This section describes how to create a geometric restriction in a shape optimization. The following topics are covered:
You can specify the minimum or maximum size of selected regions of your model; for example, the minimum thickness of a rib that is modified during the shape optimization. The value that you enter can be thought of as a radius. During the optimization the Optimization module restrains the thickness of a member to be twice the value that you entered (the diameter). If you enter a value for the minimum thickness, the Optimization module adjusts surface nodes such that the minimum diameter must be achieved along a normal to the surface of the model. If the structure is smaller than the specified value in certain regions, the shape optimization permits only growth until the member size in the regions areas satisfies the restriction. Conversely, if you enter a value for the maximum thickness, the Optimization module adjusts surface nodes such that a maximum diameter must be achieved along a normal to the surface of the model. If the structure is larger than the specified value in certain regions, the shape optimization permits only shrinkage until the member size in the regions areas satisfies the restriction.
To create a member size geometric restriction:
From the main menu bar, select Geometric Restriction
Create.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create. procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the 
tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Member size (Shape) from the list of geometric restrictions, and click Continue.
From the viewport, select the region to which the member size restriction will be applied or click Done to apply the member size restriction to the entire model.
By default, Abaqus/CAE allows you to select all of the model. To select faces or cells, use the Selection toolbar to change the type of object that you can select to Face or Cells. For more information, see “Filtering your selection based on the type of object,” Section 6.3.2.
If you would rather select from a list of existing sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting the geometric restriction region, click Done in the prompt area. For more information on selecting objects, see Chapter 6, “Selecting objects within the viewport.”
The Edit Geometric Restriction dialog box appears.
Do either of the following:
Select Minimum thickness, and enter the minimum radius of a member.
Select Maximum thickness, and enter the maximum radius of a member.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the selected regions already include members larger than the minimum thickness. If the regions include smaller members, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle, and the regions include smaller members, the Optimization module issues an error message and stops execution.
Click OK to create the member size geometric restriction and to exit the editor.
You can specify a planar symmetry geometric restriction for a shape optimization. A planar symmetry geometric restriction forces selected faces of the optimized model to be symmetric about a specified plane. You specify the plane of symmetry by selecting the axis of a coordinate system that is the normal to the plane of symmetry. The origin of the coordinate system is a point on the plane of symmetry. You can use the global coordinate system, or you can create a datum coordinate system (see “An overview of the methods for creating a datum coordinate system,” Section 62.5.4, for more information).
The mesh must be approximately symmetric across the plane of symmetry before the optimization starts so that the Optimization module can identify pairs of nodes on either side of the plane of symmetry—the master node and the slave node. By default, the master node is the node that the optimization moves out the most (the most growth) or moves in the least (the least shrinkage). The optimization displaces the master node, and the symmetry condition applies an equal displacement to the slave node so that it remains symmetrical to the master node. Alternatively, if you are trying to optimize surfaces that are in contact, you can force the Optimization module to select the master node as the node to which the optimization is applying the least growth or the most amount of shrinkage.
To create a planar symmetry restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Planar symmetry from the list of geometric restrictions, and click Continue.
From the viewport, select the faces in which the planar symmetry will be enforced. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Select the coordinate system, and select the axis of the coordinate system that represents the normal to the plane of symmetry.
Select the method that the optimization will use to determine the master point. In most cases you should select Determine from most growth and least shrinkage. You should select Determine from least growth and most shrinkage only if you are trying to optimize faces that are involved in contact.
Enter the tolerance that will be used to determine symmetric points in the X-, Y-, and Z-axes.
The Optimization module uses the tolerance to identify the pairs of symmetric nodes across the symmetry plane.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the faces are already symmetric about the plane. If the faces are not symmetric, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle, and the faces are not symmetric, the Optimization module issues an error message and stops execution.
Click OK to create the planar symmetry geometric restriction and to exit the editor.
You can specify a rotational symmetry geometric restriction for a shape optimization. A rotational symmetry geometric restriction forces selected faces of the optimized model to be symmetric about a specified axis. You choose the axis of symmetry by specifying the starting and ending coordinates of a vector representing the axis. You can use the global coordinate system, or you can create a datum coordinate system (see “An overview of the methods for creating a datum coordinate system,” Section 62.5.4, for more information).
