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
- 3D Simulation - NX Nastran Forum
- Plate problem

Options

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

Solved!
Go to solution

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

01-27-2017 09:45 AM - edited 01-27-2017 09:47 AM

Hi,

I solved a plate problem by Maple (similar to Matlab) program using Classical Plate Theory (CPT) and First Shear Deformable Theory (SDT). I attached the picture.

After I get the results from my Maple codes, I want to compare the results with FE results so I set up FE model in FEMAP and run the analysis with NX Nastran.

The FE results are somewhat close to my Maple results, but they are not identical. For example, for the deflection of a node, Maple gives me 0.68'' whereas the FE result gives 0.715''. The main question that I want to ask is why is there such a different in result assuming my Maple program is good (I double check with my professor). If anyone has compared the FE result with the theoretical results before, I would like to hear from your perspective of why you think there is a difference in my case.

I did some research and know that NX Nastran by default uses CQUAD4 element for plate which is based on Mindline-Reissner theory with transverse flexibility. And this simulation is linear static (SOL 101). I have tried the same problem with different load configurations, but there is always a difference.

I would appreciate if someone can comment on this.

Thank you,

Solved! Go to Solution.

4 REPLIES

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

01-28-2017 05:11 AM

Hello!,

The Finite Element Method is an approximate method, the accuracy of the solution depends of various factors: element type, mesh density, loadings, boundary conditions, analysis type, etc.. Here you are a few suggestions to improve accuracy:

**Results Convergence**: perform a convergence study, double your**mesh density**and rerun the analysis and compare results, you will realize very soon that displacements will converge quickly.**Element Type**: in FEMAP you have a professional FE library, compare results meshing with 2-D Shell CQUAD4 vs. 3-D Solid CHEXA, perform mesh convergence studies as well.**Analysis Type**: Linear Static analysis using NX NASTRAN (SOL101) is ONE solution, but compare results with a Nonlinear Static analysis (SOL106) activating large displacements effect (ie, geometrical nonlinearities), you will know what is good. The membrane stiffness is neglected in linear static analysis for CQUAD4 elements, only running a nonlinear analysis is captured properly. For instance, stress stiffening effect consideration is critical on curved shaped structures, "**stress stiffening**" refers to a coupling between membrane stress and lateral displacements associated with bending, if you run a linear static analysis this is useless, OK?. The bending stiffness of a beam, arc, plate or shell is increased by tensile membrane stress ("stress stiffening") and is decreased by compressive membrane stress ("stress softening", ie, buckling!!).

In summary, using Finite Element Method you can have MANY solutions, all are solutions, yes, the valid one will depending of what you are looking for: stress, displacements, reaction force, buckling load factor, etc.. You can "play" with many factors, and all have a "price" to pay (solution time, model size, model creation time, etc..), enjoy!.

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/

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

01-28-2017 01:06 PM

Thank you blas for your suggestions. I will try some of them out.

Right now, I am gonna use Patran/ Nastran and possibly other softwares to compare the results.

There is another question I want to ask. CQUAD4 element is based on Mindlin-Reissner plate theory with transverse shear flexibility which means that the users can turn on or off the transverse shear. In Femap, the transverse shear can be turned off in plate property. I want to know how does "NX Nastran" get rid of transverse shear for CQUAD4 elements. If the transverse shear is taken out, the Mindlin-Reissner shouldn't be valid anymore. Then what would CQUAD4 element become?

I'm trying to look into NX Nastran theoretical manual without much luck on CQUAD4 derivation. Let me know what you think.

Solution

Solution

Accepted by topic author Cocoki

01-29-2017
08:06 PM

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

01-29-2017 05:24 AM

Hello!,

The **CQUAD4** element of NX NASTRAN is my favorite between CTRIA6, CQUAD8, CQUAD4R, etc.., is an isoparametric quadrilateral element with optional coupling of bending and membrane stiffnesses. The formulation of the CQUAD4 element is based on the Mindlin-Reissner shell theory. The element do not provide direct elastic stiffness for the rotational degrees-of-freedom which are normal to the surface of the element.

Depending on the 2-D element, you define the properties for plate and shell elements with either PSHELL, PCOMP, PCOMPG, or PLPLANE bulk entries. Transverse shear flexibility may be included for all bending elements on an optional basis. Differential stiffness matrices are generated for all shell elements except CQUADR and CTRIAR.

The PSHELL entry allows to define the material ID for the membrane properties, the bending properties, the transverse shear properties, the bending-membrane coupling properties, and the bending and transverse shear parameters. By choosing the appropriate materials and parameters, virtually any plate configuration may be obtained.

The CQUAD4 element can model in-plane, bending, and **transverse shear behavior**. The element’s behavior is controlled by the presence or absence of a material ID number in the appropriate field(s) on the PSHELL entry. **To add transverse shear flexibility to bending, fill in MID2 and MID3**.

Adding **transverse shear flexibility** means that using MID3 adds a shear term in the element’s stiffness formulation. Therefore, a plate element with an MID3 entry will deflect more (if transverse shear is present) than an element without an MID3 entry. For very thin plates, this shear term adds very little to the deflection result. For thicker plates, the contribution of transverse shear to deflection becomes more pronounced, just as it does with short, deep beams.

You should use the CQUAD4 element when the surfaces you are meshing are reasonably flat and the geometry is nearly rectangular. For these conditions, the quadrilateral elements give more accurate results for the same mesh size than any other element type, OK?.

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/

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

01-29-2017 08:07 PM

Thank you for the useful information!

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc