turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- CAE Simulation - Femap Forum
- Buckling with Bar Offsets

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-08-2015 11:55 AM

I have a FE model of an isogridded plate: shell elements for the surface, and bar elements to represent the ribs. Ideally, the bars would all be offset to represent that the ribs are all machined on 1 side of the plate, not both sides.

Does anyone know if NX Nastran 10.1 supports a buckling solution (SEBUCKL) using bar elements with offsets?

The NX Nastran User's Guide says "Offsets should not be used in beam, plate, or shell elements (except CQUADR/CTRIAR) for buckling analysis." I seem to recall MSC Nastran fatal error messages in the past when you tried this, but I've read that MSC Nastran 2012 has a parameter (MDLPRM) that will now allow it.

With offsets, Femap & NX Nastran 10.1 allowed it to run with no apparent error. Are these results just spurious?

Thanks,

Chris

1 REPLY

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-08-2015 01:38 PM

Dear Chris,

In NX NASTRAN v10 the linear buckling analysis (SOL105) still has the offset restriction, the reason is because **the offset vectors remain parallel to their original orientation when computing the differential stiffness**. The specification of offset vectors is not recommended because may produce incorrect results. Please remember that the basic assumption in linear buckling is that the differential stiffness [*Kdaa*] is proportional to the applied load {*Pa*}. The assumption implies a linear material law and small deformations.

A little of history: the differential stiffness formulation for the CQUAD4 and CTRIA3 elements was changed in Version 68. Numerous spurious modes appeared in linear buckling of thin shell structures using versions prior to Version 68. The improved results of Version 68 can be produced with a version earlier than Version 68 by overlapping two CQUAD4 or CTRIA3 elements, one with bending stiffness only and one with membrane stiffness only. The pre-Version 68 method of calculating the differential stiffness may be activated in Version 68 by setting the system cell NASTRAN SYSTEM(170)=1 in the NASTRAN statement. The Version 68 method is the default, NASTRAN SYSTEM(170)=0. The pre-Version 68 method remains in the code to recover old results.

The following recommendations apply to linear buckling analysis.

Use at least 5 elements per half sine wave to get reasonable results in the buckling load.

For buckling of 3-D shell structures, use PARAM,K6ROT,100. to assign a stiffness to the sixth degree-of-freedom. The default is PARAM,K6ROT,0.

The following restrictions apply to linear buckling analysis (SOL105):

**Offsets should not be used in beam, plate or shell elements. The buckling loads for structures with offsets are incorrect.**Follower force effects are not included in the differential stiffness. The calculated buckling loads are incorrect. The Bulk Data entries FORCE1, FORCE2, MOMENT1, MOMENT2, PLOAD, PLOAD2, PLOAD4, RFORCE, TEMP, TEMPD, TEMPP1, TEMPP3, TEMPRB describe follower forces.

For structures that exhibit geometric nonlinearities as large deflection deformations, the linear buckling load obtained from Solution 105 may be different than the actual buckling load. For structures with significant nonlinearities, it is recommended that you perform a Nonlinear Buckling Analysis using NX NASTRAN (SOL106).

But please note that in **Nonlinear Buckling Analysis using NX NASTRAN (SOL106)** the specification of offset vectors is not permitted, the analysis gives FATAL ERROR. However, setting SYSTEM(463)=1 will disable the FATAL error message and the analysis will be allowed to continue (with offset vectors remaining parallel to their original orientation). The use of this system cell may generate incorrect results. Loading conditions that generate follower forces should not be used when SYSTEM(463) = 1. Use PARAM,FOLLOWK,NO if follower boundary conditions are specified.

In summary, avoid the use of OFFSET feature in CBAR, CBEAM, Plate & Shell CQUAD4 elements because one never knows if linear static will be enough, as either a linear EULER buckling (SOL105) or nonlinear static analysis (SOl106) are always required.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc