*Tip: Start typing in the input box for immediate search results.Can't find what you're looking for? Submit a support request here.*

# Extract Points Overview

## Extracting Points Values in StressCheck

StressCheck provides a convenient means for the computation of data at user-selected points/nodes/locations, along user-specified lines/paths, along element edges, within element faces, or across arbitrary boundary segments intersecting the finite element mesh. The data of interest may be a standard engineering function, a formula name, or a calculator expression. Additionally, the computation of fracture mechanics parameters and the integral average of stresses, strains or displacements over element edges, element faces and curve boundary segments is supported.

To perform pointwise data extractions for a solved StressCheck model, select the Points tab in the Results dialog and specify the desired Points extraction options (Figure 1).

After specifying the Points extraction options, click on Accept to perform the extraction. After the extraction is completed, a graph will appear displaying the points extraction results.

### Specifying the Solution ID(s) and Run(s)

To extract points values for a solved StressCheck model, select the Points tab in the Results dialog, set the Object and Method combo-boxes of the C/A/O/M to the desired configuration (discussed in the following), click on the Solution ID in the scrolling listbox and enter the range of Run numbers for which you wish to compute point-wise values. For example, you may enter Run: 8 to 8 if only Run number 8 is of interest. If assessing the quality of stress, strain or displacement gradients, it is a good practice to enter more than one Run number and StressCheck will automatically overlay the gradients in a single graph.

For more information on the importance of checking solution quality, refer to What Are the Key Quality Checks for FEA Solution Verification?.

#### Multi-Solution Extractions

It is possible to compute point-wise values for different Solution ID’s. This is useful if you want to compare linear with nonlinear, or solutions having different boundary conditions. To activate multiple solution computation, select the multi-solution button near the upper left corner of the Results interface . The solution selection controls will change so that you may choose up to four different Solution ID’s and corresponding Run numbers (Figure 2):

#### Solution Run Wildcards

Entering a max Run number of “0” will automatically extract using the solution with the maximum DOF.

### Specifying the Points Object

Decide whether the extraction is for one or more boundaries (set the Object combo-box of the C/A/O/M to to “Any Boundary”, the default), for one or more elements (set the Object combo-box of the C/A/O/M to “Any Element”), for one or more element faces (set the Object combo-box of the C/A/O/M to “Face” or “Face Surface”), for one or more element edges (set the Object combo-box of the C/A/O/M to “Edge” or “Edge Curve”), for one or more locations (set the Object combo-box of the C/A/O/M to “Location”), for one or more nodes (set the Object combo-box of the C/A/O/M to “Node”), for one or more points (set the Object combo-box of the C/A/O/M to “Point”), for an object set (set the Object combo-box of the C/A/O/M to “Sets”), or for one or more systems (set the Object combo-box of the C/A/O/M to “System”).

Note: the option “Any Boundary” is applicable if at least part of an element exists in the same space as the selected boundary. It is not required that the selected boundary be associated with the element, however.

#### Selecting Objects/Locations for Extracting Points Values

If the Object combo-box is not set to “Sets”, then in the Model View simply left-click on the objects/at the locations on which the function will be extracted.

- If the extraction is on a group of elements, for example, then left-lick and drag the cursor to enclose the desired group of elements in a marquee selection. The selected elements will be highlighted and ready for extraction. Note: it is important to disable the Wetted Faces toggle if internal elements are to be included in the marquee selection.
- If you wish to add one or more elements to the selected group, hold the Shift key down and left-click on the elements to be added to the group.
- If you wish to remove one or more elements from the selected group, hold the Ctrl key down and left-click on the elements to be removed from the group.
- If you wish to cancel the current selection of objects, simply right-click on the Model View.

For example, to extract a stress gradient of 1st principal stress (S1) at an arbitrary number of locations along a curve or group of curves, change the Object combo-box to “Any Boundary” and select the curve(s):

For an example of a stress gradient extraction across an offset surface, refer to StressCheck Tutorial: Offset Surface Gradients via Point Extraction.

### Specifying the Points Method

Select the method of points extraction from the Method combo-box of the C/A/O/M. The options are:

#### Selection Method

The Selection method is used to evaluate data at or along a pre-defined object such as a boundary, point, node, edge, location, system, or set. If the object selected is a boundary, then you may specify an offset range to limit the region of extraction (described in more detail below). As described above, identify the particular object(s) by clicking on the object(s) or by dragging the cursor until a desired group is completely enclosed in a rectangular box. If the group includes objects which were not to be selected then individual objects can be removed from the group by holding the Ctrl key down while clicking on them. The extraction will not be performed until the user clicks the Accept button.

#### Path Method

The Path method is used for computing data along any arbitrary path on the mesh. The type of path will depend on the object selected:

- To compute data along an arbitrary path that is specified directly on the screen, select Object: Location, left-click on the starting location, release the mouse button, and move the cursor to define the end location. When the end location is reached, then double-click. StressCheck will compute the data at the end-points and at evenly spaced intermediate points, the number of which is specified in the dialog box (next to “# of pts.”). The results will include the coordinates of the points, the data values and the minimal and maximal values within the set.
- If the Object: Node, Point, Any Boundary, System, or Edge is selected, the Method: Path will cause the first click on the screen to snap to the closest node, point, boundary, system, or edge to the mouse pick. Then, drag the mouse and the second click will snap to the nearest object to the mouse pick thus creating a line connecting the two objects. If you double-click on the second location, then StressCheck will compute the data along the line. If you click for a third time at a different location, a new line is created between the second and third object. You can create any arbitrary path until you double-click on the last pick. Along each line segment the requested function(s) will be computed in the number of specified points.
- To use the option Object: Sets, give the name of a previously defined set. A set can be defined by selecting the Sets tab in the Points tab. One or more functions can be selected from the Function(s) box. To select more than one function hold the Ctrl key while you click on the function name. Note that the Path method may not require the user click the Accept button.

For an example of extracting a stress gradient between two point locations, refer to StressCheck Demo: Extracting Stress Gradients Between Points.

### Specifying the Display Format

You may input the precision with which you wish to display data values (“Format:” field, in C standard format), as well as enter a distance if you wish to perform extraction on any plane parallel to the XY-plane (“Z-plane:” field). The default format is in scientific notation and any C language format specification can be used. For example, the number Pi (3.141592654…) will be displayed as: 3.141592654e+00 in format %16.9e or 3.14 in format %5.2f.

### Specifying the Auxiliary/Independent Variable

Use the auxiliary variable input field (“Aux. Variable”) if you want to include a variable parameter in the

results. Switch the “Aux. Variable” toggle to “Indep. Var.” and enter a parameter name if you want the auxiliary variable to be the independent variable of the graph.

For example, if graphing the results of a Design Study analysis where one or more parameters is varied across a range of values.

### Specifying the Function(s)

Select one or more standard engineering functions (e.g. Sx, Ey), or the formula (“Fmla”) or calculator (“Calc”) options, from the Func(s): list (Figure 3). To select more than one function name, or to cancel the selection of a function name, hold Ctrl while left clicking on the function name.

#### Fracture Mechanics Parameter Functions

The post-processing of StressCheck allows the extraction of SIFs via CIM (K1 and K2) or separated energy release rates via J-Integral (J1p, J2p and J3p) along the element edges/geometric curves of the crack front at any number of points along each edge/curve.

To compute fracture mechanics parameters at several points along the crack front:

- Select the geometric boundary or element edge(s) where the extraction of the SIF is required (the option Edge Curve can be used to select all edges that are slope continuous).
- Select K1, K2, J1p, J2p, and/or J3p from the function list.
- Enter the number of points along the geometric boundary or selected element edge(s).
- If a geometric boundary is selected, it is understood to be the total number of points.
- If one or more element edges are selected, it is understood to be the number of points/edge.

- Select the coordinate system for the computation of the angle at the extraction point (Figure 4) and enter the value of the radius of the integration path (see Radius of Integration below).

For pre-StressCheck v12.0 releases, the rule for the computation of the Angle at the extraction point (P) is based on the associativity of the edge to the underlying geometry as follows:

- If the selected edge lies on an ellipse, then the parametric angle of the ellipse (φ) is computed in the local system of the ellipse, regardless of the system selected.
- If the selected edge lies on a circle, then the polar angle (θ) is computed in the local system of the circle, regardless of the system selected.
- If the selected edge lies on any other type of curve or surface, or it is straight, then a polar angle (θ) is computed relative to the system selected in the interface.

For StressCheck v12.0 and future releases, the Angle column will always return the polar angle (theta), measured from the X-axis of the system selected in the interface.

The below shows the extraction of K1 along a crack front curve for an automatic integration radius (AUTO):

### Specifying the # of Point Extractions

Specify the number of uniformly spaced points to be extracted, not including the endpoints (“# of pts.:” field). By default, this field is set to “3”, meaning if a curve is selected there will be five (5) total point extractions along the curve boundary, including its endpoints. Note: the “# of pts.:” field is applicable for elements, element edges, element faces and boundaries.

### Specifying the Points Extraction Options

Several buttons/toggles exist to set additional preferences during the the points extraction.

#### Et/Em

The Et/Em switch can be toggled when extracting min/max strains to indicate whether total (Et, default) or mechanical (Em) strains should be computed.

#### Display Points

Turn on the Display Points button if you want to see the sample points being displayed on the Model View as they are being evaluated. This option is useful to visualize the density and location of the points along the selected object.

#### Labels

With the Display Points button toggled on, the user has the option to also display the point number associated with each extraction point by toggling on the “Labels” button. This allows the user to easily match the number in “N” value, or point number, on the model to the “N” column in the graph pane.

#### Average

A capability is available to compute the average of functions along element edges, element faces, element volumes and arbitrary curves. The average is understood in the integral sense, and when appropriate, the user controls the number of points used for the numerical integration.

- If the average is computed along an element edge, face or volume, then the integration is performed using Gauss quadrature, and the number of integration points
**is selected internally by the program**. - If the average is performed along an arbitrary path which runs inside one or more elements, then the integration is performed using the trapezoidal rule and
**the user controls the number of integration points**.

The quantities for which the average can be computed include the displacement components, all directional strain and stress components, and principal strains and stresses. Additionally, the average can be computed for quantities extracted in a local coordinate system and any other function that can be described using the formula option in StressCheck. The length, area or volume of the selected object is also reported with the corresponding average quantity:

- If the selected object is an element, then a volume integral is performed.
- If the selected object is an element face, the integral is performed over the area of the face.
- If a curved boundary is selected, the number of points used for the trapezoidal rule of integration is entered in the # of points field.

Note: the use of the Average option in the Points extraction is **not supported for the Calculator or for surface objects**.

The following animation shows the “Display Points”, “Labels” and “Average” options enabled for a group of selected element faces in which the goal is to compute convergence for the average von Mises strain in a bore surface:

For more information on computing the average of a function, refer to How Do I Compute the Average Stress Over An Object?.

### Specifying the Boundary/System Offset Ranges

If the Object selected is a boundary (“Any Boundary”), then you may specify an offset range (Min/Max) for P1, P2 and/or P3 (Figure 5). The default Min/Max range is 0 to 1. For example, if the selected boundary is a line, then offset 0 means the starting point of the line, offset 1 means the endpoint. An offset range of 0 to 0.5 is understood to mean that the specified function(s) will be evaluated in the starting point, the midpoint of the line plus the number of points specified in the dialog box (# of pts.) in between.

- In the case of circles and ellipses the offset range is measured in the range 0 to 1 as well. The second parameter range (“P2-Min”, “P2-Max”) is ignored for other than 3D objects.
- If the selected boundary is a surface, the initial and final range of each parameter will define an extraction grid in the parameter space of the surface. The third parameter range (“P3-Min”, “P3-Max”) only applies to object “System”.
- When “System” is selected the three parameter ranges (“P1-Min:”, “P1-Max:”, “P2-Min”, “P2-Max”, “P3-Min”, “P3-Max”) apply to the x, y and z-directions extraction ranges relative to the global, or a specified local, system. Each point in the grid will be mapped into the corresponding element in the model, the engineering results will be computed, and the results will be reported.