The mesh must be approximately symmetric around the axis of symmetry before the optimization starts so that the Optimization module can identify the group of nodes that sit on a selected face in a plane normal to the axis of symmetry. By default, the master node is the node in the group that the optimization moves out the most (the most growth) or moves in the least (the least shrinkage). The optimization displaces the master node, and the symmetry condition applies an equal displacement to the rest of the nodes in the group (the slave nodes) so that they remain symmetrical about the axis. If you are trying to optimize surfaces that are in contact, you can force the Optimization module to select the master node as the node to which the optimization is applying the least growth or the most amount of shrinkage. Alternatively, you can select a single point that will be used as the master node by all other nodes. The optimization determines how much the master node is displaced, and all other nodes are moved the same amount so that they remain symmetric about the selected axis.
To create a rotational symmetry restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Rotational symmetry (Shape) from the list of geometric restrictions, and click Continue.
From the viewport, select the faces in which the rotational symmetry will be enforced. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Enter the coordinates of the starting point and the ending point of a vector representing the axis of symmetry.
Toggle on Create a repeating pattern, and enter the angle over which the pattern created by the optimization will be repeated. The value must be between 0° and 360°. A value of 0° implies the slave nodes are symmetric about the axis of symmetry, but the optimization does not create a repeating pattern.
Select the method that the optimization will use to determine the master point. In most cases you should select Determine from most growth and least shrinkage. You should select Determine from least growth and most shrinkage only if you are trying to optimize faces that are involved in contact.
Alternatively, you can select Region and select a vertex that will be used to represent the master node.
Enter the tolerance that will be used to determine symmetric points in the X-, Y-, and Z-axes.
The Optimization module uses the tolerance to identify the nodes on the surface that lie on a plane normal to the axis of symmetry and are equidistant from the axis of symmetry.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the faces are already symmetric about the axis. If the faces are not symmetric, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle and the faces are not symmetric, the Optimization module issues an error message and stops execution.
Click OK to create the rotational symmetry geometric restriction and to exit the editor.
You can specify a point symmetry geometric restriction for a shape optimization. A rotational symmetry geometric restriction forces selected faces of the optimized model to be symmetric about a specified point of symmetry. You specify the point of symmetry by selecting a coordinate system (the point of symmetry is assumed to be the origin of the coordinate system). You can use the global coordinate system, or you can create a datum coordinate system (see “An overview of the methods for creating a datum coordinate system,” Section 62.5.4, for more information).
The mesh must be approximately symmetric about the point before the optimization starts so that the Optimization module can identify pairs of nodes on either side of the point of symmetry—the master node and the slave node. By default, the master node is the node that the optimization moves out the most (the most growth) or moves in the least (the least shrinkage). The optimization displaces the master node, and the symmetry condition applies an equal displacement to the slave node so that it remains symmetrical to the master node. Alternatively, if you are trying to optimize surfaces that are in contact, you can force the Optimization module to select the master node as the node to which the optimization is applying the least growth or the most amount of shrinkage.
To create a point symmetry restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Point symmetry (Shape) from the list of geometric restrictions, and click Continue.
From the viewport, select the faces in which the point symmetry will be enforced. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Select the coordinate system. The point of symmetry is assumed to be the origin of the selected coordinate system.
Select the method that the optimization will use to determine the master point. In most cases you should select Determine from most growth and least shrinkage. You should select Determine from least growth and most shrinkage only if you are trying to optimize faces that are involved in contact.
Enter the tolerance in the X-, Y-, and Z-planes that will be used to determine symmetric points .
The Optimization module uses the tolerance to identify the nodes that are symmetric to the point of symmetry.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the faces are already symmetric about the point. If the faces are not symmetric, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle and the faces are not symmetric, the Optimization module issues an error message and stops execution.
Click OK to create the point symmetry geometric restriction and to exit the editor.
