Where are the Recovery Points in a Solid element?

[AdamFetsch]

Where are the recovery/integration/gauss points in FEMAP solid elements?

For example, a 10 node tetrahedral element. Is there only one gauss point in the middle of the element?

Can anyone point me to some answers?

 

[BlasMolero]

Hello!,
Take a look to the following post:

http://community.plm.automation.sie...in-output-at-GAUSS-points-with/m-p/5783#U5783

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
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/