Creating 2D-View Sections

This command is only available with the Automotive Body in White Templates product.

• generate GSD wireframe planar objects from the intersection of a 3D geometry with an intersection plane,
• represent these objects in a view plane which may be different from the intersection plane,
• use the tools from the Sketcher workbench to create additional 2D sketcher wireframe objects in the view plane,
• transfer geometries created in the Sketcher workbench in both view plane and intersection plane,
• easily apply corner and thickness operations to GSD geometries in the view plane,
• visualize and select filters associated to geometries generated in the sections context.

• Compute Corners and Thicknesses
• Edit 2D-View Sections
• Edit 2D-View Section Parameters
• Transfer Elements from the View Plane to the Section Plane
• Move 2D-View Section
• Define the Section as the In Work Object

Open the 2DViewSection1.CATPart document.

1. Click Insert 2D-View Section  in the Sections Management toolbar.
   The 2D-View Section Definition dialog box appears.

2. In the 2D-View plane box, select the visualization plane or planar surface.
   Here we selected the xy plane.

3. In the Intersection plane box, select the cutting plane or planar surface.
   Note: Both planes may be identical, parallel or unrelated. You can create a 2D-view section with only these two inputs, however the created 2D view section will be very similar to a geometrical set or ordered geometrical set.
   Here we selected the zx plane.

4. Select whether you want to show only the 2D view (2D-View only) or the 2D view and the 3D intersections
   (2D-View + intersection) in both view and intersection planes.
   Here we selected 2D-View + intersection.

5. In the Content of list, select where you want to put the selected geometrical elements: either to a new group if none exists already (as in our scenario) or an existing group (Group.x).

6. In the Group Color list, select the color of wireframe objects for the current group.
   By default, the blue color is used.

   The geometries selected in the Cut elements in group area may be gathered in different groups. Every group has its own color to distinguish the generated wireframe objects created by intersecting geometries of every  group with the intersection plane. Intersection and visualization planes must be common to all the groups.

7. In the Cut elements in group area, select the geometrical elements of your choices (curves, surfaces, volumes or solids) to be inserted in the current group.
   
   Note: You can select the element and click Remove to delete it from the list.
   A rectangular boundary appears on the plane chosen as the cutting plane along with manipulators.
   

   The result of the section of the selected geometrical elements with the section plane may be a set of non-connex wireframe elements. A warning message appears each time a modification of the intersected geometry set results in a non-connex set of intersection wireframe elements.

8. Modify the size of this rectangle using the manipulators.
   The rectangle area is frozen, i.e. automatic dimensioning does not work anymore when adding or removing
   elements from the intersected geometries.
   

9. Right-click any of the manipulators of the cutting plane and select the Reset to default position command.
   The delimiting rectangle is reset to its initial position and the intersecting element is the bounded cutting surface originally selected.

   This contextual menu is only available after one of the manipulators has been moved.

10. From the Cutting Area Dimensioning tab, select a point in the Reference Point box and define width and height to specify the dimensions of cutting area.
    Note: If the reference point lies outside the cutting plane, then it is projected on the cutting plane.

11. Select EdgeFillet.2 in the Cut elements in group, select New Group among the possible destinations from the combo list and click Move to.

12. In the Group Color list, select another color for this new group.
    Here, we selected the green color.

13. Use the 2D view manipulators to move the 2D-view section for a better visibility.
    

    Click Display only Selected Elements to temporarily hide all elements from the 3D area except selected ones, until the view is restored by deactivating the view filter. Click Set Pickable only Selected Elements to temporarily see all elements as unpickable in the 3D area except selected ones, until the pickable mode is restored by deactivating the selection filter.

14. Click OK to create the 2D-view section.
    
    It is created in the current In Work Object. Grouping intersected geometries also has an influence on the structure of specification tree under the 2D-view section feature. Every group generates a node in the specification tree directly under the 2D-view section feature:
    

15. Click Filter the Section's components to hide all the nodes of the specification tree under the Group node:
    

Compute Corners and Thicknesses

1. Double-click the  2D-View Section  in the specification tree to edit it.
   The 2D-View Section Definition dialog box appears.

2. Select the 2D-View only option.

3. Select Group.2 containing EdgeFillet.2.

4. In the Default corner radius box, enter the corner radius value.
   By default, the value is 5mm.

5. Click Compute corners to manually apply the corner operation on the sharp vertices contained in the Section join node.
   The default corner radius defined in the dialog box is used for all created corners. You can independently modify each corner radius by double-clicking the radius value in the 3D area and set a different value.

   When a corner generated using Compute corners is absorbed by another corner operation, the 3D display remains, allowing you to manually modify it. A corner value of 0 preserves the sharp edge as it is. Click Remove corners to remove the corners which are generated by Compute corners. If you change the corner radius value, corners must first be removed to be recomputed with the modified value. If the corner on vertex is not available, corner on elements will be created. Specifications for corner on element on any particular sharp vertex to be cornerized will be as follows: If none of its adjacent sharp vertices are already cornerized: Distance between the vertex to be cornerized and the adjacent sharp vertices on both sides are computed. The vertex with minimum distance from vertex to be cornerized is taken as Element 1 and the edge on the other side of vertex to be cornerized is taken as Element 2. If one of the adjacent sharp vertices is already cornerized: The adjacent sharp vertex is taken as Element 1 and the adjacent Edge+Corner is taken as Element 2. If no solution with these inputs, C0 solution will be computed. The adjacent non sharp vertex is taken as Element 1 and the edge between current vertex and adjacent sharp vertex is taken as element 2. If both the adjacent sharp vertices are already cornerized: Distance between the vertex to be cornerized and the end vertices of corners on adjacent sides are computed. The Edge+Corner on the side of farther vertex is taken as Element 2. The Vertex between the adjacent Edge and corner, on the nearer side is taken as Element 1.

6. Select the Automatically compute undefined corners check box to apply a new corner operation on undetermined vertices which may remain after the compute corners operation.
   Undetermined vertices are sharp vertices introduced after being created using Compute corners.

   This check box does not affect sharp edges which result from setting their radius to 0 during the corner computation.

   When this option is used without having created the corners with Compute corners, it systematically applies the default corner radius on all sharp vertices:
   

7. Select the Thickness check box and enter a value to compute the thickness.
   The default value for the thickness is 1mm. Here we selected 5mm.
   
   This option can be applied on the result of a corner operation or on the elements of the Section join group if no corner operation has been defined. It is composed of a parallel curve followed by a closing lines operation.
   

   The closing lines operation is performed when the characteristics of the body representing a 2D-view thickness feature match with the characteristics of the body representing a section join feature. For example, the closing line operation is possible when the number of domains in input body and output body are same.

   You can click the Invert thickness orientation button in the dialog box or the red arrow in the 3D area to inverse the orientation of the parallel curve:

   The thickness and corner operations use the visualization plane (or planar surface) as the support. In the case of a bounded planar surface used as visualization plane, it is necessary that all elements on which the corner and thickness operations are performed lie within the visualization planar surface. If this is not the case, a warning message is issued and the operation fails.

8. Optionally, you can select the Ope/Close Extremitnies check box to open the thickness at either extremities.

   If you have cleared the Thickness check box, the Open/Close Extremities check box remains disabled. By default, the Open/Close Extremities check box is cleared.   Depending on the position of the cutting area with respect to the cutting element, the command gives following results: Cutting area lies inside the limits of the cutting element: a. If the Open/Close Extremities check box is selected  b. If the Open/Close Extremities check box is cleared      Result: Thickness at both the extremities is open.  Result: Thickness at both the extremities is closed.      Cutting area lies outside the limits of the cutting element: a. If the Open/Close Extremities check box is selected   b. If the Open/Close Extremities check box is cleared       Result: Thickness at the right extremity is open, while at the left it is closed, due to cutting area exceeding the cutting element.  Result: Thickness at both the extremities is closed.

9. Optionally, click the Vertices list tab.
   The Vertices list tab displays all the vertices at the sharp corners of the 2D-view section.
   The vertices are sorted as follows:

   If the curve contains only convex or concave corners, the vertices are sorted in descending order of their radii. If the curve contains convex and concave corners or sections with consecutive convex or concave corners, all vertices of the convex corners are listed first followed by the vertices of all concave corners unless Thickness option is used. If Thickness is defined and the direction is reversed using Reverse thickness direction, the convex - concave order is reversed, that is in this case the vertices of concave corners are computed first. By default, all consecutive vertices of the same type are listed in descending order of their radii. However, this is no longer valid if the order is changed manually using the Move up or Move down button. Note: The list is updated dynamically when changing a radius provided that the vertices order was not modified using a manipulator in 3D or the Move Up and Move Down buttons in the dialog box.

10. Optionally, you can change the order in which the corners are computed by reordering the vertices. Select a vertex and click Move Up or Move Down to reorder the list.

    The vertex is highlighted in the 3D geometry area.

    The Vertices list tab displays the list of vertices in either of the following cases: You have selected the Automatically compute undefined corners check box in the Corners Management area. You have clicked Compute corners in the Corners Management area.

    In case of overlapping corners between two vertices, you can also swap the computation order of the corners concerned using the handle appearing in the work area between the corresponding vertices. In the Vertices list, the order will be updated automatically. If the locally changed order impacts the computation order of these vertices with adjacent overlapping vertices, the computation order of other overlapping vertices will be swapped until they match the arrow directions of existing handles.

11. Click OK to apply the corner and thickness operations to the 2D view section.
    The 2D-view thickness node in the specification tree contains the result of the corner and thickness operations.
    

Edit 2D-View Sections

• Use the contextual command on the 2D-view section to create a temporary sketch under the 2D-view section then
  all the section's group in the specification tree.
• Use the contextual command on the 2D-view section group to create a temporary sketch under the specific group, just before the Section join node. This means that wireframe elements created in the group will be used for further corner and thickness operations. This is not the case for elements created directly under the 2D-view section feature.

1. Right-click the 2D-View Section.1 in the specification tree and select the 2D view section.1 object > Edit Section command.
   The Sketcher workbench opens.

2. Create a rectangle for instance.
   

3. Click to exit the Sketcher workbench.
   The curve appears in the 3D area and added to the specification tree:
   
   Once you have created a sketch containing no constraints and exited the Sketcher workbench, elements of this sketch are transferred to equivalent GSD wireframe features and the sketch is deleted. The generated features replace the temporary sketch in the specification tree.

If the created sketch contains constraints, a warning message appears when exiting the Sketcher workbench. You have two choices: If the constraints can be lost, sketcher elements are converted into GSD features as described above. If the constraints must be kept, sketcher elements are not replaced by GSD features and the sketch remains at its place in the specification tree when exiting the Sketcher workbench.

Edit 2D-View Section Parameters

1. Right-click the 2D-View Section.1 in the specification tree and select the 2D view section.1 object > Edit Parameters.
   The parameters of the element are displayed.

2. Double-click any value in the 3D area.
   The Parameters dialog box appears.

3. In the Value box, enter a value or use the arrows to change the value.

4. Click OK.

5. Select Edit > Update to update the new parameter.
   The new parameter is applied.

   To display parameters permanently, select the Parameters of features and constraints check box from Tools > Options > Infrastructure > Part Infrastructure > Display area.

Transfer Elements from the View Plane to the Section Plane

1. Double-click the 2D-view section in the specification tree to edit it.
   The 2D-View Section Definition dialog box appears.

2. Select the 2DView > Section transfer tab.
   The elements than can be transferred are displayed in the right-column list:
   
   This list contains all the features contained in the 2D-view section node in the specification tree (GSD or sketcher, within groups or not, wireframe or not, contained in view plane or not).

3. Choose the element to transfer (here Curve.1) from the right-column list and click the green arrow.
   It is transferred to the left-column list: In the Value box, enter a value or use the arrows to change the value.
   

   You can also choose the element to transfer by selecting the element from 3D geometry. If element is in right-column list then it is transferred to the left-column list and vice-versa. The elements created by editing the section group are identified with an asterisk and are strictly contained in the view plane.

4. Select the group where to transfer the elements in the list.

5. Click OK.
   The element is added to the specification tree under the 2D-view section node as Section transformation.x and displayed in the 3D area:
   

Move 2D-View Section

1. Double-click the 2D-view section in the specification tree to edit it.
   The 2D-View Section Definition dialog box appears.

2. Select the 2D Section Move tab.
   
   
   This list contains all the features contained in the 2D-view section node in the specification tree (GSD or sketcher, within groups or not, wireframe or not, contained in view plane or not).

3. In the Incremental value aligned with list, select the direction:

   • View Plane: allows you to move the 2D-view section elements along the visualization plane.
     By default, this option is selected.
     Note: If you are working with a 3D support, you can move the 2D-view section along the 3D grid.
     The default primary spacing of Work On Support 3D grid is 100mm for each direction.

   • Intersection Cut Direction: allows you to move the 2D-view section along the direction normal to cutting plane.
     You can switch from Intersection Cut Direction to View Plane and vice-versa by double-clicking the manipulators.

4. In the ViewPlane H and ViewPlane V boxes, specify the values to define the location of manipulators.

5. Click OK.
   The 2D-view section is moved.

Define the Section as the In Work Object

1. Click Define a Section as the In Work Object in the Sections Management toolbar.
   The Define In Work Section dialog box appears.
   

2. Click Reframe on to reframe the view and display the section elements contained in a selected group.
   For further information, refer to Infrastructure User's Guide: Viewing Objects: Reframing On an Object.

3. Click Normal View  to display the cutting plane parallel to the screen.
   For further information, refer to Infrastructure User's Guide: Viewing Objects: Snapping the Viewpoint.

4. Click Show only current section to hide all the elements from the 3D area except those of the selected section group.
   For further information, refer to Part Design User's Guide: Associating Bodies: About Boolean Operations.

5. Click Set no keep mode   to change the mode to No Keep and not retain an element on which you are performing an operation.
   For further information, refer to Keeping the Initial Element.

6. Click Lock view point  to lock or unlock the orientation of the viewing vector. If it is activated, the viewing vector is locked perpendicularly to the section plane.
   For further information, refer to Managing the Background Visualization.

7. Click OK to apply the current options.