femap constraint 1

[xzooom1]

hello ,

i modeled 2d laminate type surface i intend to model simply supported beam (composite) but when i made an anlysis using NX Nastran it give me an error

the error code is 9137 and it belongs to constraints

plz hellp how i can model the simply supported beam(laminate ) correctly on femap to avoid this error? .

 

[rb1957]

i think you're not constraining the 6 rigid body motions. i suspect you're thinking in terms of the beam and how it works, and you've probably got two force contraints (2 Fy ?) that react 2 rigid body motions(Fy, Mz); you might have a third (Fx). but you need to contrain the other degrees of motion as well (particulary torsion, along the axis of the beam).

 

[xzooom1]

plz can you tell me how i tested all constraints types the same error!!!!!!

 

[rb1957]

how many constraints do you have on the model ?

 

[xzooom1]

ok thanx all things fine now thanx for reply

but can you help me how to make frequency analysis using femap ???

 

[BlasMolero]

Frequency analysis is the most simplest analysis type in any FE code, you can arrive to a solution independly if your model is correctly constrained or exhibit rigid body motions. Then, if you have problems solving a freq. analysis it means that your FE model have another issue. Please check you have defined correctly the material properties, i.e., density. Also if thickness is prescribed, etc.. check that basic items.

You have in the FEMAP & NX NASTRAN EXAMPLE manuals a few examples of frequency analysis, please run previosly to use the program to run real life problems.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

 

[xzooom1]

thanx , but i have problem how to sort node when i list the results , the results appear sorted by number only

i need to sort it by node location with respect to x direction

thanx for reply ...

 

[BlasMolero]

Dear Xzoom1,
USER FATAL MESSAGE 9137 means the following (see NX Nastran error list):

RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX K(F-R,F-R). USER ACTION: CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO
CONTINUE THE RUN WITH MECHANISMS.

The reason: your model is not correctly constrained, you have rigid body motions, then revise your model. But as I told you before this mesage don't appear in a frequency analysis (SEMODES SOL103) because the proper solver is capable to compute rigid body motions in any direction.

If you receive this message is because you are running -say- a Linear Static Analysis (SESTATIC SOL101). Then, a debugging method is to include in the Nastran Bulk Data Section the command PARAM,BAILOUT,-1
HOW?. Simply go to "Model > Analysis > Preview Input > Edit Preview" and include the above command in the Bulk Data section, por instance:

BEGIN BULK
$ ***************************************************************************
$ Written by : Femap with NX Nastran
$ Version : 10.1.1
$ Translator : NX Nastran
$ From Model :
$ Date : Fri Apr 30 09:21:38 2010
$ ***************************************************************************
$
PARAM,BAILOUT,-1
PARAM,POST,-1
PARAM,OGEOM,NO
PARAM,AUTOSPC,YES
PARAM,K6ROT,100.
PARAM,GRDPNT,0

And finally click in ANALYZE and you are done.
But CAUTION!!, this "trick" is to see what/where rigid body motion exist in order to define a correct prescribed model, if you go to postprocessing and plot displacements results you will see values of say 1e10, then the solution is meaningless.

Another "trick" I use a lot to check models not correctly constrained is simply to perform a freq. analysis (SEMODES SOL103), animating the rigid body motions will tell you what constraint is missing ... simply!!.


Now returning to your last question: "sorting nodes by location respect to x-direction". Simply make a group of nodes where to plot results, and if you want to generate an XYPLOT of the response along X-Diretion go to F5 > XY vs. Position > Click on XY Data > select the active group, the active "output set", the ative "output vector", the X-axis, and click OK + OK, you are done!!.
Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

 

[xzooom1]

thank you

i have another question :

which is the best element type you prefer when you model composite body for example beam ?

now i use 3d solid geometry to model the beam and add layer when i construct the model , is it correct or not ?

plz tell me wich is the best elent type for composite

thank you very much to you for reply ...