Catia - Tutorial 3.pdf

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An Introduction to CATIA V5
Release 12
(A Hands-On Tutorial Approach)
Kirstie Plantenberg
University of Detroit Mercy
SDC
Schroff Development Corporation
www.schroff.com
www.schroff-europe.com
PUBLICATIONS
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Chapter 2: SKETCHER: Tutorial 2.1
Chapter 2:
SKETCHER
Tutorial 2.1: Sketch Work
Modes
Featured Topics & Commands
The Sketcher workbench
...........................
2.1-2
The Sketch tools toolbar
...........................
2.1-3
Part Modeled
...........................
2.1-3
Section 1: Using Snap to Point
...........................
2.1-4
Section 2: Using Construction Elements
...........................
2.1-6
Section 3: Geometrical and Dimensional Constraints
...........................
2.1-8
Section 4: Cutting the part by the sketch plane
........................... 2.1-10
Prerequisite Knowledge & Commands
Entering workbenches
•
Entering and exiting the Sketcher workbench
•
Drawing simple profiles
•
Simple Pads and Pockets
•
2.1 - 1
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Chapter 2: SKETCHER: Tutorial 2.1
The Sketcher Workbench
The Sketcher workbench is a set of tools that helps you create and constrain 2D
geometries. Features (pads, pockets, shafts, etc...) may then be created solids or
modifications to solids using these 2D profiles. You can access the Sketcher
workbench in various ways. Two simple ways are by using the top pull down
menu ( S tart – M echanical Design – S ketcher), or by selecting the Sketcher
icon. When you enter the sketcher, CATIA requires that you choose a plane to
sketch on. You can choose this plane either before or after you select the
Sketcher icon. To exit the sketcher, select the Exit Workbench
icon.
The Sketcher workbench contains the following standard workbench specific
toolbars.
Profile toolbar: The commands located
in this toolbar allow you to create simple
geometries (rectangle, circle, line, etc...)
and more complex geometries (profile,
spline, etc...).
•
Operation toolbar: Once a profile has been created,
it can be modified using commands such as trim,
mirror, chamfer, and other commands located in the
Operation toolbar.
•
Constraint toolbar: Profiles may be constrained with
dimensional (distances, angles, etc...) or geometrical
(tangent, parallel, etc...) constraints using the
commands located in the Constraint toolbar.
•
Sketch tools toolbar: The commands in this toolbar
allow you to work in different modes which make
sketching easier.
•
User Selection Filter toolbar: Allows you to
activate different selection filters.
•
Tools toolbar: Allows you to, among others other things,
to analyze a sketch for problems, cut the part by the
sketch plane, and create a datum.
•
2.1 - 2
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Chapter 2: SKETCHER: Tutorial 2.1
The Sketch tools Toolbar
The Sketch tools toolbar contains icons that activate and deactivate different
work modes. These work modes assist you in drawing 2D profiles. Reading from
left to right, the toolbar contains the following work modes; (Each work mode is
active if the icon is orange and inactive if it is blue.)
Snap to Point: If active, your cursor will snap to the
intersections of the grid lines.
•
Construction / Standard Elements: You can draw two
different types of elements in CATIA a standard
element and a construction element. A standard element (solid line type) will
be created when the icon is inactive (blue). It will be used to create a feature
in the Part Design workbench. A construction element (dashed line type) will
be created when the icon is active (orange). They are used to help construct
your sketch, but will not be used to create features.
•
Geometric Constraints: When active, geometric constraints will automatically
be applied such as tangencies, coincidences, parallelisms, etc...
•
Dimensional Constraints: When active, dimensional constraints will
automatically be applied when corners (fillets) or chamfers are created, or
when quantities are entered in the value field. The value field is a place where
dimensions such as line length and angle are manually entered.
•
Part Modeled
The part modeled in
this tutorial is shown
below. The part is
constructed with the
assistance of
different work
modes.
2.1 - 3
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Chapter 2: SKETCHER: Tutorial 2.1
Section 1: Using Snap to Point
1) Enter the Sketcher
on the yz plane.
2) Restore the default positions of the toolbars ( T ools – C ustomize... –
Toolbars tab – Restore position.) Move the Sketch Tools toolbar and the
User Selection Filter toolbar to the top toolbar area.
3) Set your grid spacing. At the top pull down menu, select T ools – O ptions... In
the Options window, expand the Mechanical Design portions of the left side
navigation tree and select Sketcher. Activate the options Display, Snap to
point, and Allow Distortions in the Grid section on the right side. Set your
Primary spacing and Graduations to H:
100 mm
and
20
, and V:
100 mm
and
10
.
4) Select the Spline
icon. This is located in the Profile toolbar in the right
side toolbar area.
2.1 - 4
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