Before You Begin

  Before you start creating views, this section provides you with information on the following topics:
Views as discussed in this section are created on a pre-defined sheet, and should not be confused with working views and background views, which are components of the sheet. For more information on these, refer to Sheets.
 

What is the active view?

The active view is the view from which other views will be generated. This is also the view in which all the modifications will be performed. For instance, all the 2D geometry and dress-up elements that will be added to the draft views to be created.
Open the GenDrafting_part.CATDrawing document.
View frames can be of three different colors, depending on the view status:
  • The active view has a red frame and it is is underlined in the Drafting specification tree.
  • Non-active views have blue frames.
  • During view creation, the view to be created has a green frame until you click at the desired view location to validate the creation.

In the Drafting specification tree, specific icons are used to represent the view type (Front view, Projection view, Isometric view, etc). Refer to CATDrawing Specification Tree Icons for more information.

To activate a view, you can either:

  • double-click the frame of the view.
  • or right-click the view and select Activate View.

Axes are taken into account on active views. As a result, the frame of an active view will adapt to the elements included in this view.
 

Defining the view orientation during view creation
When creating a view, you can redefine the orientation of its reference plane using the available knob. This is the case when generating a front view, an isometric view or when generating views using the wizard.
Open the GenDrafting_part.CATPart document and start creating a front view.

  1. Click the right or left arrow to visualize the right or left side, respectively.

  2. Click the bottom arrow to visualize the bottom side.

  3. Click the counterclockwise arrow to rotate the reference plane.

  4. Drag the green knob to redefine the rotating angle. The default increment value is 30 degrees.

  5. You can modify the increment value using the contextual menu which is available for the green knob. To do this, right-click the knob and select the desired option:

    • Free hand rotation: Lets you rotate the knob in a free manner using the mouse, instead of snapping it to a given increment.

    • Incremental hand rotation: Snaps the rotation to a given increment (from 30 to 30 degrees, between zero and 330). This is the default value.

    • Set increment...: Displays the Increment Setting dialog box. Enter the required value in the Increment value field. For example, type 5 deg (for 5 degrees) and click OK.

    • Set current angle to:

      • 0 deg: Sets the current angle value to 0 degrees.

      • 90 deg: Sets the current angle value to 90 degrees.

      • 180 deg: Sets the current angle value to 180 degrees.

      • 270 deg: Sets the current angle value to 270 degrees.

      • Set angle value...: Displays the Angle Setting dialog box. Enter the required value in the current angle (deg)  field. For example, type 30 and click OK.
Remember that there is no associativity between the selected plane or face in the 3D part and the projection plane of the generated views. Yet, you can modify the view projection plane if you change the 3D part orientation. For more information, refer to the Modifying the View Projection Plane section.
 

Generated geometry
  This paragraph deals with:

Dress-up settings of generated geometry

You can generate a number of geometry or dress-up elements, depending on the options you select in Tools > Options > Mechanical Design > Drafting > View tab.

For example, if you want the colors of a part to be automatically generated onto the views, check the Inherit 3D colors option. 

If the color of the part is white and the Inherit 3D colors option is checked, the generated views will be white and you may not be able to visualize them properly.
  • Note that threads are generated on the condition they are defined on 3D holes. 
  • To project sketches, you need to select the Project 3D wireframe option. However, note that a sketch cannot be projected if it is currently being edited in the Sketcher workbench. To project sketches, you need to exit the Sketcher workbench before launching the view creation.
 

Dress-up properties of generated geometry

You can change the properties of some geometry and dress-up elements after the view has been generated, provided you check the desired options in the Properties dialog box. To display it, choose Properties from the contextual menu and select the View tab.

In the following example, the graphical properties of two generated elements are overloaded. After an update of the part is performed, four items inherit the graphical properties of the 3D origin.

3D part

Modified generated item

Generated item with the same 3D origin

3D part

Modified generated item

 

Generated item with the same 3D origin

 
  • Note that if you modify the graphical properties (color, line type, line thickness, layer, no show) of generated geometry or dress-up elements, or delete these elements, such modifications are persistent at update, i.e. they are kept when updating the view later on. Also note that once you have overloaded the original graphical properties of a geometry or a dress-up element, you cannot reset it to its original properties. On the other hand, you can restore all deleted elements in a view using the Restore Deleted command.
  • Note that the persistency of this graphical dress-up/delete:
    • is only available in exact views. In views other than exact (CGR, Approximate or Raster), an update operation will reset the elements to their original properties.
    • creates additional specifications in the drawing, which increases the file size and requires additional computing during the update process.
  • As far as layers are concerned, when you select a layer and modify the graphical properties of some elements, the properties will be applied only when you update the selected layer.

    By default, the view and its elements are created in the layer None, as displayed in the Graphic Properties toolbar. Yet, if you modify your view and add elements, they will be created in the current layer, which can be layer 0, 1, 2 or any layer you select in the toolbar.

  • Each time a view is updated, generated geometry is deleted and recreated. As a result, generated geometry for which no layer is explicitly specified (which is set to the layer None), is placed into the current layer (that is, the layer which is selected in the Graphic Properties toolbar when the view is updated). Therefore, to avoid unexpected results, it is recommended to set the current layer to None before updating a view.
  • Since generated geometry is deleted and recreated each time the view is updated, when edited, the graphical properties of the geometry is stored according to its 3D origin. This way, the right properties are applied to each new geometry according to its 3D origin.
    Thus, once updated, generated geometry inherits the graphical properties corresponding to the 3D origin previously stored.
Overloaded graphical properties are not kept for the following generated items:
  • Generated shapes (hatching in sections and breakout views)
  • Edges corresponding to symbolic visualization of fillets
  • Edges representing limits of clipping, detail or broken views (this does not include the callout of detail which is not a generated element)
  • Bend limits in unfolded views of sheet metal parts
  • Annotations generated from 3D annotations or 3D application elements (structure, piping)
 

Definition of dress-up properties for generated geometry

The following table illustrates how the various dress-up properties of generated geometry are defined, depending on the view type.

 

View type

 
  • Front view
  • Unfolded view
  • View from 3D
  • Isometric view
  • Advanced front view
  • Projection view
  • Auxiliary view
  • Section view
  • Section cut
  • Detail view

Parameters

    
 
  • Hidden lines
  • Center lines
  • Axis lines
  • Threads
  • Fillets
  • 3D colors
     
 Properties defined via
Tools > Options > Mechanical Design > Drafting > View		 Properties generated in the view
 
  • 3D specifications
  • 3D points
  • 3D wireframe
  • Generation mode
 Properties defined via
Tools > Options > Mechanical Design > Drafting > View		 Properties defined via
Tools > Options > Mechanical Design > Drafting > View
 

Constraints
  Constraints detected when views are generated from the 3D do not appear on the drawing.
 

2D/3D associativity
  This paragraph deals with:

2D/3D associativity on views

A generative view results from specifications in a 3D document. This specification corresponds either to the whole document or to a feature in the document. This feature can be: 

  1. a .model document
  2. a part document (the whole document or still one or more bodies)
  3. a product document (the whole document or still one or more assemblies)
 

2D/3D associativity and view positioning

Generative views are positioned according to the center of gravity of the 3D part. If you modify a 3D part in such a way that the center of gravity of the part changes, then, when updating the view, the position of the view will be re-computed according to the new center of gravity of the part and will be modified accordingly. 

For more information on View Positioning properties, refer to the Generative Views Positioning Mode section in the Interactive Drafting User's Guide.

 

2D/3D associativity and update

Any modification applied to the specifications, before the generated views is/are updated, is detected. You can perform an update. You can update all views or a selection of views:

  • The Update icon is active in the Update toolbar when a sheet (or drawing) contains views that need to be updated (this can be all views in the sheet or some of them only). You can update all views in the active sheet by clicking this icon. 
  • An Update symbol appears in the specification tree for the views that need to be updated. You can update a selection of views by selecting and right-clicking the views you want to update and choosing Update Selection from the contextual menu. Only the items you select are updated. Update symbols remain in the specification tree for the items that have not been updated, so you always know which items are up-to-date and which are not.
  • Update symbols also appear in the specification tree to indicate drawings and sheets containing views that need to be updated. You can update all views in a given sheet (or in a selection of sheets), by selecting and right-clicking the sheets and then choosing Update Selection. You can also use the same method for a drawing: this will update all sheets (and therefore all views) in the drawing. 
  • During an update process, a dialog box is displayed to show the progress of the update. 
    When the update involves several views, a Cancel button is available in this dialog box. This allows you to interrupt the update. The view that is being processed at the time you click this button will be updated (i.e. the update of the current view will finish), and then the update will stop. The subsequent views will not be updated.
 

2D/3D associativity after updating

Use the following commands to update views:

  • Click Update to update all views in the active sheet.
  • Select and right-click the views you want to update and choose Update Selection from the contextual menu to update a selection of views. 
  • Type C:Force Update in the Power Input field to update the drawing in accordance with the 3D. Be careful when doing this, as you may lose manual modifications applied to the drawing.

During view update, the following operations are performed:

  • associative section/auxiliary view profiles are re-computed
  • the geometry is re-generated
  • any annotation/dimension/dress up element linked to the generated geometry is re-computed
  • in the case of elements (one or more) that have been graphically modified or deleted, these modifications/deletions are preserved, on the condition the view was up-to-date when you deleted or modified it.

 
  • Note that you can restore deleted elements at any time by selecting the Restore Deleted option from the contextual menu and then updating the view. You can either use the Update icon if you modified the 3D part, or key in C:Force Update if you did not modify the 3D part.
  • If you delete a generated item and subsequently perform an update, all items that have the same 3D origin as the deleted item will not be generated. Likewise, if you transfer a generated item to No Show and subsequently perform an update, all items that have the same 3D origin as the item in No Show will be transferred to No Show.
 

2D/3D associativity on generated dimensions

Generated dimensions are associative with the 3D part constraints on the condition you checked the Generation dimensions when updating the sheet option from the Options dialog box (Tools > Options > Mechanical Design > Drafting  > Generation tab).

Note that these dimensions will be re-generated in accordance with the other options checked/un-checked in the Options dialog box.

 

2D/3D associativity and color

When you refresh a generated view you have modified, the colors are re-generated with the geometrical information from the part, and you might obtain unexpected results.

As an example, if you create this part...
 
   
  ...and then modify an element in the following generated view, such as the color of line "a" as in this example:
 
   
  ...then, when updating the generated view, lines a and b will be red:
 
   
  The reason is that the view is refreshed with the part information and a and b lines are considered as the intersection of two planes and not as two different elements of the generative view. 

Note that modifications performed on the graphical properties (color, line type, line thickness) of a generated geometrical element (as is the case in our example above) are associative, i.e. such modifications are kept when updating the view later on. Also note that once you have overloaded the original properties of an element, you cannot reset it to its original properties.

 

2D/3D associativity and operations performed on parts

Operations performed on parts, and that can be saved with the part itself (such as Show/No Show, Delete, Deactivate, Visualization Filters, etc.), are taken into account when generating the view. For example, if you delete a part body, this body will not be represented on the generated view. If you then restore this part body, you can update the corresponding views; this time, the body will be represented on the generated view.

There is an exception to this rule: when generating views in exact mode, Define in Work Object is not taken into account. However, since this command is taken into account when generating views in CGR, Approximate and Raster modes, it is recommended to be wary of using Define in Work Object for such view types.
 

2D/3D associativity and part infrastructure settings

Settings used for a given part, and that only have an impact on the current session but cannot be saved with the part itself (such as the Display in Geometry Area category of settings available via Tools > Options > Infrastructure > Part Infrastructure > Display), have no impact on how or whether the part will be represented on the generated view.

 

2D/3D associativity for approximate/CGR/raster views

The up-to-date mechanism of Approximate, CGR or Raster views from CATProduct documents (in current file environment), is based on the document's inner date.
This mechanism is faster and less memory consuming than the current Exact view mode up-to-date mechanism.
Due to this mechanism, if a CATPart or cgr or .model file is moved using Save management... or Save As... , then this will modify the last modification date, thus the views will be not-up-to-date.

For more information, refer to Advantages and restrictions common to CGR and Approximate.
 

3D Elements Generated in Views

3D elements are handled differently depending on the view mode you are generating:

Exact mode

  • All CATPart elements are supported.
  • Exact Solid, Faces and Skin elements from .model documents are supported, as well as space ditto (with similar content of associated detail).

CGR and raster mode

  • All CATPart elements except wireframe and 3D points are supported.
  • All elements from .model documents are supported.
  • External MultiCAD components are supported.
 

Dress-up generated in views

You can automatically create center lines, axis lines and threads according to the criteria described below. (Note that this criteria also apply to isometric views.)
 

Center lines

  • The view plane must be perpendicular to the rotation face axis.
  • The representation of the rotation face in the view must exceed 180 degrees.
 

Axis lines

  • The view plane must be parallel to the rotation face axis.
  • Rotation faces made out of fillets are not taken into account when generating axis lines.
 

Threads (represented from the front and rear)

  • The view plane must be perpendicular to the rotation face axis.
  • The face should be a threaded hole or a thread.
  • The representation of the rotation face in the view must exceed 180 degrees.
Threads will be represented from the front AND from the rear, whether or not the hole is threaded along its whole depth.
 

Threads (represented from the side)

  • The view plane must be parallel to the rotation face axis.
  • The face should be a threaded hole or a thread.
 

Callout Representation

You can specify that the size of callout elements should not be dependent on the view scale. You have two ways of doing this:

  • After callout creation, right-click on the callout, select Properties in the contextual menu and check Size not dependent on view scale on the Callout tab.
  • Or before callout creation, in Tools > Options > Mechanical Design > Drafting > Layout tab, check the Size not dependent on view scale option. This option will apply to newly created callouts, i.e. selecting this option will not have any impact on existing callouts.

    Note that this option only applies to drawings created with versions prior to V5 R11 (i.e. versions up to V5 R10).
 

Warm Start and views

In Tools > Options > General > General tab, you can specify that you want a backup to be automatically performed on your data, which would allow you to recover your data (partially or entirely) should the application crash.

If you selected the Incremental backup option (which stores all open documents in a temporary directory, and all modifications to the document are logged in a log file), Generative Drafting views may be restored, if necessary, after a crash. However, you need to be aware of the following facts:

  • When recovering a drawing after a crash, all views which need to be restored in the drawing are automatically updated. For this reason, the drawing will contain up-to-date views, even though it was not necessarily the case prior to the crash.
  • Due to this automatic update operation, any view which was locked prior to the crash and which needs to be restored will be empty after the restore operation (remember that locking a view means that you cannot update it).

For more information regarding these options, refer to General in the Infrastructure User's Guide.
 

View generation modes

You can create views using several generation modes:

  • Exact
  • Raster
  • CGR
  • Approximate

For a detailed description of each view generation mode (including the advantages and restrictions pertaining to each one), refer to About the View Generation Modes.