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
- Nodal Stress/Elemental Stress and the Derivation T...

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

09-23-2013 11:01 AM

Gentlemen

My boss and I had a little discussion the other day about the origin of Nodal Stresses in Femap, in particular, using plate elements. It is my understanding that nodal stresses are obtained by extapolation of Gaussian stresses. I can visualize a process where by the Gaussian element, internal to the element in question and essentially of the same shape, though scaled down, would see its nodal stresses linearly extrapolated and posited to the complementary plate element nodes.

I have also read that elemental stresses could be computed by inclusion of the plate element centroidal node in the element shape function, in effect, treating the element centroidal node as a Gaussian point.

But the greater question is, which came first, the Chicken or the Egg, the nodal stresses or the elemental stress and ultimately the source of both was, I assume the Gaussian stress?

Are the Femap corner results derived from the centroidal elemental stresses or are they the extrapolated values of the Gaussian stresses?

I'm sure my questioning reveals my naivete.

3 REPLIES

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

09-24-2013 12:20 PM

Dear Brab,

To understand how FEMAP runs is critical to understand what happens with the solver NX NASTRAN, because FEMAP only plot the results coming from the solver. For **CQUAD4, CTRIAR, and CQUADR **plate elements, element forces, stresses, and strains are only calculated by NX NASTRAN at the centroid. You have the option to compute and output these quantities at the corner grid points setting the "*Element Corner Results*" customization at the NASTRAN Output Request in FEMAP. Then, to obtain the corner stresses in addition to the centroidal stress, you should request:

For the **CTRIA3** element the corner option is ignored for this element. And for the **CQUAD8**, **CTRIA6**, **CQUADR**, and **CTRIAR** elements, element forces, stresses, and strains are always calculated at both the centroid and at the corner locations. The center only option is ignored for these elements.

**STRESS/STRAIN Recovery Methods**

NX NASTRAN has the following Strain/Stress methods to recover results at corner points:

• SGAGE,

• CUBIC,

• CORNER and

• BILINEAR.

All the methods start by recovering strain at the element center and **gauss** points using the elemental strain matrix and the computed grid point displacements. From there, the various options control how these strains are extrapolated to corner locations for output. It is noted that stress results can be computed from strain using standard stress-strain relations. Thus the STRESS output control has the same recovery options as STRAIN. The explanation here describes the recovery for strain, but the analogy to stress is clear.

Except for the CENTER option which only returns strain at the center, all the other options return strain at the element center and corners. The strain at the center location is computed the same for all the options. The strain at corner locations is computed differently for the various corner options. BILINEAR uses a linear extrapolation method and is the more stable in most cases and is thus the default. The other corner options use higher order extrapolations in an attempt to be more accurate.

**• BILINEAR** – This is the default corner option and its usage is interchangeable with the CORNER option. This option uses the element linear interpolation functions to extrapolate the strain at the gauss points to the strain at the nodes. In the example of a linear varying moment in a cantilever modeled with CQUAD4 shell elements the strain variation across each element is constant. Across the length of the model, from the fixed point to the load application point, the strain will vary as a step function from element to element. This is because the CQUAD4 element has almost constant strain curvature, giving constant curvature at the gauss points, and when linear interpolated linearly yields constant strain over an element.

The discontinuity of strain from element to element can be minimized by refining the mesh. Nodal averaging of stress results, the default method in FEMAP postprocessor, will also smooth out the results.

**• CUBIC** – Is a corner option intended to smooth out the discontinuity of strain results between adjacent elements. Like the BILINEAR method it extrapolates strain to the corners using the element interpolation functions. Then it uses grid displacements and rotations to curve-fit a cubic equation that is used to adjust the linear corner strains. In the example of a linear varying moment in the cantilevered shell model, the grid point rotations will vary across the element so the curve fit gives the correct linear variation of strain curvature across the element, which translates to a linear varying stress. There is still some discontinuity of strain from element to element, but it is less than with the CORNER method.

Again, mesh refinement and nodal averaging can be used to minimize strain discontinuity.

**• SGAGE** – This method is similar to the CUBIC. But in-plane strains and curvatures are calculated independently for the cubic equation. First strains are calculated in the u and v and diagonal u-v directions at each grid point. The state of in-plane strain at the grid point is calculated using rosette strain gauge equations. Grid strain curvatures are done similarly. In the example of a linear varying moment in the cantilevered shell model, a non-constant strain variation is obtained across each element, however the accuracy is not as good as the CUBIC method. The SGAGE method is not recommended for most cases.

Later in FEMAP during postprocessing you can control how FEMAP converts the results from pure data at element centroids, corners, and nodes to the actual continuous graphical representation. There are three options to convert the data: Average, Max Value, and Min Value.

If Average is on, FEMAP will take an average of the surrounding values to obtain a result, whereas Max or Min Value will just use the max or min value, respectively, of the pertinent surrounding locations. The Min Value option should only be used when performing contours for vectors where the minimum values are actually the worst case, such as safety factor or large compressive stresses.

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

10-01-2013 09:18 AM

Thanks for your reply.

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

10-01-2013 11:26 AM

Dear Blas

I did some more investigating prior to your reply and learned this, which I believe to be correct:

Here are the explanations of stress results most important for linear static load cases with respect to common plate elements including those with mid-side nodes, (quadratic). I am not sure that the descriptions below apply to methods employing shape functions of higher order such as CUBIC and SGAGE options but I suspect they do.

Case 1) Elemental Stress w/Average Centroid Only: This case produces elemental stresses which are the average of the Gaussian point values extrapolated to the element centroid, (they may or may not be extrapolated to the centroid; not sure about that).

The nodal stresses are the averages of the element centroid stresses; an average of an average. The common node of four rectangular elements will have the same value.

Case 2) Elemental Stress w/Averaging: As before, this case produces elemental stresses which are the average of the Gaussian point values extrapolated to the element centroid, (again they may or may not be extrapolated to the centroid), so the elemental stresses do not vary for these two cases.

The nodal stresses which are produced are the average of the Gaussian point values extrapolated to the nodes. The common node of four rectangular elements will have the same value.

But the common node of the same four elements for Cases 1 and 2 will vary by some amount because Case 1 nodal results are the average of the element centroidal stress and Case 2 nodal results are the average of the extrapolated Gaussian stresses.

Case 3) Element Stress w/No Element Averaging: This is the case whose contour appears choppy. There is no smoothing. The elemental stresses are obtained in the same way and are the same as the first two cases. The nodal stresses reflect the true corner values which are the Gaussian point values extrapolated back to the nodes without averaging. There will be no common nodal values. This case can be valuable for assessing convergence.

Nodal stresses will always be smoothed/averaged and the common nodes of adjacent elements will share nodal values. The cases with Average Centroid Only and with Averaging, reflect the same nodal values as Case one and Case two above, respectively.

Please advise if I am in error.

Best regards

brab

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc