ANSYS, Inc. Release Notes
ANSYS, Inc. Release Notes
This release of the Meshing application contains many new features and enhancements. Areas where you will find changes and new capabilities include the following:
Note the following when resuming databases from previous releases:
Upon import of a legacy model into release 14.0, suppressed virtual topology entities will be deleted. This includes any virtual topology entities that were suppressed manually (for example, by right-clicking on the virtual topology entity in the Tree Outline and selecting Suppress from the context menu), but it does not include virtual topology entities that are suppressed because the body containing them is suppressed. If entities are deleted, a warning message will be issued advising you to import the model into an earlier release, unsuppress the affected entities, and save the model for use in release 14.0. Also see the Virtual Topology section below.
At release 13.0, all mesh connections were pre, but at release 14.0, all mesh connections are post. Upon import of a release 13.0 database into release 14.0, all mesh connections are updated accordingly.
When assembly meshing algorithms are used in release 14.0, Program Controlled inflation is not supported on solid bodies. The solid bodies will not be inflated. If you import a release 13.0 database that specifies the CutCell meshing algorithm and Program Controlled inflation is defined on a solid body, you must either change the Fluid/Solid designation of the solid body to Fluid or set Use Automatic Inflation to None and define local inflation controls to obtain the release 13.0 behavior. Also see the Assembly Meshing section below.
Contact regions are now resolved automatically as interfaces for use in ANSYS FLUENT. In support of this change, if you import a legacy model with all of the following characteristics into release 14.0, a message will be issued to advise you that if you do not want the contact regions to be resolved, you should delete them:
Physics Preference is set to CFD.
Solver Preference is set to Fluent.
Contact regions are defined.
However, if you do want the legacy contact regions to be resolved, you must clear and regenerate the mesh in the release 14.0 Meshing application prior to exporting/opening the mesh in ANSYS FLUENT.
Also see the Miscellaneous Changes and Behaviors section below for related information.
The logic for translating material properties of bodies/parts to continuum zone types when a mesh is exported to ANSYS FLUENT format has changed in release 14.0. Body/part names and Named Selection names are no longer considered. However, upon import of a legacy model into release 14.0, the Fluid/Solid material property for each body will be set based on pre-14.0 rules.
Special handling of sheet bodies occurs during migration based on whether the model is 3D (not planar in the XYZ plane) or 2D (planar in the XYZ plane):
If 3D or in cases in which only surface mesh is being exported, migration of sheet bodies is skipped. The pre-14.0 rules are not used to interpret the naming of the sheet bodies, and no material properties are assigned to them.
If 2D, pre-14.0 rules are applied to the sheet bodies as follows:
If Named Selections, part names, and/or body names are defined, they are applied according to the following priority:
Named Selections defined for the underlying faces in a sheet body. In such cases, a message will be issued indicating the Named Selection definition for the faces will override the Fluid/Solid material property for the sheet body.
Named Selections defined for sheet bodies
Part names
Body names
This means that when defined, Named Selections for underlying faces take highest priority, then Named Selections for sheet bodies, then part names, then body names. An exception occurs if a part name would result in a material property of Solid but a body name would result in a material property of Fluid. In such cases, the sheet body is transferred as a Fluid.
If no Named Selections, part names, or body names are defined, the sheet bodies are transferred as continuum zones and the same rules as in the 3D case are applied.
A message will be issued if the migration results in a change to the material properties of any body, in which case you can perform a right mouse button click and select Go To Object from the context menu to select the object in the Tree Outline that is responsible for the message. Also see the FLUENT Export section below.
“Assembly meshing” refers to meshing an entire model as a single mesh process, as compared to part- or body-based meshing, in which meshing occurs at the part or body level respectively. If the assembly meshing Method control (described below) is set to None, ANSYS Workbench meshing operates at the part level, but if it is set to CutCell or Tetrahedrons, the entire assembly will be meshed at one time using the selected assembly meshing algorithm.
Assembly meshing should be able to produce conformal mesh between parts if their faces are overlapping.
Assemblies can also be meshed using part-based meshing methods, but in such cases the mesher operates one part at a time, and therefore cannot mesh virtual bodies or evaluate parts that occupy the same space.
The following enhancements have been made in support of assembly meshing at release 14.0:
Assembly Meshing—Overview
The Assembly Meshing group of global mesh controls is now available. You can use one of the controls, called Method, to choose either CutCell or Tetrahedrons as your strategy for assembly meshing. CutCell is available only in the Meshing application, and only when Physics Preference is set to CFD and Solver Preference is set to Fluent. Tetrahedrons is available in both the Meshing application and the Mechanical application, regardless of Physics Preference and Solver Preference settings.
The Tetrahedrons assembly meshing algorithm is a derivative of the CutCell algorithm, with strengths and weaknesses similar to those of CutCell. The Tetrahedrons method starts from the CutCell mesh and through various mesh manipulations creates a high quality unstructured tet mesh.
Named Selections are supported for assembly meshing. However, the mesher will not fail if a Named Selection is not protected; it will issue a warning.
Assembly Meshing—Global Improvements
A Fluid/Solid material property setting is now available in the Meshing application. This property, which appears in the Details view if you select a prototype (i.e., Body object) in the Tree Outline, allows you to control the physics that occur on a model. It affects how material properties are translated when you export a mesh for use in ANSYS FLUENT. Valid options are Fluid, Solid, and Defined By Geometry. When set to Defined By Geometry, the value is based on the Fluid/Solid material property that was assigned to the body in the DesignModeler application. The Fluid/Solid property also appears in the Details view if you select a Virtual Body object in the Tree Outline, but in such cases it is always set to Fluid (read-only). This property is not available if you are using the meshing capabilities from within the Mechanical application.
When setting local (scoped) sizing controls, the Body of Influence option for Type is supported. The body of influence cannot be scoped to a line body.
The default for Proximity Size Function Sources has been changed to Edges. This setting is sufficient for most models.
Assembly Meshing—Virtual Bodies
In principal, there are two approaches for extracting fluid domains from CAD:
For internal flow, cap the inlets, outlets, and any other leakage of the solid domain and perform a Boolean subtraction operation inside the CAD system to extract the flow volume.
For external flow, create a large external domain outside of the solid object, perform a Boolean subtraction operation inside the CAD system, and delete any remaining interior voids inside the solid.
However, depending on the number of solids and the quality (or “cleanliness”) of the original CAD, these Boolean operations may fail.
Assembly meshing provides the means of extracting and meshing the flow volume within both these scenarios in one operation, and hence eliminates the need for the Boolean operations. To use these approaches, capping faces or large external domains need to be created in the CAD system. These fluid domains are represented by virtual bodies in the Meshing application. You also need to define a coordinate system at any location inside the extracted fluid domain. When you insert a virtual body into the Tree Outline, a Virtual Body Group, representing the fluid type, is created with a Virtual Body as a child object. In the Details view settings for the Virtual Body, you associate the material point with the coordinate system.
Often, you are interested only in the fluid flow and hence the solid mesh is not needed. The Keep Solid Mesh control determines whether the mesh for any body marked as a solid is discarded or kept.
Since meshing all of the solids and then discarding the solid mesh would not be efficient, you can provide the Fluid Surface in addition to the material point inside the Virtual Body definition, thereby eliminating the need to mesh the solid and leading to improved meshing performance by a factor of two or more.
To aid in finding all the faces that are needed to create a Fluid Surface object, a new Extend to Connection option has been added to the Extend Selection drop-down menu. Before you use this tool, make sure that the global size function option Min Size/Proximity Min Size is set appropriately and that the Find Contacts tool has been executed.
Due to missing rubber seals, bolt threading, or other simplifications, the solid CAD may not be “watertight.” In these situations, the assembly meshing algorithms can trace the leaks and display their leak paths graphically to help you with troubleshooting.
Leakage usually occurs if any contact is larger than 1/10 of the local minimum size. If a leak is up to 1/3 of the local minimum size, you can use contact sizing to close the gap.
Assembly Meshing—Diagnostics Tools
For performing diagnostics for assembly meshing problems, the Find Thin Sections and Find Contacts tools are available. These tools return lists of contact regions based on the global size function option Min Size/Proximity Min Size, which should be set appropriately before you invoke them. When Find Thin Sections is executed (using RMB), each of the contact regions it returns contains faces on the same body that will not be resolved properly based on the current global minimum size. When Find Contacts is executed (using RMB), the tool returns a list of contacts, which is used to pass feature information down to the meshing algorithm. The Find Contacts tool is particularly useful for assemblies in which fillets of bodies are adjacent to other bodies, forming a sharp angle. Find Contacts will preserve the edges of these fillets independent of the feature angle settings.
Related to these tools, the Use Range option has been added as a global connection setting so that searches can operate on a range of values.
Assembly Meshing—Inflation
For the CutCell algorithm, inflation is neither Pre nor Post. Rather, it may be considered a hybrid of the two, in that the technology used is like that of the Pre algorithm, but inflation occurs Post mesh generation. For the Tetrahedrons algorithm, Pre inflation is used, with inflation behaviors and limitations very similar to those of the Patch Conforming Tetrahedron mesh method.
When an assembly meshing algorithm is being used, a mixture of global (automatic Program Controlled) and local (scoped) inflation is not supported; you must choose between the two approaches:
For inflation on virtual bodies, you must use automatic Program Controlled inflation; you cannot use local controls to inflate virtual bodies. Thus in general, if you are using virtual bodies to represent flow volumes in your model, plan to use automatic inflation. Automatic inflation is specified globally by setting Use Automatic Inflation to Program Controlled. With Program Controlled inflation, faces on real solid bodies will inflate into the virtual bodies. The Fluid/Solid designation on real bodies will be respected (that is, faces on real fluid bodies will inflate into the fluid region, but the solid region will not be inflated).
Alternatively, you can set Use Automatic Inflation to None and define local inflation controls. This approach is appropriate if your model contains real bodies that represent the fluid regions.
If any global or local inflation settings are modified and you re-mesh, only the inflation layers are regenerated. This is true for both approaches, regardless of which assembly meshing algorithm is selected.
Assembly meshing algorithms support 3D inflation only. Unlike 3D inflation for part/body level meshing, for assembly level meshing the scoped body and the face that you select to be the inflation boundary do not have to be on the same part.
By default, Gap Factor is set to 1.5 for the CutCell algorithm. For the Tetrahedrons algorithm, Gap Factor is set equal to the value that is specified for non-assembly mesh methods (0.5 by default) and is updated accordingly if that value is changed.
Assembly Meshing—Additional Tools
The new Sharp Angle Tool lets you control the capture of features with sharp angles, such as the edge of a knife or the region where a tire meets the road. It can also be used for improved feature capturing in general, even if the faces that you pick to define a control do not form a sharp angle. The Sharp Angle Tool is available only when assembly meshing algorithms are being used and ensures that the desired features are captured in the assembly mesh.
Mesh groups are used to merge adjacent bodies into one body. The grouping tells the mesher to treat certain solid parts as one part and ensures that the mesh generated on the combined parts is associated with the mesh of the selected master body. Mesh grouping is available only when assembly meshing algorithms are being used. Mesh Group objects appear in the Tree Outline under the Mesh object.
Also see the Miscellaneous Changes and Behaviors section below.
At release 14.0, either the pinch control feature or the mesh connection feature can be used to join shell meshed parts after meshing.
In support of this functionality, a new option for specifying PinchBehavior is available for local pinch controls. Edge-to-edge pinch controls can be “pre” or “post, ” but edge-to-face pinch controls are always post. When set to Pre, pinches are processed before face meshing, and when set to Post, pinches are processed in a separate step after all meshing is complete.
At release 13.0, all mesh connections were pre, but at release 14.0, all mesh connections are post. The mesh connection feature leverages the Post pinch technology to automatically generate Post pinch controls internally at meshing time. This technology allows mesh connections to work across parts so that a multibody part is no longer required.
The Snap to Boundary option, which was already available for edge-to-face pinch controls, is now supported for edge-to-face mesh connections as well. When Snap to Boundary is set to Yes (the default) and the distance from a slave edge to the closest mesh boundary of the master face is within the specified snap to boundary tolerance, nodes from the slave edge are projected onto the boundary of the master face. In addition, you have more control over the snap type and snap tolerance. By default the snap tolerance is set equal to pinch tolerance, but setting the Snap Type option to Manual Tolerance lets you override it. Alternatively, you can set Snap Type to Element Size Factor to enter a factor of the local element size of the master topology. For edge-to-edge pinch controls or edge-to-edge mesh connections, the snap tolerance is set equal to the pinch tolerance internally and cannot be modified.
When used on parts and bodies that have been joined by mesh connections or post pinch controls, the Clear Generated Data option now works as follows, where the "base" mesh, which is stored in a temporary file, is the mesh in its unsewn (pre-joined) state:
If a base mesh is available, the mesh is reverted to the base mesh and the requested parts/bodies are cleared.
If no base mesh is available, the entire mesh is cleared and a warning message is issued. Reasons the base mesh may not be available include situations in which you have deleted your temporary files, exported a .mechdat file for someone else to use, or moved your project database to a different computer.
The selective meshing process (formerly known as direct meshing) has been improved at release 14.0. You can use the Mesh worksheet to create a selective meshing history, so that your meshing steps can be repeated in the desired sequence for any geometry update or re-mesh operation. You can populate the worksheet either by recording meshing steps as you perform them or by adding meshing steps to the worksheet manually. In each meshing step, the bodies associated with a given Named Selection are meshed. For greater flexibility, you can activate and deactivate steps in the worksheet to control whether they are processed or skipped during mesh generation and other worksheet operations.
The worksheet is dockable. Once you toggle it on, you can move it to the desired location which will persist whenever the Mesh object or one of its child objects is highlighted in the Tree Outline. For example, you may want to dock the worksheet alongside the Geometry window, allowing you to view both at once.
Also see the Miscellaneous Changes and Behaviors section below.
A new global group of meshing controls, called Patch Conforming Options, has been added at release 14.0. The first of these new options is Triangle Surface Mesher, which determines which triangle surface meshing strategy will be used by patch conforming meshers—either Program Controlled or Advancing Front. When set to Program Controlled, the mesher determines whether to use the Delaunay or advancing front algorithm based on a variety of factors such as surface type, face topology, and defeatured boundaries. When set to Advancing Front, the mesher uses advancing front as its primary algorithm, but falls back to Delaunay if problems occur.
The Triangle Surface Mesher control has no effect on parts or bodies being meshed with the Patch Independent Tetra mesh method. The Patch Conforming Options group of controls is inaccessible when an assembly meshing algorithm is selected.
The following enhancements related to the MultiZone mesh method have been made at release 14.0:
Improved handling of imprints. This includes imprinting through multiple bodies, through multiple levels in the same body, and through long stretches of side faces. Improvements have been made to submapping of cylindrical faces with side cutouts, especially those used as side faces along the sweep path.
Support for match controls on faces has been added, with certain limitations.
A new Prism option is available for Mapped Mesh Type. The Prism option generates a mesh of all prism elements for the part the method is scoped to. This option is sometimes useful if the source face mesh is being shared with a tet mesh, as pyramids are not required to transition to the tet mesh.
Improved handling of edge splits.
The following enhancements related to the Uniform Quad/Tri and Uniform Quad mesh methods have been made at release 14.0:
Edge, face, and body sizing are supported. When using edge sizing, you can specify a Type of either Element Size or Number of Divisions. For face and body sizing, Type is always Element Size. The Sphere of Influence and Body of Influence options are not supported for Uniform Quad/Tri and Uniform Quad.
The Uniform Quad/Tri and Uniform Quad mesh methods support mesh connections and pinch controls (post pinch only).
The following enhancements and guidelines relate to size function handling at release 14.0:
When Use Advanced Size Function is set to On: Proximity and Curvature, you now have the option to specify a global Proximity Min Size to be used in proximity size function calculations, in addition to specifying a global Min Size. By default, Proximity Min Size is set equal to the default of Min Size. Any feature that operates based on minimum element size (for example, Defeaturing Tolerance, Pinch Tolerance, and Find Thin Sections), will now be based on the smaller of the two minimum size values.
When Use Advanced Size Function is set to On: Proximity, only Proximity Min Size is available.
In cases where you applied a hard size that is smaller than the minimum size, there may be a poor size transition in proximity to the entity with the hard size. To obtain a proper size transition, reduce the Defeaturing Tolerance used by the Automatic Mesh Based Defeaturing control (or turn off Automatic Mesh Based Defeaturing entirely).
The following enhancements related to virtual topology have been made at release 14.0:
You can select specific regions (i.e., bodies or faces) before running automatic virtual cell creation so that it operates on the selected regions only. The software groups adjacent entities appropriately to form the virtual cell(s).
To facilitate more efficient virtual topology operations, Virtual Cell and Virtual Split Edge objects no longer appear in the Tree Outline. This provides improved usability in cases involving very large numbers of virtual entities. The Virtual Topology object still appears in the Tree Outline and can be used for setting global virtual topology options. Other enhancements described in this section can be used for creating, deleting, and editing virtual entities.
A new Virtual Topology Properties dialog has been implemented. You can use this dialog to edit the properties of multiple selected virtual topology entities, and your changes will be applied to all selected entities at one time. You can access the dialog via right-mouse button click or by choosing the Edit button on the Virtual Topology context toolbar.
You can insert multiple virtual cells at one time when creating virtual cells manually. Select one or more faces or one or more edges and from the selected set of faces or edges, the software creates the virtual cell(s). During this process, adjacent selected entities are grouped appropriately to form virtual cell(s), while any single selected entity (that is, one that is selected but is not adjacent to any other selected entity) forms its own virtual cell.
You can select two vertices on a face to split the face, thereby creating 1 to N virtual faces. To facilitate split face operations, you can create a virtual hard vertex, which allows you to define a hard point according to your cursor location on a face, and then use that hard point in a split face operation. In support of these features, two new objects are available (Virtual Split Face and Virtual Hard Vertex). Similar to Virtual Cell and Virtual Split Edge objects, Virtual Split Face and Virtual Hard Vertex objects do not appear in the Tree Outline.
When you define a virtual split edge by selecting Insert> Virtual Split Edge from the context menu or by choosing Split Edge on the Virtual Topology context toolbar, the split location is set to 0.5 by default. You can change the value later by using the Virtual Topology Properties dialog, or by modifying the edge split interactively as described below.
Using the F4 key, you can interactively adjust previously defined virtual split edges and virtual hard vertices. In either case, any virtual split faces affected by the change are adjusted accordingly.
A Statistics group has been added to the Virtual Topology Details view. Here you can view counts of the virtual faces, virtual edges, virtual split edges, virtual split faces, virtual hard vertices, and total virtual entities that exist within the model.
The virtual topology feature is more flexible, with the addition of more options for deleting virtual topology entities. Regardless of which object is highlighted in the Tree Outline (for example, Geometry, Virtual Topology, Mesh, etc.), you can now select virtual entities in the Geometry window, right-click, and delete the selected virtual entities (and dependents if applicable). When the Virtual Topology object is highlighted, you have the additional option of selecting the Delete button on the Virtual Topology context toolbar. You also have the option to delete all virtual entities at one time—either by RMB click on the Virtual Topology object in the Tree Outline, or by RMB click on any virtual topology entity in the Geometry window.
Left/right arrow buttons have been added to the Virtual Topology context toolbar so that you can cycle through virtual topology entities in the sequence in which they were created and display them in the Geometry window.
Suppression of virtual entities has been disabled.
The following enhancements related to POLYFLOW Export have been made at release 14.0:
Named Selections are supported. When you export a mesh file from the Meshing application to POLYFLOW format (File> Export from the Meshing application main menu, then Save as type POLYFLOW Input Files), the Named Selections that were defined will appear in the exported mesh file.
PMeshes are supported. You can create Named Selections to specify specialized modeling conditions on edges for 2-D or shell geometry; and edges and faces for 3-D geometry. The exported mesh file will contain the mesh nodes and elements associated with those Named Selections in PMesh format.
Release 14.0 provides greater control over CGNS export operations. Using the Options dialog box, you can choose a file format (ADF or HDF5) and CGNS version (3.1, 3.0, 2.5, 2.4, 2.3, 2.2, or 2.1). The defaults are ADF and 3.1 respectively.
The following enhancements related to FLUENT Export have been made at release 14.0:
Body/part names and Named Selection names are no longer considered when assigning continuum zone types for use in ANSYS FLUENT. For databases created in release 14.0, the following logic is used to translate the material properties of the bodies/parts in the model to continuum zone types:
If Physics Preference is set to CFD and you do not set the Fluid/Solid material property as described in steps 2 and 3 below, all zones are exported to ANSYS FLUENT mesh format as FLUID zones by default.
The Fluid/Solid material property assigned in the DesignModeler application is considered next. This setting overrides the default behavior described in step 1.
The Fluid/Solid material property assigned in the Meshing application is considered next. This setting overrides the default behavior described in step 1 and the Fluid/Solid material property assigned in the DesignModeler application.
For information about this change and migration of legacy models into release 14.0, see the Resuming Databases from Previous Releases section above.
Using the Options dialog box, you can choose either the Binary or ASCII file format for greater control over FLUENT export operations.
At the time of mesh export, a boundary zone type of INTERFACE is now assigned automatically to the contact source and contact target entities that compose contact regions. When reading the mesh file, ANSYS FLUENT creates a mesh interface for each contact region automatically. For related information, also see the Resuming Databases from Previous Releases section above, and the Miscellaneous Changes and Behaviors section below.
Better quad smoothing occurs at release 14.0:
Improved Laplacian smoothing
More ruled mesh on rectangles, etc.
The following changes and behaviors are new at release 14.0:
The Meshing Options panel has been removed.
The CutCellMeshing group of global mesh controls has been renamed the Assembly Meshing group. One of the controls, which used to be called the Active control, has been renamed the Method control. It lets you choose the CutCell or Tetrahedrons method for assembly meshing.
The default for Proximity Size Function Sources has been changed to Edges.
For assembly meshing algorithms in release 14.0, Named Selection names for internal face zones are not interpreted. In cases where two enclosed voids share a face, the face zone is assigned type WALL automatically regardless of whether a Named Selection has been defined for the face. In these cases, the mesh generation cannot cross any boundary so you must define a virtual body with material point for each flow volume void in order for the volumes to be meshed. This is a change from release 13.0, in which Named Selection names matching FAN, RADIATOR, or POROUS-JUMP were interpreted as FAN, RADIATOR, and POROUS-JUMP face zone types respectively, so that when two enclosed voids shared such a face, mesh generation did not stop at the boundary.
The direct meshing feature has been renamed selective meshing. In support of this change, the Allow Direct Meshing option on the Options dialog box is now Allow Selective Meshing. Also see the Selective Meshing (formerly Direct Meshing) section above.
Virtual Cell and Virtual Split Edge objects no longer appear in the Tree Outline. In addition, suppression of virtual entities has been disabled. Refer to the Virtual Topology section above for related information.
The Virtual Topology object that appears in the Tree Outline represents all definitions of virtual face or virtual edge groups, and all definitions of virtual split edges, virtual split faces, and virtual hard vertices within a model. As described above, individual objects for these virtual entities do not appear in the Tree. If a geometry operation invalidates a virtual entity, refreshing the geometry no longer causes the Virtual Topology object in the Tree Outline to become underdefined. For example, if you include a fillet and one neighboring face in the creation of a virtual cell, but later remove the fillet from the CAD model and refresh the geometry, that individual virtual cell will become underdefined (as it only includes the one neighboring face), but it will not be deleted, and there will be no change in the Tree Outline. If in a later operation, the fillet is re-added to the CAD model and refreshed, the virtual cell will be restored. When a virtual entity becomes underdefined due to a geometry operation, a message is issued indicating that the last operation resulted in an incomplete virtual entity and advises you to check your model.
The Send to Solver option, which used to be available in the Mechanical application only, is now available in the Meshing application as well. When you are defining Named Selections, the Send to Solver option lets you control whether the selected Named Selection is passed to the solver. The default is Yes for Named Selections that you create, and No for Named Selections that are generated automatically by the Mesh worksheet.
Pre-inflation with patch conforming is now 20–30% faster.
When you export a mesh to ANSYS FLUENT mesh format, contact source and contact target entities in contact regions are now resolved as INTERFACE zones and mesh interfaces are created for the contact regions automatically. This eliminates the steps required in previous releases, which involved defining Named Selections for the contact regions in the Meshing application and then in ANSYS FLUENT, ensuring the INTERFACE zone type was assigned properly and creating a mesh interface for each contact region manually. For related information, also see the Resuming Databases from Previous Releases and FLUENT Export sections above.
The Smooth Transition option for the Inflation Option control is now supported when defining 2D local inflation.
The Auto Detect Contact On Attach option, which used to be available in the Options dialog box within the Mechanical application, has been moved. This option, which controls whether contact detection is computed upon geometry import, can now be accessed by selecting Tools> Options from the ANSYS Workbench main menu, and then selecting either the Mechanical or Meshing category as appropriate. The option is enabled by default in both applications.