Obtaining general information about the model

You can use the Query toolset to obtain general information about your model including point/node coordinates; element labels, topology, and nodal connectivity; and mass properties.

Related Topics
Using the Query toolset to query the model
Understanding the role of the Query toolset
Customizing mesh display

To obtain general information about your model, select ToolsQuery from the main menu bar or click the tool in the Query toolbar. For tools that require meshes to be available, you can use the ViewPart Display Options or ViewAssembly Display Options menu items to display the native mesh. Select one of the following from the General Queries field in the Query dialog box that appears:

Point/Node

Select a point or node. Abaqus/CAE displays the X-, Y-, and Z-coordinates of the point.

Distance

Select two points or nodes. In the Part, Property, and Mesh modules you can select points, edges, or faces. Abaqus/CAE displays the following:

  • The X-, Y-, and Z-coordinates of each entity.

  • The absolute distance between the entities.

  • The X-, Y-, and Z-components of the vector between the two entities.

The distance between non-point entities is always the shortest distance between two points within the entities.

Angle

Select two edges or two faces or select an edge and a face. Abaqus/CAE displays one of the following, depending on your selection:

  • The angle between the two edges.

  • The angle between the normals to the face.

  • The angle between the edge and the normal to the face.

When you select an edge, Abaqus/CAE displays an arrow along the edge. When you select a face, Abaqus/CAE displays an arrow on the face that indicates the normal to the face. The angle is defined as the angle that must be swept by one edge or face to align the two arrows. The angle is always positive and less than or equal to 180°.

Feature

Click mouse button 3 on a feature in the Model Tree, and select Query from the menu that appears. Abaqus/CAE displays the following information about the selected feature:

  • Name and description; for example, solid extrude.

  • Status, if the feature is suppressed or if it failed to regenerate.

  • The name of its parent, if any.

  • The names of its children, if any.

  • The value of any parameters that define the feature.

Shell element normals

  • For parts with shell regions, Abaqus/CAE displays the part or assembly using the shaded render style. The side of the shell where the surface normal coincides with the shell normal (top face) is colored brown; the opposite side (bottom face) is colored purple.

  • For axisymmetric parts with wire regions, Abaqus/CAE displays cyan arrows indicating the directions of the normals.

You can use the Assign menu in the Property module or the MeshOrientationNormal menu in the Mesh module to reverse the normal directions. For more information, see Assigning shell/membrane normal directions.

Beam element tangents

Abaqus/CAE displays cyan arrows indicating the directions of the beam tangents.

You can use the Assign menu in the Property module or the MeshOrientationNormal menu in the Mesh module to reverse the tangent directions. For more information, see Assigning beam/truss tangent directions.

Mesh stack orientation

You can use this tool to query only hexahedral, wedge, and quadrilateral elements because these are the only elements that can be stacked to form a continuum shell, cohesive, cylindrical, or gasket mesh. For hexahedral and wedge elements, Abaqus/CAE colors the top face brown and the bottom face purple. Similarly, arrows indicate the orientation of quadrilateral elements. In addition, Abaqus/CAE highlights any element faces and edges that have inconsistent orientation. For more information, see Creating a model with cohesive elements using geometry and mesh tools, Continuum shells, Swept meshing of cylindrical solids, and Gaskets.

If the region is a native Abaqus mesh, you can change the mesh stack orientation by changing the direction of the sweep path. For solid regions, you can assign a new mesh stack orientation independent of the sweep path. If the region is an orphan mesh, you can use the Edit Mesh toolset to change the mesh stack orientation. For more information, see Specifying the sweep path, Applying a mesh stack orientation, and Orienting the stack direction, respectively.

Note:

The query results do not account for changes made in the mesh stack orientation while defining a solid composite layup or a composite shell layup in the Property module.

Mesh

For an assembly, part or part instance, geometric region, or element, Abaqus/CAE displays the following:

  • The total number of nodes and elements in the selected area

  • The number of elements for each element shape

By default, Abaqus/CAE displays mesh information in the message area, but you can display this information in tabular format in the Mesh statistics dialog box by toggling on Display detailed report in the prompt area. The Mesh statistics dialog box also enables you to display mesh information by part instance or by element type.

Element

  • Element label

  • Element topology; for example, linear hexahedron

  • Abaqus element name; for example, C3D8I

  • Nodal connectivity.

Mesh gaps/intersections

Select the mesh parts or part instances, and enter the maximum distance between a node and an element face. Abaqus/CAE highlights element edges that intersect the boundary faces and element edges that are closer than the specified distance to boundary faces.

Mass properties

This query displays information about the surface area, area centroid, volume, volume centroid, mass, center of mass, and moments of inertia about the center of mass or about a specified point for your selection. For more information, see Querying mass properties.

Geometry diagnostics

  • Invalid, imprecise, or small geometry

  • Topology

Sets
Select a set from the list of sets provided. If desired, toggle on Highlight set to highlight the set in the viewport. Click Done.

Abaqus/CAE displays the following information about the selected set in the message area, depending on your selection:

  • Geometry set: components, index, instance name, set name, set type, total number of components
  • Element set: element label, element type, connectivity, instance name, set name, set type, total number of elements
  • Node set: node label, nodal coordinates, elements sharing the node, instance name, set name, set type, total number of nodes

Surfaces
Select a surface from the list of surfaces provided. If desired, toggle on Highlight surface to highlight the surface in the viewport. Click Done.

Abaqus/CAE displays the following information about the selected surface in the message area, depending on your selection:

  • Geometry surface: index, side, instance name, surface name, surface type, total number of surfaces
  • Mesh surface: element label, element type, connectivity, side, instance name, surface name, surface type, total number of faces

Geometry face normal
Select a face. For a curved surface, you are prompted to select the point or enter the X-, Y-, and Z-coordinates of the point at which to evaluate the normal. You can select reference points, attachment points, or vertices. The surface normal components in the global Cartesian coordinate system appear in the message area.
Element face normal
Select an element. The surface normal components in the global Cartesian coordinate system appear in the message area.