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
- Re: Stress Post-Processing Data results for a soli...

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

09-12-2016 10:53 AM

Hello everyone,

I'am amateur for femap. I have a problem with the Stress presentation of Post-Processing Data for a solid that meshes different zones. This solid was imported from file .stp (that I designed Catia V5) into Femap Nastran for analysis Finite Elements. I divided differrent zones for mesh differrent size on solid (as joint photo).

The nonlinear analysis (Nonlinear Static) present correctly the zone of the Von Mises stress. But when I present other stress direction, it is likely not correct to present stress in the zone divided (as joint photo).

Anyone can give me some idea to prove this problem ?

Thank you for you answer.

Solved! Go to Solution.

6 REPLIES

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

09-12-2016 02:39 PM

NASTRAN reports linear stresses in the Global Coordinate System. Nonlinear stresses are reported in the Elemental Coordinate System. Therefore Y-Stress will look great for linear, but look strange for nonlinear. In FEMAP, you can transform the Elemental Nonlinear Stresses to Global in the Meshing Toolbox on the Post-Processing Tab -

PIck the Nonlinear Stress component you would like to visualize, and then set the "Solid Stress/Strain" transform to the Global Coordinate System (0 in FEMAP).

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

09-13-2016 03:23 AM

Hello, masherman

Thank you for you reply. I follow your steps but the result is unchange (as the joint photo).

Highlighted

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

09-13-2016 10:42 AM

When you mention the stresses are not as expected, what orientation are you expecting? It would be common to be interested in radial and hoop stress around a hole. If you want to see the direct stresses in that orientation, then you must create a cylindrical coordinate system at the center of the hole. Then use the transform dropdown under Solid Stress/Strain to this system, not X is radial and Y is tangential. This transformation will work for the linear stress output without any other action.

Now for nonlinear, an extra setting is required to make the transformation work correctly. As Mark stated, for nonlinear, the solid element stress output is oriented/reported in the element system. So we need to change the orientation setting in Femap to match this. This is the little icon with an arrow through it, to the right of "transform" and it will bring the following form where you should update the solid element to "element"

Many users prefer to stick to results like von mises and principal stresses to avoid this issue.

Hope this helps.

Joe

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

09-13-2016 11:07 AM

Hello Joe,

Thank you very much for your advice. I follow your step and the problem has been solved.

To answer your question,

I would like to observe the stress along Y-direction in the root of notch, and calculate stress gradient.

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

09-15-2016 03:53 PM

>>NASTRAN reports linear stresses in the Global Coordinate System. Nonlinear stresses are reported in the Elemental Coordinate System.

Mark, thanks for this valuable insight. Is the above mentioned in any of the Femap or NX Nastran documentation? Will be helpful to have it bookmarked for future purposes.

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

09-16-2016 09:28 AM

In the latest Nastran documentation(Help/NXNastran/basic nonlinear guide;section 2 page 12), you can find the following section:

Output

For this output discussion, an element is a nonlinear element if it supports geometric nonlinear and

PARAM,LGDISP,1 is defined, and/or material nonlinear (plasticity, creep or hyperelastic) is defined

on this element.

Element stress and strain output is requested with the STRESS case control command. The stress

and strain output for nonlinear elements is written into both a nonlinear and a linear format. The

nonlinear format outputs stresses together with strains. Compared to the linear format, the nonlinear

format provides more information with regard to nonlinear material laws (effective strain, equivalent

stress etc.). The stresses and strains of the small strain elements refer to the undeformed area

and length, respectively. **The components of the stresses and strains are in the deformed element****coordinate system which co-rotates with the elements' rigid body deformation.**

Averaged grid point stresses are requested with the GPSTRESS case control command. Averaged

grid point stresses for nonlinear elements is available in nonlinear static analysis but not in nonlinear

transient analysis.

Element forces are requested with the FORCE case control command except for the CBUSH and

CBUSH1D elements. The STRESS and NLSTRESS case control commands should be used to

request the element force and stress output for the CBUSH and CBUSH1D elements. Element forces

per unit length refer to the undeformed length. The components of the element forces are in the

deformed element system. For nonlinear elements, element forces are available in nonlinear static

analysis but not in nonlinear transient analysis. Element forces are not available for solid elements.

Deformations are requested with the DISPLACEMENT case control command. The output of

displacements and rotations is available in nonlinear static and transient analysis.

Grid point forces are not available in nonlinear static or transient analysis.

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc