Querying the model in the Visualization module

Locate the Query dialog box.

From the main menu bar, select ToolsQuery or click the tool in the Query toolbar.

The Query dialog box appears.

To obtain information on a particular node, do the following:

1. Select Node from the General Queries field of the Query dialog box.

   Abaqus/CAE displays a prompt in the prompt area.

2. Select a node from the viewport.

   The undeformed and deformed X-, Y-, and Z-coordinates of that node appear in the message area, along with the node's displacement. The same information that appears in the message area is also written to the replay file.

   Note:

   To resize the message area, drag the top edge; to see information that has scrolled out of the message area, use the scroll bar on the right side.

To obtain information on the distance between two nodes, do the following:

1. Select Distance from the General Queries field of the Query dialog box.

   Abaqus/CAE displays a prompt in the prompt area.

2. Select two nodes from the viewport.

   The following information appears in the message area:

   • The undeformed and deformed X-, Y-, and Z-coordinates of each node, along with the node's displacement.

   • The absolute undeformed and deformed distances between the nodes.

   • The X-, Y-, and Z-components of the undeformed and deformed vector between the two nodes.

   • The absolute relative displacement between the nodes.

   • The X-, Y-, and Z-components of the relative displacement between the two nodes.

To obtain information on the angle formed by three nodes, do the following:

1. Select Angle from the General Queries field of the Query dialog box.

   Abaqus/CAE displays a prompt in the prompt area.

2. Select three nodes from the viewport. The second node that you select is the vertex of the angle.

   The following information appears in the message area:

   • The undeformed and deformed X-, Y-, and Z-coordinates of each node, along with the node's displacement.

   • The absolute undeformed and deformed angle between the nodes.

To obtain information on a particular element in an output database, do the following:

1. Select Element from the General Queries field of the Query dialog box.

   Abaqus/CAE displays a prompt in the prompt area.

2. Select an element from the viewport.

   The following information appears in the message area:

   • The element's label, element type, material, and section.

   • The labels of connecting elements.

   • The current field output variables at the integration point locations.

To obtain general information on the mesh, select Mesh from the General Queries field of the Query dialog box.

The following information appears in the message area:

• The name of the current output database.

• The number of nodes.

• The number of elements.

• The element types.

To obtain general information on the mass properties in an output database, do the following:

1. Select Mass properties from the General Queries field of the Query dialog box.

   Abaqus/CAE displays a prompt in the prompt area and displays the mass properties for the default selection method, All elements, in the message area.

   Note:

   If you have already used the Mass properties query in the current session and chose a different selection method, Abaqus/CAE displays in the prompt area the last selection method that you used but does not generate new results in the message area.

2. Choose one of the following selection methods from the list in the prompt area:

   • All elements

   • Select elements from viewport

   • Part instances

   • Element sets

   • Sections

   • Materials

   • Element types

   • Display groups

   Abaqus/CAE displays additional selection fields in the prompt area, depending on the selection method that you chose.

3. Complete your selection as follows:

   • If you chose Select elements from viewport in the previous step, make selections from the viewport (for more information, see Selecting objects within the viewport”). You can select a part instance in the prompt area and enter a single element number to get mass information for that element.

   • For the remaining selection methods, select the part instance, element set, section, material, element type, or display group name from the list in the prompt area, or make selections from the viewport.

   When you select an object from the prompt area or when you click Done to complete a viewport selection, Abaqus/CAE displays the mass properties for your selection in the message area.

4. If any items in your selection have poorly defined density or thickness, click Options in the prompt area to display the Mass Properties Query Options dialog box and specify a value to be substituted by Abaqus/CAE for the undefined quantity.

   Click OK in the dialog box to save your entries and close the dialog, or click Reset to return to the previous settings.

Abaqus/CAE displays the mass properties in the message area for the items you selected. The following properties are available:

• Surface area (for shell elements only)

• Area centroid

• Volume

• Volume centroid

• Mass

• Center of mass

• Moments of inertia about the center of mass or about a specified point

To obtain the surface normal components, do the following:

1. Select Element face normal from the General Queries field of the Query dialog box.

   Abaqus/CAE displays a prompt in the prompt area.

2. Select an element face in the viewport, and click Done.

   The surface normal components in the global Cartesian coordinate system of the element face appear in the message area.

The surface normal components will differ if you query the same element face on the undeformed shape and the deformed shape.

Close the Query dialog box when you have finished requesting information.