The following animation shows the von Mises stress Seq) distribution when the offset ranges (P1, P2) are set to [0,0.5] for the selected surface:

Note: Points which lie outside the model domain will be ignored; a warning may occur if this is the case.

### Specifying a X, Y, Z Location

If the Object is set to “Location”, the user may enter (or screen pick) the X, Y, Z coordinates relative to the selected coordinate system (Figure 6). If the location is within the model domain, the extraction will then be performed at this spatial location.

### Specifying a Local System

Optionally, select a local system as the reference for the extraction (“System:” combo-box). By default, the “System:” combo-box is set to “Global”, but can be set to any local system (e.g. “SYS1”) or the Material system. The system combo box in the Results interface is used for deciding whether the stress/strain/displacement selected must be interpreted in the global, local or material direction. The coordinates of the extraction points are reported in both local and global coordinates. Local coordinates are identified based on selected system number (#) and system type:

- “X(SYS#), Y(SYS#), Z(SYS#) for Cartesian.
- “R(SYS#), T(SYS#), Z(SYS#) for Cylindrical/Polar.
- “R(SYS#), T(SYS#), P(SYS#) for Spherical.

Global coordinates are given as Cartesian regardless of the system type selected and labeled as X(Global), Y(Global), Z(Global). Note: if a Cylindrical system is selected, the extraction values will be in terms of R, T, Z instead of X, Y, Z. For example, Sx will be transformed to radial stress and Sy will be transformed to tangential stress.

For more information on extractions in Cylindrical coordinates, refer to StressCheck Tutorial: Results in Cylindrical Coordinates (R, T, Z) and How Do I View Radial and Hoop Stresses/Strains?

### Specifying the Integration Radius (K1/K2/J1p/J2p/J3p Only)

If one or more fracture mechanics parameters (i.e. K1, J1p) are selected for points extraction, a Radius: option will appear to allow the user to input the radius of integration for the CIM or J-integral, respectively (Figure 7).

By default, Radius: is set to “AUTO”, meaning the radius of integration will automatically be determined based on the boundary layer thickness along the crack front. However, if Radius: is enabled the user may input a specific integration radius. For guidelines on the selection of the integration radius, refer to Fracture Mechanics Analysis Overview.

If, during the extraction of the SIF or J-integral, the radius of the integration path is too large and falls outside the domain, the program will reduce its size by half and try again. This operation will be repeated up to five times, each time dividing the previous radius by 2. If, after five attempts, the radius is still too large, the computation of the SIF will fail and a warning message will be issued.

### Performing the Points Extraction

Once all selections have been made, and options specified, click on the Accept button. The Points extraction will be performed at **all requested locations** **within the model domain** for the selected Solution ID(s), Run(s) and function(s), and a graph pane will be produced containing exportable details on the Points extraction. A new Points extraction may be performed at any time, resulting in a new graph pane. If the “Display Pts.” button was enabled, a red “+” will appear in the Model View at each extraction location. If the “Display Pts.” and “Label” buttons were enabled, a point number (N) will accompany the red “+” at each extraction point. To clear these labels, click the right mouse button while the Model View has focus.

When computing function average values (i.e. “Average” button enabled) from a sequence of at least 3 solutions, StressCheck performs an estimation of the true value of the selected function by projecting the results from the finite element solutions to an infinite number of degrees of freedom. The result of this projection is reported as the “Estimated Limit” together with the percent deviation from the value corresponding to the solution chosen having the highest number of degrees of freedom. The below shows a typical graph output where Sx and Sy were computed on a circular boundary using 88 points:

Note: For the Point extraction interface, if an element edge is selected and the analysis reference is Extrusion, then it is possible to interpret the extraction to indicate the position of the edge in any plane parallel to the XY-plane. This feature allows defining the extraction procedure in 2D, and then interpreting the extraction as if the edge is located in an arbitrary plane (defined by the Z-plane input field) when the model is extruded.