|
In this task, you will learn how to:
|
|
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. |
|
Creating a front view
|
|
|
|
Open the
GenDrafting_part.CATPart document. Define a
new drawing sheet. |
|
-
Click Front View
in the Views toolbar.
-
Select one plane of the 3D part or a plane surface, to
define the reference plane.
Blue arrows appear.
|
- Note that you can redefine the projection plane using the blue
arrows at any time before the view generation: to the bottom, the
left, the right, the top, or rotated using a given snapping or
according to an edited rotation angle. For more information, refer
to Before You Begin >
Defining the view orientation.
- 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
|
-
Click in the drawing to generate the view.
|
By default, the axis and center lines are generated. You can also
view hidden lines, threads, fillets, project 3D points, etc. To
customize the view properties, right-click the frame of the view and
select Properties. Click the View tab and
select the required options in the Properties dialog box. |
|
- In the case of an assembly view, you can
insert Bill of Material information
into the active view.
- 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.
|
|
|
Creating a front view with a 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. |
|
-
Click Front View
in the Views toolbar.
-
In the part specification tree, select the local axis
system, Axis System.1.
|
Remember that you have to select the axis system in the
specification tree and not in the 3D part. Otherwise it would be like
selecting a line in the 3D part instead of the axis system. |
-
Select one plane of the 3D part or a plane surface, to
define the reference plane.
-
Click in the drawing to end the view creation. The part
local axis system appears in the view.
|
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. |
|
|
Creating a front view from specific sub-bodies/sub-products
|
|
|
|
You can multi-select specific sub-products in a product and/or several
sub-bodies in a part to create front views displaying the selected elements
only. 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. |
|
-
Click Front View
in the Views toolbar.
-
Select one body, or press the Ctrl key and
then multi-select the desired elements in the specification tree.
-
In the 3D, point to the geometry to choose a projection
plane. As you go over the geometry with the cursor, the oriented preview
automatically appears on the 3D document.
|
|
Be careful: once you multi-select 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 document.
|
|
The Hide/Show mode on a body is not projected in a generated view. It is not considered as a body modification, so the
Update icon does not take it into account. To visualize the Hide/Show modification of a body in the generated view, type
c:force update in the Power Input field. |
|
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 to select another document, the Front View command
quits. |
-
When the oriented preview corresponds to the projection
plane you want, click on the plane to validate.
The front view is previewed. At this point, you can still
modify its orientation:
-
Click in the drawing to generate the view.
|
|
Creating a front view using 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 as often as necessary without having to select the features
again. |
|
Open the
Product_Balloon.CATProduct document. |
|
-
Before you start creating views from selection sets, you
first need to create one or more selection sets for this product. For
more information, refer to
Storing Selections Using Selection in the Infrastructure User's
Guide. For example, create a selection set to store the product
screws.
-
Click Front View
in the Views toolbar.
-
Activate the CATProduct document and select Edit >
Selection Sets...
-
In the Selection Sets Selection dialog box that is
displayed, select a selection set and click the Select button. The
selection set items are highlighted in the 3D and in the specification
tree.
For more information, refer to
Selecting Selection Sets in the Infrastructure User's Guide.
|
Once you have selected a selection set, you can use the Ctrl
key to select additional sub-bodies or sub-products. |
-
In the 3D, point to the geometry to choose a projection
plane. As you go over the geometry with the cursor, the oriented preview
automatically appears on the 3D document.
-
When the oriented preview corresponds to the projection
plane you want, click on the plane to validate.
The front view is previewed. At this point, you can still
modify its orientation:
-
Click in the drawing to generate the view.
|
- You can also use selection sets when creating isometric views
and advanced front views.
- You can also use selection sets to select the sub-bodies and/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 will not be seen as needing
an update, and if you do update the view, its definition will not
change. You have to create the view over again in order for your
modifications to be taken into account.
|
|
|