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
- Different maximum nonlinear von Mises stress

Options

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

Different maximum nonlinear von Mises stress

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

12-19-2017 10:10 AM

Hello,

Refer to the attached images. For same geometry, loading and boundary conditions; I get different values of max. nonlinear von Mises stress from nonlinear static and advanced nonlinear static anaylsis. Do you know why this is so?

Regards,

Su

3 REPLIES 3

Re: Different maximum nonlinear von Mises stress

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

12-19-2017 06:03 PM

Dear Su,

Without having the two FEMAP models in hand is difficult to know the details used in material model, analysis options, etc.. Please note the diferences are notable between NX NASTRAN basic nonlinear (SOL106) and advanced nonlinear (SOL601), aka ADINA. For instance, depending the resultant strain level the differences could be important.

**SOL106**: The SOLID nonlinear elements for small strain analysis can handle material or geometric nonlinearities or both. In geometric nonlinear analysis, the elements may undergo large total displacements and rotations**but the net deformation of each element has to remain small**, therefore these elements are called “small strain” elements. For linear material and infinitesimal deformation, a nonlinear analysis with small strain elements gives results which are identical to a linear analysis.**SOL601**: Advanced Nonlinear Solution supports incomplete quadratic 3-D elements for tetrahedral and pyramid elements, and are isoparametric displacement-based elements. In addition to the displacement-based elements, special mixed interpolated elements are also available, in which the displacements and pressure are interpolated separately.**SOL601**: The 10-node tetrahedron is obtained by collapsing nodes and sides of rectangular elements. Spatially isotropic 10-node and 11-node tetrahedra are used in Solution 601. The stresses/strains can be output either at the center and corner grid points (PSOLID STRESS=blank or GRID), or at the center and corner Gauss points (PSOLID STRESS=1 or GAUSS).

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/

Re: Different maximum nonlinear von Mises stress

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

12-20-2017 04:53 PM

Dear Blas,

Thanks for your detailed response on SOL106 vs SOL601!

I have attached the Femap model. Could you please let me know if the difference in maximum stresses is due to some particular analysis settings in this case? The strain values are very close to each other.

Also, can I plot the stresses at Gauss points in Femap v11.2 using GUI?

Best regards,

Su

Re: Different maximum nonlinear von Mises stress

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

12-22-2017 02:37 PM

Dear Su,

I see some improvements are recommended to be performed in your FEMAP model, and also I found some errors as well, here you are:

**HEX MESH**

Here is extremely critical to mesh with HEXAEDRAL elements, specially in nonlinear analysis, forgot tetrahedral elements because TET are less accurate and the model size is in average around 10 times bigger for the same element size: 49437 nodes your TET10 model, 6872 nodes mine HEX8 only, size matter, specially in nonlinear analysis!!. I have recorded a video to explain how to mesh the geometry with solid HEX elements (I hope you love the Country music ...):

[video]

**ERROR IN LOADINGS**

I see you have applied a Moment load in surface, wrong!!, solid elements don't have rotational DOF, then is useless to apply a moment on a surface of a solid meshed with 3-D solid elements.

You need to apply a TORQUE load on surface. The command will ask you a vector defined by two points (base & tip) to apply the torque load. Once applied you can expand the load (use **MODEL > LOAD > EXPAND** command) to see the resulting force loads, this is the way how FEMAP will export the analysis file to the NX NASTRAN solver:

**YOUR MATERIAL MODEL**

__I see you have defined a bi-linear material model with vonMises yield stress = 172 MPa and Work hardening slope H=1949 MPa, that is a slope of stress vs plastic strain.__

My option here in general is clear: with STEEL because most of the times the Plasticity Modulus H in general is not know exactly, I always select **PLASTIC **model with vonMises Yield criterion (in your case yield stress= 172 MPa), which means that after reaching yield the line on the stress-strain chart is horizontal, ie, an elastic-perfectly plastic nonlinear material model.

**YOUR NONLINEAR ANALYSIS PARAMETERS (SOL106)**

I note in the BULK DATA Options that **PARAM=LGDISP,1** is not activated, wrong!!. This means you are performing a ** linear** geometric analysis (small displacements), the only nonlinearity is material. Please be aware of this error, this is critical to activate large displacements effect, then nonlinear geometric analysis will be performed, OK?.

Also, the most crucial data for successful nonlinear static solutions are contained in the **NLPARM** bulk data entry. NLPARM defines strategies for the incremental and iterative solution processes, surprise you have not setup any options!!.

Here you are my settings:

- For number of TimeSteps I set a minimum of
**50**. - For max. iterations per step =
**5**. - for the STIFFNESS UPDATES the
**SEMI**method usually provides better convergence than the AUTO method, at the expense of higher computing cost. - For the solution strategy =
**Full Newton-Raphson**.

And here you are the nodal vonMises stress results of the nonlinear static (SOL106) analysis:

**ADVANCED NONLINEAR (SOL601)**

Again I note in the BULK DATA of your FEMAP model the parameter for LARGE DISPLACEMENTS EFFECT is not activated, then your nonlinear results are useless again. Here you are MY OPTIONS:

If I run the analysis here you are the results:

**RESULTS COMPARISON**

Well, not too much diferences, with SOL106 the material plastify locally (maximum displacement URES=0.0509 mm), with SOL601 the material seems to remain in elastic regime (maximum displacement URES=0.0509 mm), and the maximum resultant displacement is the same.

**OUTPUT AT GAUSS POINTS **

Regarding the question **STRESS/STRAIN OUTPUT at GAUSS POINTS WITH SOLID ELEMENTS**, it was explained here, apparently with low interest by the FEMAP & NX NASTRAN community:

Well, I hope the above explanation to be of help to study more in detail all the parameters of the nonlinear analysis of both Basic Nonlinear (SOL106) and ADVANCED NONLINEAR (SOL601) modules, 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/

Follow Siemens PLM Software

© 2019 Siemens Product Lifecycle Management Software Inc