Creating a Front View

You can create a front view of the 3D part using a reference plane.

This task shows you how to:

Before you begin: Open a 3D part representation and create a new drawing with an empty sheet.
See Also
About View Creation

Create a Front View

You can create the front view either from a part or from the sub-part of a product, using a reference plane.

  1. From the View Layout section of the action bar, click Front View .
  2. To define the reference plane, select either of the following:
    • A plane of the 3D part or a plane surface.
      Important: If you select a plane surface, the reference orientation is the external normal of the planar surface.
    • Two edges: These edges correspond to both axes defining the reference plane according to which the front view is generated. The first edge determines the horizontal axis.
    • A point and an edge or vice versa, two points and an edge, or three points: you can thus define a plane.

    View orientation handle appears that lets you redefine the projection plane before generating the view. For more information, see Define the view orientation during view creation.



  3. Click in the drawing to generate the view.



    Tip: By default, the axis and centerlines are generated. You can also view hidden lines, threads, fillets, and project 3D points. To configure the view properties, right-click the frame of the view and select Properties. In the Properties dialog box, under the View tab, select the required options.

Define the View Orientation During View Creation

When creating a view, you can redefine the orientation of its reference plane using the view orientation handle.

This is the case when generating a front view, an isometric view or when generating views using the wizard.

Open a 3D part representation 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. Right-click the green knob and select the required 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.

Important: 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, see Modifying a View Projection Plane.

Create a Front View with a Local Axis System

This functionality lets you consider a local axis system when creating a view. Thus the origin of the generated view is the projection of the origin of the local axis system selected in the view plane.





  1. Click Front View .
  2. In the part tree, select the local axis system, Axis System.1.
    Important: Remember that you have to select the axis system in the tree and not in the 3D part. Otherwise it would be like selecting a line in the 3D area instead of the axis system.
  3. Select one plane of the 3D part or a plane surface, to define the reference plane.



  4. Click in the drawing to create the view. The part local axis system appears in the view.



    Important: When creating views with a local axis system, only the origin of the axis system is taken into account and respected in the generated view. The orientation is not taken into account.

Create a Front View from Specific Sub-bodies/Sub-products

You can multiselect specific sub-products in a product or several sub-bodies in a part to create front views displaying the selected elements only. These multiselected 3D elements are previewed and then used as reference planes for generating several front views.

Open a 3D product.

  1. Click Front View .
  2. Select one body, or press Ctrl + multiselect the required elements in the tree.



  3. In the 3D area, point to the geometry to choose a projection plane. As you go over the geometry with the pointer, the oriented preview automatically appears on the work area.



    Important: Be careful once you multiselect bodies or sub-products, and go further into the procedure, you cannot select or de-select any more bodies or sub-products.
    • As you highlight a 3D element (going over it with the cursor), you can preview and then select the plane corresponding to this highlighted element.
    • As you highlight and select one or more elements defining the final plane, you can preview and assign a given orientation to this final plane.
    • Once you defined the plane, you can preview the front view within the 3D representation.

    Note that once an element is selected, that element becomes gray colored. In addition, you can only work in one 3D document. If you try to select another document, the Front View command closes.

  4. When the oriented preview corresponds to the projection plane you want, click the plane to validate.

    The front view is previewed. At this point, you can still modify its orientation:



  5. Click in the drawing to generate the view.



Create a Front View Using the Selection Sets

Selection sets let you gain in productivity, particularly in the case of large assemblies, when generating several views with numerous common features. You can select and store these features once and reuse the selection set whenever required without having to select the features again.

Open a 3D product.

  1. Before you start creating views from selection sets, you first need to create one or more selection sets for this product. For more information, see Using Selection Sets. For example, create a selection set to store product screws.
  2. Click Front View .
  3. In the tree, activate the 3D shape representation.
  4. From the Tools section of the action bar, click Selection Sets... .
  5. In the Selection Sets Selection dialog box, select a selection set and click Select.
    The selection set items are highlighted in the 3D area and in the tree.

    For more information, see Using Selection Sets.

    Important: After selecting a selection set, press Ctrl to select additional sub-bodies or sub-products.
  6. In the 3D area, point at the geometry to select a projection plane.
    As you move the cursor over the geometry, the oriented preview appears.



  7. When the oriented preview corresponds to the projection plane you want, click the plane to validate.

    The front view is previewed. At this point, you can still modify its orientation:



  8. Click in the drawing to generate the view.



    Notes:
    • You can also use selection sets when creating isometric views.
    • You can also use selection sets to select the sub-bodies or sub-products from which you want to generate the front view.
    • Views created from selection sets are not associative with the selection sets themselves: if you modify a selection set after having created a view from it, the view does not need an update. And if you update the view, its definition does not change. You have to create the view again so that your modifications are taken into account.