Using Sets in StressCheck

Sets are a convenient way of grouping objects together in user-defined collections for visualization, assignment of attributes, extractions, etc. Sets may be user-defined, in which the user provides a unique Set name and then specifies the collection of objects to be included in the set, or automatically-generated, such as after making an assignment of a material or boundary condition via selection of objects from the Model View.

In the latter case, Sets will have the prefix “SET” followed by the next available integer. The below animation shows the creation of a new surface Set “SET8” after the assignment of a traction to a selected surface:

To define a Set, select the Sets tab in the Input dialog, set the Object and Method combo-boxes of the C/A/O/M to the desired configuration, and specify a unique Set name in the ID: box. New sets must be given a name and may be defined either by explicitly selecting individual objects in the Model View (Method: Selection), selecting a surface or bounded group of surfaces which encloses the desired objects (Method: Region), or by defining a box location/dimensions that will be used to identify the objects for selection (Method: Locate). In the latter case, any object which lies within the box location/dimensions, or which intersects with the box surfaces, will be selected. Finally, click the Accept button to add the Set. The Set can now be used anywhere the Set: combo-box appears. To check the contents stored in the Set, select the Set definition record from the listbox and its contents will be returned to the “Contents:” list.

The below animation shows the definition of a surface Set “SURFS” based on the marquee selection of surfaces:

Note: Set names cannot start with “SET” or “_” since “SET” and “_” are prefixes exclusively used for automatically created Sets.

Object Selection for Set Definitions

There are three methods available for specifying a list of objects to be included in a Set definition: Selection, Region and Locate.

Selection Method

To define a Set by the Selection method, you may select an object or group of objects by object type (such as Edge, Face, Any Surface, Any Boundary, Any Element, Any Body, etc.) or use Any Object to select any object independent of object type. An object is selected from the Model View by pointing to it and clicking on the left mouse button.

• A group of objects can be marquee selected by left-clicking and dragging the cursor until the desired group is completely enclosed in a rectangular box.
• Holding the Shift key down while left-clicking will allow selection of multiple objects for assignment.
• 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.
• If you wish to cancel the current selection of objects, simply right-click on the Model View.

Note: to select internal elements when defining sets, disable the Wetted Faces toggle before marquee selecting the elements from the Model View.

Region Method

Attributes such as thickness, material, p-Discretization, and some element-oriented boundary conditions may be assigned according to whether an element (or object) lies within the boundaries of a sheet body or within the volume of a geometric shell. This feature is particularly useful for assigning attributes to sub-domains of parts with automatically generated meshes.

To define a Set by the Region method, select a surface or bounded group of surfaces (i.e. geometric shell) which encloses the desired objects. All elements (or objects) attached to the selected sheet body or lying within the volume of the selected geometric shell will automatically be selected for Set definition.

Locate Method

To define a Locate set, choose the Locate method. Supply the X,Y,Z coordinates of the center of the base of the box, and the width, height and depth of the box. The base of the box is located in the XY plane at Z=0. As you tab through the input fields, you will see the box appearing on the screen. When you have supplied the desired location and dimensions, click Accept to complete the Set definition.

Note: In most cases, explicit selection of objects from the Model View is the best way to define Sets, but there are situations when Locate sets are necessary. For example, applying thickness, material properties and element-based boundary conditions to sub-regions of an automatically meshed parametric model will require the use of Locate sets. This is because the model will be remeshed in response to a change in a parametric dimension, and the attributes assigned to elements in the original model will no longer be valid.

By defining Locate sets, attributes will automatically be re-assigned to whatever elements (or objects) lie within the defined box location/dimension. In the current release, only rectangular boxes that are aligned with the global coordinate system may be defined.

Adding a Set Definition

Once an object or group of objects are selected, to add the new Set definition record simply click the Accept button. If an existing Set definition record has already been selected from the scrolling list, you first must click Deselect to cancel the current selection of objects. Then, you are able to update the Set name in the ID: box and create the new Set definition record as usual.

Note: If you enable the check box next to the Set ID: box, all existing Locate sets will be displayed in the Model View. When you select a Locate set record from the list box, the outline will be highlighted in the Model View, and the input values will feed back to the user interface. You may modify these values and click Replace to revise the definition of the Locate set.

A Note About Model Inputs and Sets

All Model Input interfaces that create Sets automatically have a combo-box (Set: ) which permits the use of pre-defined Sets. If you wish to use a pre-defined Set rather than to create a new Set by explicit selection, choose the pre-defined Set name from the Set: combo-box before clicking Accept. To create Sets by explicit selection, the combo box should be set to “New set”.

A Note On Assigning Attributes to Element Sets

The specification of an element Set is required for the assignment of certain model attributes, such as material properties and body force loads. However, efficiently and reliably defining the element Set(s) may require the selection of surface/solid geometry (i.e. Mesh Region or Any Body Sets) or the identification of meshed body numbers (i.e. Automeshed Element Sets).

Assignment by Mesh Region

Attributes such as thickness, material, p-discretization, and some element oriented boundary conditions may be assigned according to whether an element lies within the boundaries of a sheet body or within the volume of a geometric shell. This feature is particularly useful for assigning attributes to automatically generated meshes. Choose the AOM settings Select > Mesh Region > Selection then select a geometric surface. All elements attached to the selected sheet body or lying within the volume of the selected geometric shell will automatically be selected. Clicking Accept will then generate a Region Set containing these elements.

Assignment by Any Body

Attributes such as material, p-discretization, and some element oriented boundary conditions may be assigned according to whether an element is associated with a body (or bodies) . As with the Mesh Region method, this feature is particularly useful for assigning attributes to automatically generated meshes. Choose the AOM settings Select > Any Body > Selection then select one or more geometric bodies. All elements associated to the selected body (or bodies) will automatically be selected.

When Any Body is used for assignment of attributes, such as material properties, some elements within the body (or bodies) may not be selected. This may happen because elements created inside the body (or bodies) but not associated to the body (or bodies) will not be recognized by the Any Body option. In this respect, Mesh Region and Any Body methods are complementary methods.

Assignment by Automesh Element Sets

When MeshSim is used, StressCheck will automatically create element Sets for each automeshed body. The Set ID will have the name _AUTO_B_#, in which the # is a sequential number identifying each meshed body. These mesh Sets may then be selected when assigning attributes using Any Element as the object. If the automesh for any body must be regenerated, then the assignment of attributes using these mesh Sets will be updated automatically.

For more information on defining and using Sets, refer to StressCheck Tutorial: Using Sets and How Do I Use Sets to Select and View Groups of Elements and Other Objects?

Querying/Replacing/Deleting a Set Definition

If the user wishes to query a list of the current objects stored in an existing Set definition record, edit the objects in an existing Set definition record, or delete an existing Set definition record, the user first selects the Set definition record from the scrolling listbox directly under the C/A/O/M combo-boxes. Once it is selected, the Accept button will become inactive and the Replace and Delete buttons will be activated.

Querying a Set Definition Record

Starting with StressCheck v12.0, it is now possible to query the Set definition contents (“Contents” list), as well as if/where a Set definition was used in model assignments (“Used By:” list), for any selected Set ID.

For example, selecting an element face Set (SET11) from the Set definitions listbox will result in the population of the “Contents:” list with the elements/face numbers currently stored in the Set ID and, since the Set ID was used in the assignment of a load record (“LOAD1”), the population of the “Used By:” list with that reference:

Replacing a Set Definition Record

Once a Set definition record is selected, the user may update the objects in the Set definition, and then click Replace to update the Set definition record. After clicking Replace, the Accept button will become active and the Replace and Delete buttons will become inactive. Note that the Set definition record must be re-selected to refresh the “Contents:” and “Used By:” lists.

Deleting a Set Definition Record

Once a Set definition record is selected, the user may click Delete to delete the Set definition record. After clicking Delete, the Accept button will become active and the Replace and Delete buttons will become inactive. Note: warnings may occur if the deleted Set was used in any model assignments, such as material or boundary condition assignments.

Removing All Set Definition Records

To remove all Set definition records, click the Purge button. Note: warnings may occur if any Sets were used in model assignments, such as material or boundary condition assignments.