Edit Result dialog box

The Edit Result dialog box also appears as the Result tab within the Post View dialog box.

Result Selection
Mode/Iteration list	Appears when there are multiple load cases, modes, iterations, or time steps.Specifies the load case (linear statics solutions), mode (modal solutions), iteration (optimization solution processes), or time step (nonlinear solutions).
Result Type
Results list	Specifies the result type to display. Available results depend on the analysis type and the specified output requests.
Component list	Specifies the result component to display. Available components depend on the result type.
Complex Options
Complex	Determines the value displayed at nodes for results in complex format:RealDisplays the real part of the complex result at nodes. ImaginaryDisplays the imaginary part of the complex result at nodes.AmplitudeDisplays the absolute amplitude of the complex result at nodes.Signed AmplitudeDisplays the signed amplitude of the complex result at nodes.At Phase AngleDisplays the value at nodes of the complex result at a specified phase angle. Enter a phase angle in degrees in the text box.
Shell and Beam Locations
Beam	Available for Stress – Element-Nodal and Strain – Element-Nodal results.Available when the model contains 1D beam or bar elements.Specifies the beam stress recovery point. Stress recovery points for standard cross sections are displayed in the Beam Section dialog box. Stress recovery points for user-defined beam sections are assigned when you define the beam section. Select a recovery point from the Beam list. Or choose the Minimum or Maximum value for all stress recovery points. If you calculate beam stresses from element forces, Minimum and Maximum return the minimum and maximum stresses for the complete section, regardless of recovery points.
Shell	Available for Stress – Element-Nodal and Strain – Element-Nodal results.Available when the model contains 2D shell elements.Specifies the shell layer. See Shell locations.
Beam Results
Calculate Beam Results from Forces and Beam Geometry	Available for Stress – Element-Nodal and Strain – Element-Nodal results.Available when the model contains 1D beam or bar elements.Calculates beam stresses and strains from element forces and beam geometry.Note: When you select this option, the software queries the results file for material properties and section definitions. If that information is not available in the results file, the software queries the CAE model for that information. If the Simulation file is not loaded (for example, for imported results) you may not be able to generate beam results for nonstandard sections.For more information, see Beam stresses.
Add Fillets	Available when the Calculate Beam Results from Forces and Beam Geometry check box is selected.Modifies beam section geometry to add fillets to interior corners. The fillet radius is determined by multiplying the Fillet Radius Scale Factor by the beam section wall thickness; the scale factor must be a value between 0 and 1.
Fillet Radius Scale Factor	Available when the Add Fillets check box is selected.Type the scale factor for determining the fillets.
Symmetric Result Options
Set Symmetric Results	Appears when symmetric results are available. Opens a display options dialog box to let you set the display of symmetric results.
Displacement Offset
Offset by a Reference Node	Available for displacement results.Offsets the displacement value with respect to a reference node location.
Method	Appears when the Offset by a Reference Node check box is selected.Lets you specify the method for selecting a reference node.Pick from Model Lets you select a node in the graphics window.By Node IDLets you select a node by typing its ID.
Node Label	Appears when Selection Mode is set to By Node ID. Type a node ID in the box and click to select it.
Select Node	Appears when Selection Mode is set to Pick from Model. Lets you select the reference node in the graphics window.
Mark IDs	Appears when the Offset by a Reference Node check box is selected.Displays the ID of each selected element or node in the graphics window.
Clear Highlights	Appears when the Offset by a Reference Node check box is selected.Removes all the identifying labels or IDs from the display of the model. Clear Highlights does not clear the selection of elements or nodes.Note: The identifying labels or IDs return if you select more entities and the Mark IDs check box is selected.
Clear Selection	Appears when the Offset by a Reference Node check box is selected.Clears the selection of all elements or nodes and clears the Selectionbox.
Plies
Location	Appear when you post process a ply result.Lets you specify the location in ply.Middle Lets you select the middle of the ply.TopLets you select the top of the ply.BottomLets you select the bottom of the ply.Note: Only the locations that are available for the selected result will be shown.
Result Combination
Combine At	Specifies the type of results on which to perform combination calculations or to not perform combination calculations.NoneResults are not averaged or summed.NodesAvailable for results displayed on nodes.Use nodes to perform combination calculations.ElementsAvailable for results displayed on elements.Use elements to perform combination calculations.
