap forum I assume that you use Nastran. The approach is probably valid for other solvers also, perhaps with some modification.
A few suggested steps:
On the node you want to excite, apply a constraint for the DOF you want to excite. This constraint should be in addition to your general constraints for the structure.
Next create a sinus function in time domain, basically a time dependent function with amplitude as function of time (vs Time). I suggest that you use 1.0 as peak amplitude.
Then create a displacement load on the node you want to excite for the DOF you want to excite. Use you required amplitude value for the displacement and make it dependent of the time function you just created.
Now you have a displacement with a time dependent amplitude function, and the constraint will ensure the the node is forced to move as requested.
So, now you use the constraint set and the load set to set up the Time-History Analysis.
I hope you can make it work now.
Good luck.
Thomas
BlasMolero
Mechanical
Dear Caleb,
The first data to have exactly defined in a finite element analysis problem is to identify clearly the excitation: this will tells you if the problem is linear o nonlinear, static or transient dynamic, ie, the type of analysis run. When the word "Hz" appear in any excitation this is dynamic problem, but we need to know more if the analysis should be solved in the frequency domain or time domain. Yes, because in the case of Simcenter NASTRAN we have many methods to solve dynamic problems: direct & modal, and also time & frequency domain, really rich.
• SEDFREQ SOL108: Direct Frequency Response Dynamic Analysis
• SEDTRAN SOL109: Direct Transient Response Dynamic Analysis
• SEMFREQ SOL111: Modal Frequency Response Dynamic Analysis (freq domain)
• SEMTRAN SOL112: Modal Transient Response Dynamic Analysis (ie, Modal Time History Analysis, time domain)
I prefer to work always in the frequency domain, is faster, then I try to use always the SOL111 & SOL112 modal methods based in normal modes performing previously the eigenvalue analysis (SOL103), forget al all the direct ones. In the modal methods the accuracy of the dynamic response is based in the number of modes extracted & used to compute the response, and this is very easy to achieve & control by end user: the sum of modal mass should be always above of 85% of the total mass of the system in the direction of the excitation, easy!!
In your case, you mention words 30 Hz & peak displacement: this means you need to apply to the base node a transient displacement to represent a 30 Hz single sine pulse defined in the time domain.
To learn how to define a sine function visit my blog here:
iberisa.wordpress.com
Basically:
• Use command MODEL > FUNCTION
• Select the Equation radio button and enter the following values (I like to use 24 points to define the sine pulse function):
Delta X = 1/30/24
X = 0 Y = sin(360*30*!x)
To X = 1/30
• Click the SINGLE VALUE button and enter the following values, this will expand the function till end time=0.05 s
X = 0.05 Y = 0
The resulting function curve will be the following:
Then when you apply the enforced displacement to the base node of the spider rigid RBE2 element prease associate the loading with this function and you are done!!.
Of course, the analysis type will be Modal Transient Response Dynamic Analysis (SEMTRAN SOL112), also know as Modal Time History Analysis.
To learn more please visit my Support website in the following address:
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48004 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
The first data to have exactly defined in a finite element analysis problem is to identify clearly the excitation: this will tells you if the problem is linear o nonlinear, static or transient dynamic, ie, the type of analysis run. When the word "Hz" appear in any excitation this is dynamic problem, but we need to know more if the analysis should be solved in the frequency domain or time domain. Yes, because in the case of Simcenter NASTRAN we have many methods to solve dynamic problems: direct & modal, and also time & frequency domain, really rich.
• SEDFREQ SOL108: Direct Frequency Response Dynamic Analysis
• SEDTRAN SOL109: Direct Transient Response Dynamic Analysis
• SEMFREQ SOL111: Modal Frequency Response Dynamic Analysis (freq domain)
• SEMTRAN SOL112: Modal Transient Response Dynamic Analysis (ie, Modal Time History Analysis, time domain)
I prefer to work always in the frequency domain, is faster, then I try to use always the SOL111 & SOL112 modal methods based in normal modes performing previously the eigenvalue analysis (SOL103), forget al all the direct ones. In the modal methods the accuracy of the dynamic response is based in the number of modes extracted & used to compute the response, and this is very easy to achieve & control by end user: the sum of modal mass should be always above of 85% of the total mass of the system in the direction of the excitation, easy!!
In your case, you mention words 30 Hz & peak displacement: this means you need to apply to the base node a transient displacement to represent a 30 Hz single sine pulse defined in the time domain.
To learn how to define a sine function visit my blog here:
• Ejemplos de Mallado con FEMAP
Consejos de Mallado y Análisis por Elementos Finitos con Simcenter FEMAP y Simcenter Nastran A menudo publico vídeos en mi canal de YOUTUBE con consejos de mallado y análisis por Elementos Finitos …
iberisa.wordpress.com
Basically:
• Use command MODEL > FUNCTION
• Select the Equation radio button and enter the following values (I like to use 24 points to define the sine pulse function):
Delta X = 1/30/24
X = 0 Y = sin(360*30*!x)
To X = 1/30
• Click the SINGLE VALUE button and enter the following values, this will expand the function till end time=0.05 s
X = 0.05 Y = 0
The resulting function curve will be the following:
Then when you apply the enforced displacement to the base node of the spider rigid RBE2 element prease associate the loading with this function and you are done!!.
Of course, the analysis type will be Modal Transient Response Dynamic Analysis (SEMTRAN SOL112), also know as Modal Time History Analysis.
To learn more please visit my Support website in the following address:
Best regards,
Blas.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48004 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
- Status
Similar threads
- Locked
- Question