Creating a Front View

This task will show you how to create a front view either from a part or from the sub-part of a product. You will use a reference plane.

A front view is a projection view obtained by drawing perpendiculars from all points on the edges of the part to the plane of projection. The plane of projection upon which the front view is projected is called the frontal plane.

In a Product Structure context, if you create a front view from a scene of a product, you can directly select the Scene object in the specification tree. You do not necessarily need to select the Product and sub-products any more.

Choose a scenario:

	creating a front view,
	creating an advanced front view,
	creating front view with local axis system,
	multi-Selecting Sub-Bodies/Sub-Products,
	projecting points from 3D.

Before You Begin, make sure you customize the following settings:

Grid:
De-activate the Grid icon from the Tools toolbar (bottom right).

View names and scaling factors:
Go to Tools->Options ->Mechanical Design -> Draftingoption (Layout tab) and check the View name and Scaling factor options.

3D colors inheritance
Go to Tools->Options->Mechanical Design->Drafting option (Generation tab) and un-check the 3D colors inheritance option.

Creating a front view

Open the GenDrafting_part.CATPart document. Define a new drawing sheet.

1. Click the Front View icon

from the Views toolbar.

2. Select one plane of the 3D part or a plane surface, to define the reference plane.
Blue arrows appear.

If you select a plane surface, the reference orientation will be the external normal of the planar surface.

To define the reference plane, you can also select:

	Two edges These edges correspond to both axes defining the reference plane according to which the front view will be generated. The first edge determines the horizontal axis.
	A point and an edge, or three points You will thus define a plane.

In other words, you will select, in the geometry, one of the followings:

	a plane
	a point and then an edge
	an edge and then a point
	two edges
	two points and then an edge
	three points

Note that you can redefine the projection plane using the arrows at any time before the view generation.

3. Click inside the sheet to generate the view.

Right-click the frame of the view, select the Properties option from the contextual menu, View tab and check the required options in the Properties dialog box. By default, the axis and center lines are generated. You can also view hidden lines, threads and fillets.

For fillets, you can choose to view either Boundaries, Symbolic, Original Edges or Projected Original Edges.

	Boundaries: thin lines, representing the mathematical limits of the fillets.
	Symbolic: original edges, projected in a direction that is normal to each corresponding surface.

	Original Edges: original edges, at the intersection of the two surfaces joined by the fillet.
	Projected Original Edges: original edges, projected on fillet surfaces in the direction of the view projection.

Creating advanced front views

The advanced front view command allows the user to make several choices at view creation, such as view name, view scale. Pertinent projection plane is proposed (this plane can be linked by default to local axis) and an object selection caused associated element selection.

Open the Pinmounting.CATPart document. Define a new drawing sheet. Activate the drawing by selecting drawing window.

1. Click the advanced front view creation command

, a dialog box appears:

2. Name the view in the associated field:

3. Modify the scale value in 1:2

4. Click OK to validate your settings.

5. Select one plane of the 3D part or a plane surface, to define the reference plane.
Blue arrows appear, you can still choose a plane and an orientation before view generation.

6. Click inside the sheet to generate the view.

Creating front view with local axis system

This functionality allows you to take into account a local axis system when creating a view. That way, the origin of the generated view is the projection of the origin of the local axis system selected in the view plane.

Open the Axisprojection.CATPart document. Define a new drawing sheet.

1. Select the drawing to activate it and click the Front View icon

from the Views toolbar.

2. In the Part tree, select the local 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 end the view creation. The part local axis system appears in the view.

Multi-Selecting Sub-Bodies/Sub-Products

You can multi-select sub-products in a product and also bodies in a part. These multi-selected 3D elements will be previewed and then used as reference planes for generating several front views.

Open the Product_Balloon.CATProduct document. Double-click Scene1 at the down left of the screen.

1. Click the Front View icon

from the Views toolbar.

2. Select one body or press the Ctrl key and then multi-select the desired elements in the specification tree.

Multi-select several bodies in a product:

3. Select the geometry defining the projection plane.

As you go over the geometry with the cursor, the oriented preview automatically appears on the 3D document.

4. Click on the desired plane in the 3D.

Be careful: once you multi-select bodies or sub-products, and go further into the dialog, 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 document.

Note that once an element is selected, this element becomes gray colored.

In addition, you can only work in one 3D document. If you try selecting another document, you automatically leave the Front View command.

The multi front view is being created and you can still modify the multi front view orientation:

5. Click on the drawing document to generate the views.

You can insert Bill of Material information into the active view.

Projecting points from 3D

Open the PointSketch.CATPart document.

1. In Tools ->Options -> Mechanical Design -> Drafting -> Generation tab, check Project 3D Points to allow you to project points from 3D (no construction elements).

Then set the projection parameters:

2. Click Configure to open the following dialog box:

3. You can select the following settings:

	`3D symbol inheritance`: the 3D points symbols will be preserved in the 2D.
	`Symbol`: you can choose a symbol in the following menu:

Select the cross as symbol.

4. Then create a front view (here with (x, z) plane).

Points from 3D are projected. These points behavior is the same as other projected geometries behavior. It can be dimensioned, dressed-up, isolated, etc. in different view type except section cut views.

5. Right-click on the front view and select Properties.
Choose the View tab and in the Dress-up area, uncheck 3D points.

viewpropertiesNLS.gif (8023 bytes)

The points disappear:

You can modify interactively graphic properties after generation, they will be preserved from view update.