Modal analysis of pre-stressed beam structure (NX Nastran) 1

[jvacik]

Hello,
I am dealing with relatively simple problem. I would like to perform modal analysis of fully restrained beam with induced stress-state in it (simplification of working screw). I am using Siemens NX8.5. I found some remarks in NX help - I defined SOL 103 Real Eigenvalues solution with static subcase (constraints & bolt pre-load) followed by Eigenvalue Method subcase. After the solution I realized that the natural frequencies do not differ from untensioned state. Does the SOL 103 support the "bolt-preload"? Or did I forget to swith any parameter? Thanks for reply

 

[BlasMolero]

Hello!,
Yes, in fact, you can to perform modal analysis with bolt pre-loading effects + contact surface-to-surface effects with NX NASTRAN.

Since modal analysis is essentially solving the differential equation of free-vibration, the load is not in the equation. So in SOL 103, the load is ignored. There are two method to take into account the pre-loading effects:

• Use SOL103 with STATSUB, or
• Use SOL106.

1. Use STATSUB:
Specifying the gravity load in a static subcase and including the STATSUB case control in the dynamic subcase will cause the differential stiffness to be computed and included in the normal mode solution.
Here you are an example of modal analysis of an assembly with NO contact between components.

And here you are the same model solved using bolt-preload + surface-to.surface contacts plus also node-to-node explicit contact CGAP 1-D elements to take in aaccount the contact with a rigid floor:

For more info take a look to my blog:

http://iberisa.wordpress.com/2011/1...-ensamblaje-con-contactos-surface-to-surface/

2. Use SOL 106:
NX NASTRAN SOL 106 provides an easy way to perform modal analysis with pre-load. The key is to put the METHOD command in the case control and put an eigenvalue card, such as EIRGL, in the bulk data session. Also, param LGDISP needs to be specified to compute the differential stiffness, and NMLOOP should be a value not equal to zero so that the normal modes are computed based on the updated non-linear stiffness.

Here is an example using SOL 106:
$
$ Normal Mode Analysis with Preload - Solution 106
$ Note that LGDISP = 1 is set to get differential stiffness matrix
$ case control METHOD = 10 calls eigenvalue module
$
SOL 106
$
CEND
$
TITLE = Normal Modes with Preload
SUBCASE 1
NLPARM = 1
LOAD = 1
METHOD = 10
SPC = 100
DISPLACEMENT = ALL
$
BEGIN BULK
$
$------8-------8-------8-------8-------8-------8-------8-------8-------8-------
8
$
$ Param Cards
$
PARAM WTMASS 0.00259
PARAM COUPMASS 1
PARAM POST -2
$
$ Nodes
$
GRID 1 0 0. 0. 0.
GRID 2 0 10. 0. 0.
GRID 3 0 20. 0. 0.
GRID 4 0 30. 0. 0.
GRID 5 0 40. 0. 0.
GRID 6 0 50. 0. 0.
GRID 7 0 60. 0. 0.
GRID 8 0 70. 0. 0.
GRID 9 0 80. 0. 0.
GRID 10 0 90. 0. 0.
GRID 11 0 100. 0. 0.
$
$ Bar Elements
$
CBAR 1 11 1 2 0. 1. 0.
CBAR 2 11 2 3 0. 1. 0.
CBAR 3 11 3 4 0. 1. 0.
CBAR 4 11 4 5 0. 1. 0.
CBAR 5 11 5 6 0. 1. 0.
CBAR 6 11 6 7 0. 1. 0.
CBAR 7 11 7 8 0. 1. 0.
CBAR 8 11 8 9 0. 1. 0.
CBAR 9 11 9 10 0. 1. 0.
CBAR 10 11 10 11 0. 1. 0.
$
$ Bar Properties
$
PBARL 11 12 I +
+ 2. 1. 1. .1 .1 .1
$
$ Material Properties
$
MAT1 12 1.0E+7 .33 .101
$
$ Restraints
$
SPC1 100 345 1 THRU 11
SPC1 100 1234 1
SPC1 100 234 11
$
$------8-------8-------8-------8-------8-------8-------8-------8-------8-------
8
$
$ EIGRL Card for Eigenvalue Specification
$
EIGRL 10 3
$
$ PARAM Cards: LGDISP & NMLOOP
$
PARAM LGDISP 1
PARAM NMLOOP 5
$
$ NLPARM Card
$
NLPARM 1 5 AUTO 5 25 PW NO+
+ 0.001 1.0E-7
$
$ FORCE Card
$
FORCE 1 11 0 500. 1. 0. 0.
$
$
ENDDATA

Best regards,
Blas.



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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[jvacik]

Hello,
thank you for providing so much useful information. But, allow me one more question. How did you modelled the preload in bolts joining the deck with the rest of the structure? I watched the video on your website and I didn't noticed any BOLTLD parameter in your static subcase definition, which I intended to use in my working-screw-problem. NX Nastran guide mentioned that the bolt pre-load function is supported in SOL 103 but as I said before - there was no difference in my previous computations.
Thanks in advance for reply.

 

[jvacik]

edit:
Bolt pre-load is supported only in SOL 103 Response simulation

 

[BlasMolero]

Hello!,
NX Nastran provides a contact capability for SOL 101 linear static analysis, and also in consecutive SOLs 103, 105, 111 and 112. According the NX NASTRAN USER's GUIDE manual:

"A contact condition can be included in a normal mode solution (SOL 103), and in an optional dynamic response calculation (SOLs 111 and 112). In the normal mode solution, contact stiffness result is added from the end of the converged linear statics contact solution. The contact stiffness values in the normal mode solution represents the final contact condition of the structure around the contact interface. Thus, it will appear that the resulting contact surfaces are attached during the normal mode analysis. Since the calculated normal modes include the final contact interface conditions, the response calculation (SOLs 111 and 112) which use these normal modes automatically include the same conditions.

The inputs for the normal mode solution are consistent with differential stiffness solutions which require a linear statics subcase. The difference is that the linear statics subcase should include the BCSET case control command. When defining the normal modes subcase, a STATSUB case control command must be included to reference the subcase id containing the contact definition. The contact solution in the linear statics subcase must fully converge before moving to the normal mode portion of the run.

Contact conditions can be used with the element iterative solver. However, differential stiffness conditions cannot be generated with the element iterative solver. Therefore, the default sparse solver will always be used, even when the element iterative solver is requested."

Clear, OK?. Now to the bolts: the typical use of bolt pre-loading is to joint two plates in contact, then this is the reason why you need to define and include surface-to-surface contact between plates in your analysis, the above explain you how to do it.

The NX Nastran approach for bolt preload is very efficient because the entire run is automated allowing for direct entry of the bolt preload forces. During the run, the model is solved twice. The first solution calculates the deformed shape of the bolted medium resulting from bolt preload forces. The software then performs an intermediate calculation. The appropriate compressive forces to apply to the bolts during the second solution are calculated correcting for differences in the length of the bolt model and the loaded length of the actual bolt. Solving the model a second time gives the stress state resulting from bolt preload forces and, optionally, service loads. Bolt preload is supported in SOLs 101, 103, 105, 107 through 112, and 601.

Contact Definition
When a contact definition exists, the contact conditions are included in both solutions. To decrease the solution time, the second solution begins with the contact status from the end of the first solution. As a result, the contact element creation steps and some of the initial contact iterations are avoided in the second solution.

The above demostrates that NX NASTRAN (SOL103) can solve problems with both bolt-preloading and also surface-to-surface contact.

Now to NX Advanced Simulation: In an "SEMODES 103" solution, bolt preload can be added either in 'Static Offset' or 'Stress Stiffening' subcases only. Either one of these 2 subcases should be made active in order for this command to be available. This will add STATSUB = 1 in the case control section of the nx nastran input.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/