Assignment of Constraints in StressCheck

To assign constraint boundary conditions to a StressCheck model, select the Constraint 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 constraint ID in the ID: combo-box. Then, select the object or objects to be constrained and input the constraint data. Constraints may be constant, parametric or formula-based, and may be assigned to geometric or mesh objects. Finally, click on Accept to add the constraint assignment record to the constraint ID.

To assign a constraint record to a different constraint case, simply specify a different constraint ID in the ID: combo-box before clicking Accept. The below animation shows a normal/tangent Spring Coefficient constraint of Kn = 1e6 lbf/in/in^2 and Kt = 1e4 lbf/in/in^2 being assigned to a surface:

Summary of Constraint Methods

Many methods are available for assigning constraints, including General, Spring Coefficient, Rigid Body and more. The constraining objects/methods available depend on the currently selected reference (Planar, 3D, etc.).

Note: Rotation constraints (e.g. Rx, Ry, Rz) are not applicable to Planar and 3D solid elements. Rotation constraints are applicable to beam elements only.

Boundary Constraint Methods

General

General means that you will prescribe one, two or three displacement components to one or more boundaries in the global or in a local Cartesian coordinate system. For example, if one of the boundaries of the solution domain lies on a plane of symmetry, which in 2D elasticity appears as a line of symmetry then you will prescribe the normal displacement to be zero.

For General constraints the data type may be Fixed, Constant, Parametric or Formula. Fixed means that the selected displacement component is set to zero.

• If the displacement is constant along a boundary then the constant value must be entered into the appropriate field.
• A parameter or parametric expression can be used also to specify a prescribed displacement. The value of the displacement is computed from a parametric expression entered in the corresponding input field. Any combination of previously defined parameters and constants can be used.
• For the formula type, the formula name is entered into the appropriate box. When a formula is defined in a coordinate system other than the global system, then the name of the coordinate system must be entered also.

For an example of a general constraint being used to compress a coil spring by a prescribed displacement, refer to StressCheck Demo: 3D Geometric Nonlinear Analysis.

Symmetry

Symmetry means the normal displacement component is set to zero. Symmetry constraints are applicable only to straight edges or flat faces. A check is automatically performed every time symmetry is specified to make sure that the selected face or faces are flat. A warning message is issued if symmetry is applied to faces which are not flat.

Note: for axially symmetric (Axisym.) analyses, in theory there is no need to constrain the Ur displacement component along the Z-axis. However, due to issues related to numerical precision, it is recommended to specify symmetry constraints along R=0.

Antisymmetry

Antisymmetry means the tangential displacement components are set to zero. Antisymmetry constraints are applicable only to straight edges or flat faces. A check is automatically performed every time anti symmetry is specified to make sure that the selected face or faces are flat.

Built-In

Built-In means all displacement components are set to zero (fixed). The selected edges or faces can be flat or curved.

Floating

Floating means prescribing one or more directions (in global or in a local Cartesian coordinate system) in which all the selected edges/faces are constrained to move by the same amount. For example, in the unit cell shown below, representative of a typical fiber/matrix arrangement, three faces have symmetry constraints, while the other three have floating symmetry constraints in the direction normal to the faces (Global Z-direction):

In this example, the user simply selects the group of faces to be constrained and checks the direction of the floating constraint (Z) to create the record.

Note: floating constraints are not compatible with multi-body contact analysis.

Spring Coefficients (Spring Coeff.)

When an elastic body is constrained by means of distributed springs, or loaded by displacements imposed on distributed springs, then the spring coefficients modify the stiffness matrix. For this reason the spring coefficients are entered as constraints, and the magnitudes are in units of force/length/area. In the case of Spring Coefficients the data type may be Constant, Parametric, or Formula.

• Spring coefficients can be specified in the direction of the Global or a local coordinate system, or in the direction normal/tangent (Norm./Tan.) to the selected object(s).
  • For Norm./Tan., the tangent direction means all tangents on the selected object(s). Tangent spring coefficients with magnitudes << E (where E is the elastic modulus of the body) may be used to constrain rigid body rotations if constraining a node or nodes will introduce modeling errors.
• Two options are available for spring coefficient inputs: Force/Length/Area (default) or Force/Length.
  • If Force/Length is input, then the spring rate in force/length will be distributed over the selected surface area(s).

For an example of a spring coefficient constraint being used to support a 3-Pt bending specimen, refer to StressCheck Tutorial: 3-Pt Bending Specimen with Normal Spring Constraints.

For details on performing a compression-only spring analysis or defining a formula spring coefficient, refer to How Can I Perform a Compression Only Spring Analysis? and StressCheck Tutorial: Defining a Formula Spring Coefficient.

Multi-Body Contact Constraint Methods

Contact

Specify the contact spring coefficient (in units of force/length/area) to be used for a multi-body contact analysis; alternately, after two contact zones have been selected and if material properties are assigned to the bodies associated with the contact zones, the Generate button may be pressed to automatically generate the recommended contact constant.

Once the contact spring coefficient is specified, and two contact zones are selected, click Accept to generate the Contact constraint.

For an example of defining contact zones and pairing the contact zones with contact constraints for a fitting/I-beam fastened connection, refer to StressCheck Tutorial: Fitting + I-Beam Multi-Body Contact Analysis. Note: Contact zones are created by selecting surfaces or faces in 3D and curves or edges in 2D (Mesh tab, set A/O/M to Create > Contact Zone). At least two contact zones must be created for each potential contact pair.

For more details on the multi-body contact implementation, requirements, and guidelines, refer to Multi-Body Contact Overview, Numerical Simulation Series: Mechanical Contact, Introduction to Multi-Body Contact in StressCheck, Helpful Hints and Tips: Multi-Body Contact Overview and General Recommendations and What Are Some Common Multi-Body Contact Issues?.

Auto Contact

With the release of StressCheck v12.0, a new contact method is available (Auto Contact) to accommodate the automatic generation and assignment of contact pairs based on surface proximity during assembly meshing. Three options are available to independently control each Auto Contact constraint assignment:

• Contact: associated contact pair will use the Contact method outlined above during a multi-body contact analysis (default).
• Fused: if neighboring element faces/edges/node locations perfectly match after assembly meshing, will “fuse”/bond the associated contact pair during a multi-body contact analysis.
• Free: associated contact pair will be ignored during a multi-body contact analysis.

To learn more about this method, refer to the “Auto Contact” section in Multi-Body Contact Overview.

Point Constraint Methods

There are two (2) point constraint methods: Rigid Body and Node. To specify a Rigid Body or Node constraint, the object Node or Point should be selected first.

In 2D (Planar) elasticity there are three (3) rigid body modes per body, and in 3D elasticity there are six (6) rigid body modes per body; in axially symmetric (Axisym.) elasticity, there is only one rigid body mode which is a rigid body translation in the Z-direction.

Point constraints are admissible only for preventing rigid body displacement and rotation; the body must be in equilibrium under the action of external forces. Unlike the errors introduced by concentrated forces, errors introduced by point constraints are not localized, except when the point constraints are to prevent rigid body displacement only, in which case the body must be in equilibrium under the applied forces. In every other case the reactions at point constraints are dependent on the mesh and the polynomial degree of elements. For this reason multipoint constraints should not be used.

Rigid Body

StressCheck provides a convenient way for specifying rigid body constraints. Rigid body constraints should only be used if the body is in equilibrium under the applied loads.

• In the case of 2D (Planar) elasticity the user selects two nodes. StressCheck will then create a right-handed local coordinate system, the x-axis of which is directed from the first node to the second. In this local coordinate system both displacement components are constrained for the first node; only the displacement component in the direction of the local y-axis is constrained for the second node.
• In the case of 3D elasticity, The user selects three non-colinear nodes, and StressCheck creates a right-handed local coordinate system, the x-axis of which is directed from the first node to the second. In this local coordinate system, all displacement components are constrained for the first node; two displacement components are constrained for the second node, and only one displacement component for the third node.

For more information on rigid body constraints, refer to When Can I Use Rigid Body or Node Constraints?, Helpful Hints and Tips: Using the 3-2-1 Rigid Body Constraint Approach and Helpful Hints and Tips: Constraining Rigid Body Motion.

Single Node/Point (Node)

Individual nodes/points can be constrained in one or more directions by checking Data Type: Fixed and enabling the X, Y and/or Z inputs. Care must be taken to ensure the model is not over constrained. In the case of beams, three displacements (X, Y and Z) and three rotations (Rx, Ry and Rz) in global coordinate directions can be prescribed.

Note: in the Extrude reference, an additional “Extrude” option will appear that, when checked, will duplicate the node constraint above and below the midplane. This option is recommended in the event rigid body rotation is present after extruding:

For more details, refer to When Can I Use Rigid Body or Node Constraints?

Fastener Constraint Methods (Planar Only)

Fastener elements may be constrained through fixed/imposed displacements (Displacement) or connected to each other via infinite shear stiffness (Rigid Connection). For more details, refer to Fastened Connection Analysis Overview.

Displacement

Specify fixed or prescribed displacement components for the center of a fastener element. A fastener element has two degrees of freedom associated with its center.

Connection

Create a rigid connection (infinite shear stiffness) between two or more fasteners that share the same xy-coordinates.

Selecting Objects for Assignment to a Constraint ID

You may constrain an object (such as an edge, boundary, face, or surface) or a group of objects during constraint assignment. 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: assigning to geometric objects, if associated with elements, will result in the associated elements inheriting the assignment. It is recommended to assign constraints to geometry whenever applicable in case the mesh is updated.

Specifying a Set for Assignment to a Constraint ID

Alternatively, if a there is a set definition containing a list of objects for assignment, the name of this set may be specified in the Set: combo-box instead of selecting the objects from the Model View. Simply select the name of the set, and the objects in the set list will automatically be selected in the Model View.

Constraint Directions

You may select the Norm./Tan. reference frame or the XY (Planar) or XYZ (3D) reference frame, the default of which is the Global system. The positive normal is understood to be the outward normal. To select a different reference frame, select the desired system from the System: combo-box.

In 2D, the direction of the tangent is such that moving in that direction the positive normal is to the right. Depending on your choice for direction, either the Normal and Tangent or the X and Y components will be highlighted. You may select either or both. For example, if you wish to apply a constraint only in the tangential direction, then turn on the checkbox in front of tangent and turn off the checkbox in front of Normal.

Constraint Data Types

The data type may be fixed, constant, formula or parametric. Fixed means that the selected displacement component is set to zero. If the displacement is constant along a boundary then the constant value must be entered into the appropriate box.

The parametric option can be used also to specify a prescribed displacement. The value of the displacement is computed from a parametric expression (up to 15 characters long) entered in the corresponding input field. Any combination of previously defined parameters and constants can be used.

Prescribed displacement components may be specified by formulas. The formula name is entered into the appropriate box. When a formula is defined in a coordinate system other than the global system then the name of the coordinate system must be entered also.

Adding an Assignment to a Constraint ID

Once an object or group of objects are selected, and a constraint ID is specified in the ID: combo-box, to add the new constraint assignment record to the record listbox directly under the C/A/O/M combo-boxes simply click the Accept button. Note: if an existing constraint assignment record has already been selected from the record listbox, you first must choose Set: “New set” or re-select the action, object, or method. Then, you are able to create the new constraint assignment record as usual.

Replacing/Deleting an Assignment to a Constraint ID

If the user wishes to edit the data in an existing constraint assignment record, or delete an existing constraint assignment record, the user first selects the constraint assignment record from the record listbox directly under the C/A/O/M combo-boxes. Once it is selected, the Status column will read “Selected”, signifying the record can be replaced (updated) or deleted.

Replacing a Constraint Assignment Record

Once a constraint assignment record is selected, the user may update the data in the Constraint tab, and then click Replace to update the constraint assignment record. After clicking Replace, the Accept button will become active and the Replace and Delete buttons will become inactive.

Deleting a Constraint Assignment Record

Once a constraint assignment record is selected, the user may click Delete to delete the constraint assignment record. After clicking Delete, the Accept button will become active and the Replace and Delete buttons will become inactive.

Removing All Constraint Assignment Records

To remove all constraint assignment records, regardless of constraint ID, click the Purge button.

Querying/Deleting/Purging Constraint ID’s via Edit Constraint Cases

By clicking the Edit button at the bottom of the Constraint tab, a dialog is displayed to provide the user the ability to query single constraint records, delete single or multiple constraint records (Delete button), entire constraint ID’s (Purge ID button), or the full records list (Purge List). The Edit Constraint Cases dialog (Figure 14) allows the user to display all records (Show All) or sort constraints by ID.

• Individual records shown in the list can be selected by clicking the corresponding row. The Constraint tab of the Input dialog will update to display the associated constraint record data, and the Model View will update to highlight the objects associated with the constraint record set name.
• Multiple records can be selected by holding Ctrl and picking each row desired for selection.
• A continuous series of records can be chosen by clicking on the first row, and then dragging the mouse to the last row, or hold down Shift while pressing the up or down arrow keys to extend the selection or directly click on the last row to complete the selection.
• The Previous and Next buttons can be used for cycling through individual records on the list. Once a record(s) has been selected, the Delete button can be used to remove it from the list.
• To remove an entire constraint ID, simply select the correct ID from the dropdown and click Purge ID.
• Purge All can be used at any time to remove all of the records from the list.