Nodal Combination	Appears when Combine At is set to Nodes. Available for results that are displayed on nodes.AverageCalculates a nodal average across all adjacent elements for elemental and element-nodal results. Use this feature for a smoother display of stress and/or strain results, for example.MaximumFor each node, takes the maximum value of all the contributions of the adjacent elements that share the node. Absolute MinimumFor each node, takes the absolute minimum value of all the contributions of the adjacent elements that share the node. Absolute MaximumFor each node, takes the absolute maximum value of all the contributions of the adjacent elements that share the node. Arithmetic MeanFor each node, compute the arithmetic mean of all the nodal values of the elements that share the node.DiscontinuityNot available for invariant quantities (derived results, such as Von-Mises).Compute several types of discontinuities. See below.MinimumFor each node, takes the minimum value of all the contributions of the adjacent elements that share the node. SumThis option is available for Grid Point Force — Element-Nodal and Grid Point Moment — Element-Nodal results, and if the structural output request for your solution specifies Grid Point Force.At the nodes of the elements in consideration, this option sums the force data (for grid point force results) or moment data (for grid point moment results). Signed Absolute MinimumFor each node, takes the signed absolute minimum value of all the contributions of the adjacent elements that share the node. Signed Absolute MaximumFor each node, takes the signed absolute maximum value of all the contributions of the adjacent elements that share the node. For more details about these options, see Nodal combination options for element-nodal results.
Discontinuity	The following options appear only when Nodal Combination is set to Discontinuity.Relative DiscontinuityCompute the relative discontinuity at nodes (percentage).Weighted DiscontinuityCompute a weighted discontinuity at nodes (percentage).Local DiscontinuityCompute the difference between the maximum and the minimum values.Locally Balanced DiscontinuityCompute a locally balanced discontinuity (percentage).For more details about these discontinuities, see Nodal combination options for element-nodal results.
Average Across	Appears when Nodal Combination is set to Average.Controls how elemental or grid point results are averaged at nodes.MIDsWhen the MIDs check box is cleared, averaging does not occur across elements that reference different material property IDs.PIDsWhen the PIDs check box is cleared, averaging does not occur across elements that reference different property IDs.Element TypeWhen the Element Type check box is cleared, averaging does not occur across elements of different types like shell elements vs. solid elements.Feature AngleWhen the Feature Angle check box is cleared, averaging does not occur across elements on different sides of a feature edge when the feature angle exceeds the value you enter in the Feature Angle box.For more information about these options, including how averaging occurs when you use more than one of these options, see Averaging options for elemental and grid point results.
Include Visible Elements Only	Appears when Combine At is set to Nodes.Lets you restrict the summation to the nodes in the elements displayed in the post view. You can limit the post view display to a group of elements by using the Show Only command on the group or by turning off individual meshes in the Post Processing Navigator.
Include Internal Elements	Available when Nodal Combination is set to Average and the Feature Angles check box is selected.When the Include Internal Elements check box is cleared, averaging does not use results for elements that do not have free faces.
Include Midnodes	When your mesh includes parabolic elements, displays results at the midside nodes.
Element Criterion	Appears when Combine At is set to Elements. Available for results displayed on elements.Specifies the criterion used for determining the element results display:AverageDisplays the average of all values for each element.CentroidDisplays the result at the element centroid.MaximumDisplays the maximum value for each element.MinimumDisplays the minimum value for each element.Absolute MinimumFor each element, takes the absolute minimum value of all the contributions of the adjacent elements that share the elements. Absolute MaximumFor each element, takes the absolute maximum value of all the contributions of the adjacent elements that share the element. Signed Absolute MinimumFor each element, takes the signed absolute minimum value of all the contributions of the adjacent elements that share the node. Signed Absolute MaximumFor each element, takes the signed absolute maximum value of all the contributions of the adjacent elements that share the node.
Coordinate System
Coordinate System	Specifies the coordinate system used to transform the magnitude and direction of vector and tensor data components.For more information, see Coordinate systems in post-processing.
Axis of Rotation	Available for cylindrical coordinate systems.Specifies the axis of rotation for the coordinate system.