You can specify a stamp control geometric restriction for a shape optimization. A stamp control geometric restriction results in an optimized model that can be manufactured by a tool and die stamping operation along a specified direction. You choose the direction by specifying the starting and ending coordinates of a vector representing the direction. You can use the global coordinate system, or you can create a datum coordinate system (see “An overview of the methods for creating a datum coordinate system,” Section 62.5.4, for more information).
The mesh should define a stampable model before the optimization starts; otherwise, the mesh may become distorted when the optimization creates a stampable model in the first iteration. The master node can lie anywhere in the region that you select to be governed by the stamp restriction. By default, the master node is the node in the region that the optimization moves out the most (the most growth) or moves in the least (the least shrinkage). The optimization displaces the master node, and the stamp condition applies an equal displacement to the rest of the nodes in the region (the slave nodes) so that the model remains stampable. If you are trying to optimize surfaces that are in contact, you can force the Optimization module to select the master node as the node to which the optimization is applying the least growth or the most amount of shrinkage. Alternatively, you can select a single point that will be used as the master node by all other nodes. The optimization determines how much the master node is displaced, and all other nodes are moved the same amount so that the model remains stampable.
To create a stamp control restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Stamp control from the list of geometric restrictions, and click Continue.
From the viewport, select the faces to which the stamp control will be applied. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing face sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Enter the coordinates of the starting point and the ending point of a vector representing the direction along which the stamping tool moves.
Enter the draw angle, which represents the angle of the tool that is creating the stamped model. The value must be between 0° and 45°.
Enter a positive value for the amount of undercut that can be tolerated in the stamping region.
Select the method that the optimization will use to determine the master point. In most cases you should select Determine from most growth and least shrinkage. You should select Determine from least growth and most shrinkage only if you are trying to optimize faces that are involved in contact.
Alternatively, you can select Region and select a vertex that will be used to represent the master node.
Enter the tolerance in the X-, Y-, and Z-axes.
The Optimization module uses the tolerance to identify the nodes on the surface that lie on a plane normal to the axis of symmetry and are equidistant from the axis of symmetry.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the model is stampable. If the model is not stampable, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle and the model is not stampable, the Optimization module issues an error message and stops execution.
Click OK to create the stamp control geometric restriction and to exit the editor.
You can specify a turn control geometric restriction for a shape optimization. A turn control geometric restriction results in an optimized model that can be manufactured by a tool on a lathe cutting into the model along a specified direction. You choose the direction by specifying the starting and ending coordinates of a vector representing the direction. You can use the global coordinate system, or you can create a datum coordinate system (see “An overview of the methods for creating a datum coordinate system,” Section 62.5.4, for more information).
The mesh should define a turnable model before the optimization starts; otherwise, the mesh may become distorted when the optimization creates a turnable model in the first iteration. The master node can lie anywhere in the region that you select to be governed by the turn restriction. By default, the master node is the node in the region that the optimization moves out the most (the most growth) or moves in the least (the least shrinkage). The optimization displaces the master node, and the stamp condition applies an equal displacement to the rest of the nodes in the region (the slave nodes) so that the model remains turnable. If you are trying to optimize surfaces that are in contact, you can force the Optimization module to select the master node as the node to which the optimization is applying the least growth or the most amount of shrinkage. Alternatively, you can select a single point that will be used as the master node by all other nodes. The optimization determines how much the master node is displaced, and all other nodes are moved the same amount so that the model remains turnable.
To create a turn control restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Turn control from the list of geometric restrictions, and click Continue.
From the viewport, select the faces to which the turn control will be applied. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing face sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Enter the coordinates of the starting point and the ending point of a vector representing the direction along which the cutting tool moves.
Select the method that the optimization will use to determine the master point. In most cases you should select Determine from most growth and least shrinkage. You should select Determine from least growth and most shrinkage only if you are trying to optimize faces that are involved in contact.
Enter the tolerance in the X-, Y-, and Z-axes.
The Optimization module uses the tolerance to identify the nodes on the surface that lie on a plane normal to the axis of symmetry and are equidistant from the axis of symmetry.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the model is turnable. If the model is not turnable, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle and the model is not turnable, the Optimization module issues an error message and stops execution.
Click OK to create the turn control geometric restriction and to exit the editor.
You can specify a demold geometric restriction for a shape optimization. A demold geometric restriction forces the optimized model to satisfy specified manufacturing requirements; for example, it can prevent undercuts and hollow regions in a part that must be extracted from a mold. You choose the demolding direction by specifying the starting and ending coordinates of a vector representing the axis. You can use the global coordinate system, or you can create a datum coordinate system (see “An overview of the methods for creating a datum coordinate system,” Section 62.5.4, for more information).
The mesh should define a demoldable model before the optimization starts; otherwise, the mesh may become distorted when the optimization creates a demoldable model in the first iteration. The master node can lie anywhere in the region that you select to be governed by the demold control restriction. By default, the master node is the node in the region that the optimization moves out the most (the most growth) or moves in the least (the least shrinkage). The optimization displaces the master node, and the stamp condition applies an equal displacement to the rest of the nodes in the region (the slave nodes) so that the model remains demoldable. If you are trying to optimize surfaces that are in contact, you can force the Optimization module to select the master node as the node to which the optimization is applying the least growth or the most amount of shrinkage. Alternatively, you can select a single point that will be used as the master node by all other nodes. The optimization determines how much the master node is displaced, and all other nodes are moved the same amount so that the model remains demoldable.
To create a demold control restriction:
From the main menu bar, select Geometric RestrictionCreate
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Demold control from the list of geometric restrictions, and click Continue.
From the viewport, select the faces to which the demold control will be applied. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing face sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
By default, the region in which the Optimization module checks for collisions is the same as the region in which it enforces the demold restriction. If desired, select 
from the top of the Edit Geometric Restriction dialog box, and select the collision check region.
Faces inside the collision check region cannot be penetrated by faces outside the region. If a node attempts to penetrate an element in the collision check region during the shape optimization, the Optimization module scales back the displacement of the node. The collision check region must include the faces to which the demold control will be applied.
Enter the coordinates of the starting point and the ending point of a vector representing the direction along which a mold is withdrawn from the demold region.
Enter the draw angle, which represents the angle of a mold that is being withdrawn from the demold region. The value must be between 0° and 45°.
Enter a positive value for the amount of undercut that can be tolerated in the demold control region.
Select the method that the optimization will use to determine the master point. In most cases you should select Determine from most growth and least shrinkage. You should select Determine from least growth and most shrinkage only if you are trying to optimize faces that are involved in contact.
Enter the tolerance in the X-, Y-, and Z-axes.
The Optimization module uses the tolerance to identify the nodes on the surface that lie on a plane normal to the axis of symmetry and are equidistant from the axis of symmetry.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes a mold could be withdrawn from the demold region. If the mold could not be withdrawn, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle, and the mold could not be withdrawn, the Optimization module issues an error message and stops execution.
Click OK to create the demold geometric restriction and to exit the editor.
You can specify a drill control geometric restriction for a shape optimization. A drill control geometric restriction results in an optimized model that can be manufactured by a tool drilling into the model along a specified direction. The hole created by the tool is symmetric about the axis of the tool. In addition, the tool can be withdrawn from the hole. You choose the axis of the tool (and the drilling direction) by specifying the starting and ending coordinates of a vector representing the axis. You can use the global coordinate system, or you can create a datum coordinate system (see “An overview of the methods for creating a datum coordinate system,” Section 62.5.4, for more information).
The mesh should define a drillable model before the optimization starts; otherwise, the mesh may become distorted when the optimization creates a drillable model in the first iteration. The master node can lie anywhere in the region that you select to be governed by the drill control restriction. By default, the master node is the node in the region that the optimization moves out the most (the most growth) or moves in the least (the least shrinkage). The optimization displaces the master node, and the stamp condition applies an equal displacement to the rest of the nodes in the region (the slave nodes) so that the model remains drillable. If you are trying to optimize surfaces that are in contact, you can force the Optimization module to select the master node as the node to which the optimization is applying the least growth or the most amount of shrinkage. Alternatively, you can select a single point that will be used as the master node by all other nodes. The optimization determines how much the master node is displaced, and all other nodes are moved the same amount so that the model remains drillable.
To create a drill control restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Stamp control from the list of geometric restrictions, and click Continue.
From the viewport, select the faces to which the drill control will be applied. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing face sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Enter the coordinates of the starting point and the ending point of a vector representing the direction along which the drilling tool moves.
Enter the draw angle, which represents the angle of the tool that is drilling the hole. The value must be between 0° and 45°.
Enter a positive value for the amount of undercut that can be tolerated in the drill control region.
Select the method that the optimization will use to determine the master point. In most cases you should select Determine from most growth and least shrinkage. You should select Determine from least growth and most shrinkage only if you are trying to optimize faces that are involved in contact.
Alternatively, you can select Region and select a vertex that will be used to represent the master node.
Enter the tolerance in the X-, Y-, and Z-axes.
The Optimization module uses the tolerance to identify the nodes on the surface that lie on a plane normal to the axis of symmetry and are equidistant from the axis of symmetry.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the model is drillable. If the model is not drillable, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle and the model is not drillable, the Optimization module issues an error message and stops execution.
Click OK to create the drill control geometric restriction and to exit the editor.
A penetration check geometric restriction in a shape optimization results in an optimized model with faces that cannot penetrate selected regions.
To create a surface penetration check restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Penetration check (Shape) from the list of geometric restrictions, and click Continue.
From the viewport, select the faces to which the penetration check will be applied. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing face sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Select the regions that cannot be penetrated by faces of the optimized model.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the model is not already penetrating the selected regions. If the model is penetrating the selected region, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle and the model is penetrating the selected region, the Optimization module issues an error message and stops execution.
Click OK to create the penetration check geometric restriction and to exit the editor.
You can specify a fixed region restriction for a shape optimization. A fixed region is restrained in selected degrees of freedom (1-, 2-, or 3-direction. The degrees of freedom are defined relative to a selected coordinate system.
To create a fixed region restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Fixed region from the list of geometric restrictions, and click Continue.
From the viewport, select the faces to which the fixation will be applied. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing face sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Select the coordinate system that defines the degrees of freedom. You can select the global coordinate system, or you can create a datum coordinate system (see “An overview of the methods for creating a datum coordinate system,” Section 62.5.4, for more information).
Toggle on the degrees of freedom that you want to restrain.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the region is already restrained in the selected degrees of freedom. If the region has displacement in the selected degrees of freedom, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle and the region has displacement in the selected degrees of freedom, the Optimization module issues an error message and stops execution.
Click OK to create the fixed region geometric restriction and to exit the editor.
You can specify a growth restriction for a shape optimization. A growth restriction limits how much a face can grow (surface nodes are moved out) or shrink (surface nodes are moving in) relative to the initial design. For example, if you are optimizing a model that will be cast, you can use a growth restriction to control the maximum and minimum wall thickness in a region.
To create a growth restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Growth from the list of geometric restrictions, and click Continue.
From the viewport, select the faces to which the growth restrictions will be applied. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing face sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Toggle on Maximum in shrink direction, and enter a positive value specifying the maximum inward displacement of a surface node.
Toggle on Maximum in growth direction, and enter a positive value specifying the maximum outward displacement of a surface node.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the growth of the face is already limited. If the growth of the face exceeds the specified value, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle and the growth of the face exceeds the specified value, the Optimization module issues an error message and stops execution.
Click OK to create the growth geometric restriction and to exit the editor.
You can specify a design direction restriction for a shape optimization. You can use a design direction restriction to keep selected nodes of your model on a planar or circular surface during the optimization. The optimization displaces the master node, and the design direction restriction applies an equal displacement (either magnitude or direction or both) to the rest of the nodes in the region (the client nodes). In addition, you can specify the axes of a coordinate system (rectangular, cylindrical, or spherical) that are applied.
The mesh should define nodes that can be moved along the design direction before the optimization starts; otherwise, the mesh may become distorted when the optimization moves nodes in the first iteration. The master node can lie anywhere in the region that you select to be governed by the design direction restriction. By default, the master node is the node in the region that the optimization moves out the most (the most growth) or moves in the least (the least shrinkage). If you are trying to optimize surfaces that are in contact, you can force the Optimization module to select the master node as the node to which the optimization is applying the least growth or the most amount of shrinkage. Alternatively, you can select a single point that will be used as the master node by all other nodes.
To create a design direction restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Design Direction from the list of geometric restrictions, and click Continue.
From the viewport, select the faces to which the design direction restriction will be applied. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing face sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Choose whether a client node should follow the master node by moving in the same direction or with the same magnitude or both.
If you chose to move a client node in both the same direction and with the same magnitude as the master node, toggle on the axes along which the movement will be applied.
Select the method that the optimization will use to determine the master node. In most cases you should select Determine from most growth and least shrinkage. You should select Determine from least growth and most shrinkage only if you are trying to optimize faces that are involved in contact.
Alternatively, you can select Region and select a vertex that will be used to represent the master node.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the nodes can be moved along the specified design direction. If the nodes cannot be moved along the design direction, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle and the nodes cannot be moved along the design direction, the Optimization module issues an error message and stops execution.
Click OK to create the design direction geometric restriction and to exit the editor.
You can specify a slide region control, or contact, geometric restriction for a shape optimization. A slide region control geometric restriction results in an optimized model with a face that contacts a specified surface and follows the contours of the surface. You can select the specified surface from the model. Alternatively, the specified surface can be a surface of revolution generated by a rotating a selected face about a selected axis. You choose the axis of rotation by specifying the starting and ending coordinates of a vector representing the axis. You can use the global coordinate system, or you can create a datum coordinate system (see “An overview of the methods for creating a datum coordinate system,” Section 62.5.4, for more information).
If you select the face from the model, the definition of the surface slide control restriction is complete. If you select a face that will be used to form a surface of revolution, the Optimization module selects the master node from the nodes on the face. By default, the master node is the node on the face that the optimization moves out the most (the most growth) or moves in the least (the least shrinkage). The optimization displaces the master node, and the surface slide restriction forces an equal displacement to the rest of the nodes on the face (the slave nodes) so that the contact conditions are satisfied.
To create a surface slide control restriction:
From the main menu bar, select Geometric RestrictionCreate.
The Create Geometric Restriction dialog box appears.
Tip: You can initiate the Create procedure in two other ways:
Click Create in the Geometric Restriction Manager. (You can display the Geometric Restriction Manager by selecting Geometric RestrictionManager from the main menu bar.)
Click the tool in the Optimization module toolbox.
From the Create Geometric Restriction dialog box that appears, enter the name of the geometric restriction.
Select Slide region control from the list of geometric restrictions, and click Continue.
From the viewport, select the faces to which the surface slide control will be applied. For more information, see “Using the face curvature method to select multiple faces,” Section 6.2.4.
If you would rather select from a list of existing face sets, do the following:
Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available sets.
Select the set of interest, and click Continue.
Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.
When you have finished selecting faces, click Done in the prompt area.
The Edit Geometric Restriction dialog box appears.
Select the approach that you will use to define the contact surface.
If you selected the Free-form approach, select the contact surface.
If you selected the Conserve a turnable surface approach, do the following:
Select the starting point and the ending point of a vector representing the axis of rotation.
Select the coordinate system that defines the vector. You can select the global coordinate system, or you can create a datum coordinate system (see “An overview of the methods for creating a datum coordinate system,” Section 62.5.4, for more information).
Enter the tolerance in the X-, Y-, and Z-axes.
The Optimization module uses the tolerance to identify the nodes on the contact surface.
If desired, toggle on Ignore in first design cycle (default). When the optimization starts, it assumes the surfaces are in contact. If the surfaces are not in contact, the Optimization module issues a warning and tries to continue. If you toggle off Ignore in first design cycle and the surfaces are not in contact, the Optimization module issues an error message and stops execution.
Click OK to create the slide region control geometric restriction and to exit the editor.