FEMAP Stress Linearization Tool

Siemens Phenom Siemens Phenom
Siemens Phenom

We have written an add-in for FEMAP v10.3.1B/v11 that performs stress linearization in solid FEMAP models.  Once you install it, there’s an .exe that can be run that as long as FEMAP is running will pop up a FEMAP Add-In pane inside of FEMAP and walk one through picking two nodes to calculate the linearization between. 

 

This is based on 2007 ASME Section VIII, Division 2 – Annex 5.A Linearization of Stress Results for Stress Classification.

 

I would also like to credit the engineers at Pressure Vessel Engineering, they have an excellent web site and some very useful information about Stress Linearization and Pressure Vessel stress analysis –

 

http://www.pveng.com/FEA/FEANotes/NutsBoltsStress/NutsBoltsStress.php

 

Remember –

 

This is a Beta Test unsupported FEMAP utility.

 

This program assumes your solid stresses are in the Global Rectangular system, it does not account for solid elements stresses with any other reference coordinate system.  The transform to a Coordinate System in line with the SCL is hard-coded from Global.

 

Basically, one chooses two nodes in FEMAP and a FEMAP Output Set.  According to the ASME Document (the document), this Stress Classification Line (SCL) should be as perpendicular to the outer surfaces of the pressure vessel to be effective.  .  The program linearly interpolates the six components of 3-D stress at multiple points along this line.  A membrane stress value is calculated at the interpolations points based on the 1/t formula from the document.  A bending stress value is also calculated, according to the document, only the stress in the plane perpendicular to the SCL should be used, these is the “Full Component Bending” option, with it on, all components are used, with it off, it’s only using the in-plane ones.  We’ve seen tools that do this both ways.  The bending stress is calculated with the 6/t^2 formula from the document.  The calculated Membrane and Bending stresses are plotted vs. the SCL.  In addition, some other key values are indicated.  The actual full component stress values are also shown along the SCL from the FEA results.

 

Download and unzip to a temp directory and then run the setup in there.

 

Works with FEMAP v10.3.1 and v11.0.x – you need a solid model with stress results, run the .exe and a pane will displayed in FEMAP.

  

Choose an Output Set, Select Two nodes, and the stress linearization is performed along the line.  Each time you select two new nodes, or change the output set, or any of the options, the graph/results will be updated, and a copy of the results gets sent to the clipboard, so if you paste, you get –

 

FEMAP Stress Linearization Tool

All Data Calculated as von Mises Stresses

Only in-plane (relative to the SCL) stress tensor components used to calculate linearized bending stress.

 

FSLT Graph

 

Stress Linearization between Nodes 6121 and 6123

Data from FEMAP Model - C:\mastemp\StressLinearization\Example\FEMAP.modfem

From FEMAP Output Set 4 - Titled - Step 1, Sub 4, - 1.

The Linearized Membrane Stress is calculated as 243.729

The Linearized Bending Stress is calculated as 1867.64

The Linearized Maximum Combined Membrane and Bending Stress is calculated as 1963.162

The Maximum von Mises Stress along the SCL is 2689.801

 

 FSLT SCL

Comments
Builder
Builder

Dear Mark,

 

I installed Femap 12.0.1 version and I have a problem with SCL tool.

Please could you help me?

SCL.PNGSCL

 

Best regards

Stefano

Builder
Builder

Dear @masherman ,

 

I just install new Femap 2019 and I would like to know if "stress linearization tool" works with Pyramid elements.

 

I perform some test and during  stress component calculation I receive this message:

 

linearization_femap2019_1.PNGSCL

 

Could you please help me?

 

Thanks 

Best regards

Stefan Milani

Siemens Phenom Siemens Phenom
Siemens Phenom

The tool does not support pyramid elements.  Let me take a look at the code and see if it is possible.  I will get back to you shortly.

 

Mark.

Siemens Phenom Siemens Phenom
Siemens Phenom

I checked the code, all is working as it should, the only problem is the error message is bogus.  Stresses are getting transformed for the pyramid elements, the message is extraneous.  We will fix the incorrect generation of this message for FEMAP v2019.1's first maintenance release.

 

Mark.

Builder
Builder

Dear @masherman ,

 

thanks for your reply.

 

I've done many test, and I saw that in some cases "stress" distribution drop to "zero value", as you can see in the following figure.

 

linear.pngStress

 

This happened not only with pyramid elements, but also with other type of elements (linear and parabolid).

Stresses are calculated correctly or there's a problem?

 

Thanks 

Best Regards

S