Display Beam Results in Local Coordinate Systems	Available for Stress – Element-Nodal and Strain – Element-Nodal results.Available when the model contains 1D beam or bar elements.Displays beam results in the local (element) coordinate system, while displaying shell and solid results in the specified coordinate system.
Shell Results in Projected Coordinate System	Available for Stress - Elemental and Stress – Element-Nodal results.Available when the model contains 2D shell elements.Available for the following coordinate systems:Absolute RectangularAbsolute CylindricalAbsolute SphericalWork RectangularWork CylindricalWork SphericalSelected RectangularSelected CylindricalSelected SphericalWhen you select the check box, the software projects the selected coordinate system onto the plane of each element and creates a consistent coordinate basis across all elements in the mesh.This allows you to display the X and Y components of stress along a uniform orientation throughout the mesh.Note: Before selecting the check box, use the 2D Element Normals command to ensure element normals are oriented consistently across the mesh.
Display Result on Face Normal	Available for frequency nodal results.Available when the result quantity is a vector. Projects the selected vector result component (X, Y, Z, or Magnitude) along the local normal of each node. The software calculates the local normal of a node from its shared element face normal.
Units	Specifies the units to display results in.
Scale	Specifies a scale factor. Results values are multiplied by the scale you enter here. The default is 1.0.
Absolute Value	Converts positive and negative results to absolute values.
	Available for Stress – Element-Nodal and Strain – Element-Nodal results.Appears when the Absolute Value check box is selected.Specifies the absolute value calculation method.Derived Component(Default method) The software first calculates the derived quantity using the unaltered values of the tensor components, and then takes the absolute value of the derived result, such that reported results are all algebraically positive. This option is available for these result quantities: Determinant, Mean, Max Shear, Min, Mid, and Max Principal, and Octahedral.Tensor ComponentsThe software calculates the derived results using the absolute values of the tensor components. The method is available for legacy purposes.
Apply dB Scaling	Scales the displayed results based on the decibel scale that you select. Available for Acoustic Pressure, Acoustic Intensity, and Acoustic Power results.
dB Scale	Appears when the Apply dB Scaling check box is selected.Specifies the decibel scale for scaling your output.dB10Scales the output using 10 Log(acoustic_quantity/dB_reference)dB20Scales the output using 20 Log(acoustic_quantity/dB_reference)where:acoustic_quantity is the quantity you are measuring, such as pressure, intensity, or powerdB_reference is the reference value you enter in the dB Reference (N/mm^2(MPa)) box.Decibel scales are used for different applications. For example, you might use dB10 for plotting intensity levels of speech, and you might use dB20 for plotting sound pressure levels of machinery.
dB Reference (N/mm^2(MPa))	Appears when the Apply dB Scaling check box is selected.Sets the reference value for the result type you select in the results list. Change the reference value depending on the acoustic medium you are computing for. For example, you would use different dB reference values for air and water.The default reference values are in SI units based on the output quantity you select in the results lists.The software calculates the results using the dB reference value and updates the displayed plot.
Acoustics coupling list	Appears when the results are for vibro-acoustic solutions.Specifies the display of fluid elements and structural faces based on coupling and distance.Fluid coupled faces : closest distance to structural faces - Element-FaceDisplays the free fluid faces that are coupled to the structural faces within the distance specified in the Fluid-Structure Interface Modeling Parameters modeling object. The distance between faces is displayed in the legend.Fluid uncoupled faces : search distance - Element-FaceDisplays the fluid faces that are outside of the search distance and that are uncoupled. The search distance is specified in the Fluid-Structure Interface Modeling Parameters modeling object.Fluid coupled and uncoupled faces: distance - Element-FaceDisplays the fluid faces that are uncoupled as transparent, and the fluid faces that are coupled as blue.Structural coupled (0) and uncoupled (1) faces - Element-FaceDisplays the structural faces that are uncoupled as transparent, and the structural faces that are coupled as blue.
Result type list	Scalar is the only option.
Acoustic Post Environment Settings
Appears when the post-processing environment is set to Acoustics. For more information, see Post-processing environments.
Spectrum Scaling	Sets the scaling for the spectrum.
Weighting	Sets the acoustical weighting scheme to use to represent the data. The acoustical weighting scheme scales the data for noise perception and measurement.

How do I

Create a post view

Learn more

Beam post-processing

Coordinate systems in post-processing

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Edit Result dialog box, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });