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 - Femap Forum
- Inconsistencies in calculation of plane stress and...

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

06-11-2015 07:26 AM - edited 06-12-2015 02:19 AM

Hi at all,

I am using plane strain and plane stress elements very often in my calculations. But frequently I don't know, how I have to define the acting forces on such elements. There are two possibities:

- force

- force per unit width

So I made some investigations in FEMAP 11.2, concerning plane stress and plane strain elements and found out, that there are some inconsistencies in calculation results and in model definition procedure (see attachments).

Summary:

Depending on which solver you are using, the definition of acting forces are different (marked yellow)

In some cases the Mises stress or the translation will be calculated wrong.

What does the plane stress option in Femap structual options inside the formulation dialog box do?

Best regards

MaPi

4 REPLIES

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

06-12-2015 06:09 AM

Dear MaPi,

Regarding** 2-D PLANE STRESS** **Solid **elements in NX NASTRAN please note the following:

- The PLANE STRESS elements represent structures that are
**thin**relative to their lateral dimensions and are planar, so nonsense to study thick solids. Then the comparison is not plane stress vs. plane strain, but plane stress vs. solid, or plane strain vs. solid, the result should be different. - The CPLSTS4, CPLSTS8, CPLSTS3, and CPLSTS8 are plane stress elements.
- For both linear static analysis using NX NASTRAN (SOL101) and basic nonlinear (SOL106) they must be defined in the X_Y plane of the basic coordinate system. For Advanced NonLinear (SOL601) they must be defined in the X_Z plane.
- The elements CTRIA3, CTRIA6, CTRIAR, CQUAD4, CQUAD8, and CQUADR can optionally be modeled as plane stress elements, but these elements have a slightly different stiffness formulation than the CPLSTSi elements. As a result, results can be slightly different.
- To make sure you are using genuine
**PLANE STRESS**elements in FEMAP & NX Nastran make sure to select**PLANE STRAIN**under Element/Property Type (yes, I have been requesting for years to FEMAP developers to have both 2-D PLANE STRESS & 2-D PLANE STRAIN to appear explicitly as separated options in the screen, but this is what we have ...)

_

Click in **FORMULATION** and under NASTRAN select **2.. CPLSTS3,CPLSTS4,** etc.. that are the NX NASTRAN 2-D Solid Plane stress elements, OK?.

I will prepare a simply model using FEMAP V11.2 to check that everything runs correctly, and results are reasonable, 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
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-12-2015 07:30 AM

Hi Blas,

thx for your fast reply. Using solver 101 and 106:

The plain strain element in xy-plane calculates a Mises stress like plane stress element, but elongations like plane strain. Look at the Analysis_summary.pdf. That's very mysterious.

Also the fact, that xy-plain strain elements have to be loaded via a force and xz-plain strain element have to be loaded via a force per unit width to get the same result.

Best regards

MaPi

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

06-22-2015 02:28 PM

Dear MaPi,

In the new release of **FEMAP V11.2.1** the error of writting a 2-D solid plane stress **CPLSTS4** element as CQUAD4 element is solved, now if you click in PREVIEW ANALYSIS you will see that the nx nastran input deck is correct:

Also, the output vector computed by NX NASTRAN are plane normal stress results in the X & Y plane, as well as vonMises stress.

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
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-23-2015 07:37 AM

Hi Blas,

thx, I have just installed the latest FEMAP Version. Next time I will repeat my investigations using version 11.2.1 and give feedback again.

Best regards

MaPi

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc