You can use the elastic remeshing method to specify that the motion of the interior nodes is induced by the motion of the boundaries.
Select the Elastic remeshing menu.
Elastic remeshing
Specify the domain of the elastic remeshing method using the Domain of the sub-task menu, in the manner described previously for the fixed domain method.
Deformation domain
Define the deformation of the domain by specifying the deformation method for each of the topological entities, setting the mesh distortion check criteria, and defining the modulus used in the pseudo-elastic equation. Note that the elastic remeshing method requires sufficient boundary conditions for the entities to ensure that the whole domain does not undergo rigid motion.
Because the number of entities can be quite large, they are grouped in lists according to their geometric dimension (that is, surfaces, lines, and points). It is recommended that you follow a top-down approach, to methodically define the methods on each entity: first the surfaces, then the lines, and finally the points. At any point during this process you can click Upper level menu to automatically check if the methods applied on adjacent entities are compatible. If an incompatibility is detected, a message will appear in the output text window of Ansys Polydata (see Figure 2.14: Output Text Window) that explains the cause of incompatibility and the topological entities involved.
For 3D geometries, define the method of deformation and associated boundary conditions for surfaces.
Methods on surfaces
The Methods on surfaces of domain <domain name> menu will open (where <domain name> is the name of the domain you defined in the previous step), displaying a list of all of the relevant surfaces. By default, no methods are applied on the surfaces, and so they are listed in this menu as having no constraints on surface. If a surface has a method imposed on it because an adjacent domain already has a deformation method defined (for example, Fixed domain, Rigid translation), the imposed method will be displayed in the list and you cannot modify it.
Select a surface in the list and click the button to enter the Method along <surface name> menu.
Click Modify method: <current method name>.
Modify method:<current method
name>
The Select method along <surface name> menu will open.
Select the appropriate method for the surface. You have the following choices:
To allow the position of the nodes to be computed by the remeshing method defined on the domain of higher dimension, select no constraints on surface.
Select method: no constraints on
surface
Click Upper level menu to return to the Method along <surface name> menu.
To specify that the motion of the interior nodes is induced by the boundary motions, select elastic remeshing.
Select method: elastic
remeshing
This model requires boundary conditions, which you can define either by clicking Boundary conditions in the Method along <surface name> menu, or by clicking Methods on lines in the Preprocessor: mesh deformation menu.
Click Upper level menu to return to the Method along <surface name> menu.
If the surface is a plane and you would like the interior nodes to move in this plane with a motion that is induced by the boundary motions, select planar elastic remeshing.
Select method: planar elastic
remeshing
This model requires boundary conditions, which you can define either by clicking Boundary conditions in the Method along <surface name> menu, or by clicking Methods on lines in the Preprocessor: mesh deformation menu.
Click Upper level menu to return to the Method along <surface name> menu.
To specify that the interior nodes move along a ruled surface induced by the motion of two opposing boundary lines, select ruled surface.
Select method: ruled surface
After you have selected this option, the Specify the starting line of the ruled surface menu item will be available for selection, so that you can specify the starting line. Select this option to open the Select a starting line menu. Select the appropriate line and click the button. The selected line will then be listed as the Starting line.
This model requires boundary conditions, which you can define either by clicking Boundary conditions in the Method along <surface name> menu, or by clicking Methods on lines in the Preprocessor: mesh deformation menu. It is recommended that you allow the generation lines to be free lines (that is, have no constraints imposed).
Click Upper level menu repeatedly until you return to the Method along <surface name> menu.
Important: The ruled surface menu item should only be selected if the surface meets the criteria described for the ruled surface method in Surface Transformations. If the surface also meets the criteria for the sliceable ruled surface method, you should consider using this latter method (as described in the option that follows), as the sliceable ruled method moves the nodes according to the pseudo-elastic equation. The ruled surface method, on the other hand, uses linear interpolation for the motion of the nodes.
To specify that the interior nodes move along a ruled surface induced by the motion of two opposite boundary lines, select sliceable ruled surface.
Select method: sliceable ruled
surface
After you have selected this option, the Specify the starting line of the ruled surface item will be available for selection, so that you can specify the starting line. Select this option to open the Select a starting line menu. Select the appropriate line and click the button. The selected line will then be listed as the Starting line.
This model requires boundary conditions, which you can define either by clicking Boundary conditions in the Method along <surface name> menu, or by clicking Methods on lines in the Preprocessor: mesh deformation menu. It is recommended that you allow the generation lines to be free lines (that is, have no constraints imposed).
Click Upper level menu repeatedly until you return to the Method along <surface name> menu.
Important: Ansys Polydata does not check if the surface is really sliceable. It is your responsibility to provide a sliceable mesh on the surface.
To specify uniform motion for the nodes in a given direction, select rigid translation.
Select method: rigid
translation
After you have selected this option, the Modify direction of movement and Modify amplitude of movement items will become available. Click these items and revise the default values in the panels that open, as necessary.
Important: You can use an evolution function or a user-defined template to define the amplitude. Simply click the EVOL or button under the Ansys Polydata menu bar prior to clicking Modify amplitude of movement. After you have approved the amplitude value in the panel, the appropriate menus will open. Click Upper level menu to return to the Select method along<surface name> menu.
After the direction and amplitude are defined, click Upper level menu to return to the Method along <surface name> menu.
To specify that the nodes of the surface remain fixed at their original coordinates, select fixed surface.
Select method: fixed surface
Click Upper level menu to return to the Method along <surface name> menu.
To specify that the surface be treated as a plane of symmetry, select symmetry.
Select method: symmetry
This model requires boundary conditions, which you can define either by clicking Boundary conditions in the Method along <surfacename> menu, or by clicking Methods on lines in the Preprocessor: mesh deformation menu.
Click Upper level menu to return to the Method along <surface name> menu.
Specify the boundary conditions of the surface.
Boundary conditions
The Methods on lines of <surface name> menu will open, presenting a list of boundary lines for the current surface. By default, any undefined line will be listed as a free line (that is, no constraints).
Select a line in the list and click the button. The Method along <line name> menu will open, which provides options for defining the deformation of the line. See the section that follows related to the setup for the Methods on lines of domain <domain name> menu for further details.
Click Upper level menu to return to the Methods on lines of <surface name> menu and continue selecting lines for modification until all the boundary conditions for the surface are appropriately defined. Then click the button to return to the Method along <surface name> menu.
Click Upper level menu to return to the Method on surfaces of domain <domain name> menu.
Repeat steps 3.(a)i.–3.(a)v. for each of the remaining surfaces.
Click Upper level menu to return to the Preprocessor: mesh deformation menu.
Define the method of deformation and associated boundary conditions for lines. Note that this step is only necessary if you did not specify all of the boundary conditions when defining the motion of the surfaces, or if you want to modify an existing line setup.
Methods on lines
The Methods on lines of domain <domain name> menu will open (where <domain name> is the name of the domain you defined in a previous step), displaying a list of all of the relevant lines. By default, no method is applied on a given line, and it is listed as being a free line. A line may be listed with a deformation method as a result of your boundary condition definitions for the motion of surfaces, or if a method has been imposed on it because an adjacent domain already has a deformation method defined. In the latter case, you cannot modify the imposed method.
Select a line in the list and click the button to open the Method along <line name> menu.
Click Modify method: <current method name>.
Modify method:<current method
name>
The Select method along <line name> menu will open.
Select the appropriate method for the line. You have the following choices:
To allow the position of the nodes to be computed by the remeshing method defined on the domain of higher dimension, select free line.
Select method: free line
Click Upper level menu to return to the Method along <line name> menu.
To specify that the motion of the interior nodes is induced by the boundary motions, select elastic remeshing.
Specify method: elastic
remeshing
This model requires boundary conditions, which you can define either by clicking Boundary conditions in the Method along <line name> menu, or by clicking Methods on points in the Preprocessor: mesh deformation menu.
Click Upper level menu to return to the Method along <line name> menu.
To specify the deformation of a line by defining control points, select line deformation.
Select method: line deformation
At a minimum, this model requires that you specify a value for the direction at one node and a value for the amplitude at one node. You may define further control points as desired, imposing a direction and/or the amplitude. You can define a control point either by clicking Boundary conditions in the Method along <line name> menu, or by clicking Methods on points in the Preprocessor: mesh deformation menu.
Click Upper level menu to return to the Method along <line name> menu.
To specify uniform motion for the nodes in a given direction, select rigid translation.
Select method: rigid
translation
After you have selected this option, the Modify direction of movement and Modify amplitude of movement items will become available. Click these items and revise the default values in the panels that open, as necessary.
Important: You can use an evolution function or a user-defined template to define the amplitude. Simply click the EVOL or button under the Ansys Polydata menu bar prior to clicking Modify amplitude of movement. After you have approved the amplitude value in the panel, the appropriate menus will open. Click Upper level menu to return to the Method along <line name> menu.
After the direction and amplitude are defined, click Upper level menu to return to the Method along <line name> menu.
To specify that the nodes of the line remain fixed at their original coordinates, select fixed line.
Select method: fixed line
Click Upper level menu to return to the Method along <line name> menu.
To specify that the line be treated as a line of symmetry, select symmetry.
Select method: symmetry
Important: The symmetry method for lines is only available for 2D geometries.
This model requires boundary conditions, which you can define either by clicking Boundary conditions in the Method along <line name> menu, or by clicking Methods on points in the Preprocessor: mesh deformation menu.
Click Upper level menu to return to the Method along <line name> menu.
Specify the boundary conditions of the line.
Boundary conditions
The Methods on points of <line name> menu will open, presenting a list of boundary nodes for the current line. By default, any undefined point will be listed as a free point (that is, no constraints).
You can perform the following actions in this menu:
modify the method on a control point
Select a node in the list and click the button. The Modify control point menu will open, which provides options for defining the motion of the control point. See the section that follows related to the setup for the Methods on points of domain <domain name> menu for further details.
Click Accept current setup - Vertex #<ID> to return to the Methods on points of <line name> menu, and continue selecting nodes for modification until the boundary conditions for the line are appropriately defined.
add a new control point
Click the button to the left of Add a new control point to open the Modify control point menu, where you can select a node and designate the deformation method of the point. Note that the button is only available if you have specified the line deformation method for the associated line.
By default, the first node of the line that is not already designated as a control point will be selected. You can select a different node by clicking either the Move upstream -1 / -5 item or the Move downstream +1 / +5 item as many times as necessary, thus moving along the line in increments of 1 or 5 nodes. The number of the node that is currently selected will be displayed in the Modify control point menu, and the graphics display window will show where it is located on the line.
Next, select a deformation method for the new control point. See the section that follows related to the setup for the Methods on points of domain <domain name> menu for further details.
Click Accept current setup - Vertex #<ID> to return to the Methods on points of <line name> menu, and continue adding new control points as necessary.
Click the button to return to the Method along <line name> menu.
If you selected line deformation for the method in step 3.(b)iii. and you added a control point to the line, then you have the option of removing a control point. To begin, click Remove control points to open the Delete control points of <line name> menu. Then, select the node you no longer want as a control point, and click the button. After you approve the deletion in the panel that opens, the control point will be removed.
Important: Only added control points can be removed. A panel will open with a warning if you attempt to delete a boundary node, and no action will be taken.
When you have finished deleting control points on the line, click Upper level menu to return to the Method along <line name> menu.
Click Upper level menu to return to the Methods on lines of domain <domain name> menu, and repeat steps 3.(b)i.–3.(b)v. for each of the remaining lines.
Click Upper level menu repeatedly until you return to the Preprocessor: mesh deformation menu.
Define the method of motion for points. Note that this step is only necessary if you did not specify all of the boundary conditions when defining the deformation of the lines, or if you want to modify an existing point setup.
Methods on points
The Methods on points of domain <domain name> menu will open, listing all of the nodes and their current methods. No methods are applied by default, on the nodes, and so each node for which this is true is listed as being a free point. A node may be listed with a motion method as a result of your boundary condition definitions for the deformation of lines, or if a method has been imposed on it because an adjacent domain already has a deformation method defined. In the latter case, you cannot modify the imposed method.
Select a node in the list and click the button to enter the Modify control point menu.
Select the appropriate method for the node. You have the following choices:
To allow the position of the node to be computed by the remeshing method defined on the domain of higher dimension, select free point.
Select method: free point
Click Accept current setup - Vertex #<ID> to return to the Methods on points of domain <domain name> menu.
To specify only the direction of the displacement of the node, select direction imposed.
Select method: direction
imposed
Note that the amplitude will be determined by the deformation method applied on the associated line.
After you have selected this option, the Modify direction of movement item will become available. Click this item and revise the default values in the panels that open, as necessary.
Click Accept current setup - Vertex #<ID> to return to the Methods on points of domain <domain name> menu.
To specify the direction and the amplitude of the displacement of the node, select direction and amplitude imposed.
Select method: direction and amplitude
imposed
After you have selected this option, the Modify direction of movement and Modify amplitude of movement items will become available. Click these items and revise the default values in the panels that open, as necessary.
Important: You can use an evolution function or a user-defined template to define the amplitude. Simply click the EVOL or button under the Ansys Polydata menu bar prior to clicking Modify amplitude of movement. After you have approved the amplitude value in the panel, the appropriate menus will open. Click Upper level menu to return to the Modify control point menu.
Click Accept current setup - Vertex #<ID> to return to the Methods on points of domain <domain name> menu.
To specify only the amplitude of the displacement of the node, select amplitude imposed.
Select method: amplitude
imposed
Note that the direction will be determined by the deformation method applied on the associated line.
After you have selected this option, the Modify amplitude of movement item will become available. Click this item and revise the default value in the panel that opens, as necessary.
Important: You can use an evolution function or a user-defined template to define the amplitude. Simply click the EVOL or button under the Ansys Polydata menu bar prior to clicking Modify amplitude of movement. After you have approved the amplitude value in the panel, the appropriate menus will open. Click Upper level menu to return to the Modify control point menu.
Click Accept current setup - Vertex #<ID> to return to the Methods on points of domain <domain name> menu.
When a node remains fixed at its original coordinates because it is part of a surface or line that is fixed, the only available option is fixed point.
Select method: fixed point
imposed
Note that this option is not available for nodes that are part of a surface or line that is not fixed. In such circumstances the only way to fix the node is by selecting amplitude imposed and specifying an amplitude of 0.
Click Accept current setup - Vertex #<ID> to return to the Methods on points of domain <domain name> menu.
Repeat steps 3.(c)i. and 3.(c)ii. for each of the remaining points.
Click Upper level menu to return to the Preprocessor: mesh deformation menu.
If the associated task is not a steady task, define checks for element distortion by clicking Element distortion check in the Preprocessor: mesh deformation menu.
Element distortion check
The Element distortion check menu will open, allowing you to make changes to the criteria Ansys Polyflow will use when evaluating the element distortion that results from the remeshing. The default settings are appropriate for most cases.
If any of the elements reach the specified distortion limits during the simulation, the manner in which Ansys Polyflow will proceed will depend on whether you selected Stop if distortion limits exceeded or Warning if distortion limits exceeded. If you selected the former, the current calculation is halted momentarily and adjustments are made, so that the global simulation can proceed. For example, a time-dependent simulation will halt the current time step and then proceed with a time step that is half of the original value. If you selected Warning if distortion limits exceeded, the simulation will continue unaltered but you will receive a warning.
When you are satisfied with the distortion check criteria, click Accept the current setup. Ansys Polydata will perform an immediate evaluation of the initial mesh quality in the domain of the current sub-task. If the initial mesh exceeds the criteria in any way, you will receive a warning. You can then perform one of the following options:
Save your session, go back into your meshing tool, and create a better initial mesh.
Modify the distortion check criteria such that the initial mesh is within the limits.
Make sure that Warning if distortion limits exceeded is selected and proceed with the simulation.
Creating a better initial mesh is the best option of those described previously, as it is not a good idea to start with a highly distorted initial mesh. The other options should only be used for the sake of interest, and even then, only if you know in advance that the mesh deformations you defined will not yield elements that are too distorted.
Define how the modulus
is calculated for the pseudo-elastic equation
(Equation 35–3), and
therefore specify whether and in what manner the mesh element
quality indicators are factored into the elastic remeshing.
Numerical parameters for elastic remeshing
The Numerical parameters for elastic remeshing menu will open, where you have the following choices:
To specify that the mesh is treated as an isotropic homogeneous pseudo-elastic medium, select Select modulus: constant. This option is only recommended for simple deformations, as it does not account for the quality of the mesh elements.
Select modulus: constant
To specify that the modulus is a function of the element quality, such that the elements with worse quality at a given iteration of the solution are stiffer than those with better quality, select Select modulus: function of quality indicator Q. This option corresponds to Equation 35–8, and is recommended for complex geometries.
Select modulus: function of quality indicator
Q
After you have selected this option, the Modify modulus exponent n = <current value> item will become available. The exponent defined by this item corresponds to
in Equation 35–8. Click this item and revise the default value in the
panel that opens, as necessary. To specify that the modulus is a function of the element quality, such that the stiffness of an element increases when it becomes more distorted relative to its initial undeformed state (and vice versa), select Select modulus: function of quality indicator ratio Q/Q0. This option corresponds to Equation 35–7, and is recommended for complex geometries. This option is selected by default, as it is most likely to provide suitable results.
Select modulus: function of quality indicator
ratio Q/Q0
After you have selected this option, the Modify modulus exponent n = <current value> item will become available. The exponent defined by this item corresponds to
in Equation 35–7. Click this item and revise the default value in the
panel that opens, as necessary.
Click Upper level menu to return to the Preprocessor: mesh deformation menu.
Click the button to return to the Task menu, and continue defining the task.