Cancel
Showing results for 
Search instead for 
Did you mean: 

Inconsistencies in calculation of plane stress and plane strain elements

Creator
Creator

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

Re: Inconsistencies in calculation of plane stress and plane strain elements

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

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 ...)

plane_stress1.png_

 

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

 

plane_stress2.png

 

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/

Re: Inconsistencies in calculation of plane stress and plane strain elements

Creator
Creator

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

Re: Inconsistencies in calculation of plane stress and plane strain elements

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

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:

 

plane_stress-analysis-preview.png

 

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

 

plane_stress_results.png

 

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/

Re: Inconsistencies in calculation of plane stress and plane strain elements

Creator
Creator

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