Random and Frequency Response Analysis Displ

[crostolo]

Hi all,
if I have a classical model, linked to a single node by mean a RBE2 element, in order to apply loads with the Large Mass Method for Random Analysis and Frequency Response Analysis; is there a way to display the relative displacement (relative to the base node)?

What I mean is that the deformation you get from the results of these analysis show the "displacement" of the whole model (model and base node of the large mass method).
Is there, at least, a way to substract from all the node of the model the displacement of the base node (the node where is applied the input load for the large mass method)?

Thanks for the answer
crostolo

 

[RealSaladsamurai]

Hi crostolo: Here is how I accomplish this.

Create a node somewhere in space. The location is arbitrary, it is only used as a "container" to store the subtracted relative displacement results. That being said, I like to put it close to the actual node of interest so I remember which result it is storing.

Then go to Model > Constraint > Equation. I create a constraint equation for each DOF that I want relative displacements in. As a concrete example, assume that the base input node (attached to seismic mass) is N_S, the node of interest is N, and the arbitrarily placed container node is N_C.

The idea is to end up with an equation of the form (in x-direction for example):
N_Cx = Nx - N_Sx
or
-N_Cx - N_Sx + Nx = 0.

The order that you select the nodes is the order that the terms of the equation will be written and you NEED -N_Cx to appear first, so select it first.

For more information, see MPC in the Nastran Quick Reference Guide.

Also note that if you go back into Femap to edit this equation, Femap will list (in the edit equation GUI) the nodes that you selected in ascending order and not necessarily in the order you selected them. I think this is an oversight since it makes it difficult to quickly see what your MPC looks like in Femap ... you will need to go to the Nastran deck to confirm (whick is always a good idea anyway!).

Hope that helps.

________________________
FEMAP v11.1.0
MSC Nastran v2013

 

[jbrackin]

You should be able to use Femap to display the relative deformation. Try the following in the postprocessing toolbox:
Create/Select Deformed style; Select the output set and vector of interest(RMS values t3 displacement)
under "options" see "Deform Relative To"; change from origin to fixed node and then select the large mass node as the fixed node.

Now your deformed plot is relative to the large mass node displacement. You can then use data table, or just the select tool, to look at nodes of interest.

 

[BlasMolero]

Hello!,
Please note in FEMAP activating the option "Relative Enforced Motion Results" in the NASTRAN Output Request it can be used recover relative results from an enforced motion analysis.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[RealSaladsamurai]

Blas: My option for Relative Enforced Motion Results is GRAY and so I cannot select it. I assume that I have made some other selection somewhere that is interfering with it. It is a modal frequency response using an applied acceleration (SPCD). Any thoughts?

________________________
FEMAP v11.1.0
MSC Nastran v2013

 

[BlasMolero]

Hello!,
Precisely this picture is from my blog where I run an enforced motion Modal Frequency Response (SOL111), ie, a Sine Frequency Swept under an enforced motion AY=0.25G in the frequency range between 0-500 Hz, here you are the post:

https://iberisa.wordpress.com/2013/...on-modal-frequency-response-dynamic-analysis/

Here you are the answer:

Best regards,
Blas.


~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[RealSaladsamurai]

Hi Blas - I cannot select the option. See image.

________________________
FEMAP v11.1.0
MSC Nastran v2013

 

[BlasMolero]

Hello!,
I run NX NASTRAN solver. I note your firm say FEMAP v11.1.0 & MSC Nastran V2013, then this could be the reason??.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[RealSaladsamurai]

Probably! BURNT AGAIN BY MSC!!!

Thanks again Blas!

________________________
FEMAP v11.1.0
MSC Nastran v2013