sunusoidal load nastran

[marouaha]

hi,
i need to simulate a sample excited with a shaker.
i must imput a sunusoidal displacement at the clamped end of the sample and the i recover the response from the free end .
i use the dirct frequency response analysis.
i ask if some one can help me to imput the sinusoidal displacement.

 

[Rhei]

Hi,
this is an example of what cards you should use to apply the excitation as enforced displacement by means of the Direct Enforced Motion method:

$ This card is the one which groups all the loads you have in your analysis, in this case only the enforced motion
$DLOAD, SID, S, S1, L1
DLOAD, 2, 1., 1., 8
$
$RLOAD2, SID, EXCID, DELAY, DPHASE, TB, TP, TYPE
RLOAD2, 8, 9, , , 7, , DISP
$
$ Assuming you are exciting from 20 to 100 Hz and the amplitude of your excitation is constant and equal to 5g
TABLED1, 7
,20., 5., 100., 5., ENDT
$
$ The node to which you apply the SPCD card (so the enforced motion) must be constrained, therefore you need an SPC card also
$SPCD, SID, G1, C1, D1
SPCD, 9, 16, 3, 1.
$ Since it is a clamped end, you need to constrain all the dofs, included the one used for the enforced motion (in this case it is number 3)
SPC1, 1, 123456, 1, 16,

 

[marouaha]

thx,
I work with msc nstran with patran 12.2.

 

[Rhei]

The part of code I posted earlier is exactly for msc nastran.
Once you have created your finite element model using patran, just open the .bdf file and add the code I gave you in your file.
Then you just need to change some values according to your needs. I will repeat the code here to show which parts you need to change:

$DLOAD, SID, S, S1, L1
DLOAD, 2, 1., 1., 8
$
$RLOAD2, SID, EXCID, DELAY, DPHASE, TB, TP, TYPE
RLOAD2, 8, 9, , , 7, , DISP
$
$ Change the frequency values and the magnitude
TABLED1, 7
,20., 5., 100., 5., ENDT
$
$ Change the grid point to which you want to apply the excitation (16) and the direction in which you want to give it (3)
$SPCD, SID, G1, C1, D1
SPCD, 9, 16, 3, 1.
$ Change the grid point (16), it has to be equal to the one tou defined in the SPCD card
SPC1, 1, 123456, 1, 16,

Also, in your Case Control section (which means, before the BEGIN BULK) you need to add these 2 lines:
SPC = 1
DLOAD = 2

Finally, have a look at this website about Patran:

http://web.mscsoftware.com/patran/c...ic_functions&topic=HTOC_p3_patran_main_window

you might find something useful

 

[marouaha]

thx again,
can you tell if nastran can determine the damping effect of friction between to plate.

 

[Rhei]

Not in a frequency response analysis (SOL108), because contact is a nonlinear condition, whereas SOL108 is a linear solution. Therefore you will need to use a transient solution (like SOL109) and input a sine wave

 

[marouaha]

thx ,
so can i have the modal damping and the friction damping of the bending modes?

 

[Rhei]

Not sure what you mean, but if you need to define the modal damping you have to use the TABDMP1 card, which needs to be activated by a SDAMPING card in the Case Control

 

[marouaha]

Hello olgola,
Thanks for the reply
the problem definition is:

I work with msc nstran with patran 12.2. I use to simulate a sample excited with a shaker.
i must imput a sunusoidal displacement at the clamped end of the sample and then i recover the response from the free end. Then, i must introduce the friction coefficient.
finallyi need to determine the modal damping 'including the friction effect'.

 

[marouaha]

using sol 109 or 112 i can't get the modal analysis. i attached my .bdf file.
i apply the following time dependent force t f
0 0
0.0075 45
0.015 0
0.025 -45
0.03 0
i don't know how to modify this card like you have suggest. "activate TABDMP1 card by a SDAMPING card in the Case Control
Regards

 

[marouaha]

i determine the damping using the strain energy methode by the stress element and the strain element of every bending mode

 

[Rhei]

First of all, if you have to work with modal damping you need SOL112, not the 109, because the 109 is a direct solution, which means it does not compute the normal modes and also you cannot define modal damping.

Then, there is something that is not clear in your setup: your beam is clamped therefore you have all the dofs 123456 in the SPC1 card, but then you apply a force to a grid (9704)which is close to the fixed end. If this is meant to reproduce the base-shaking condition it will not work, because you are not moving the beam base since it is completely fixed.
The cards you need to have in your input file are the ones I told you in my previous posts (since you are using a transient solution you need the TLOAD2 card instead of the RLOAD2, but all the others are the same).
Unfortunately I do not know how to set it up using Patran.

To define modal damping in Patran have a look here:

http://www.scc.kit.edu/scc/sw/msc/Nas102/prob04.pdf

at pages 13-14 and see if you manage to do it

 

[marouaha]

hello thinx,
I constraint the dofs 1.3.4.5.6 dof and i apply a sine wave at the clamped end but when i plot the results the beam translate in the y direction. i dont obtaine the mode shape. have you any proposition. the attached file is the bdf card of the model.

 

[Rhei]

Hi,
your beam translates in the y direction because it is not constrained, thus it has a rigid body mode.
To constraint the y direction you need to add number 2 in your constrained dofs (which will be 123456).
To simulate the base motion you must not use an input defined as a FORCE.

Have a look at the first video in this page:

https://www.google.fr/webhp?sourceid=chrome-instant&ion=1&espv=2&ie=UTF-8#q=patran base motion

it should explain how to do it in Patran. Try also thus one

https://www.youtube.com/watch?v=nxcj4TbnDt8&feature=youtu.be