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CATIA V5 Fundamentals - Lesson 10: Drafting
Copyright DASSAULT SYSTEMES
10-1
Copyright DASSAULT SYSTEMES
Lesson 10: Drafting
In this lesson, you will learn to create a drawing of a part.
Case Study: Drafting
Design Intent
Stages in the Process
Start a New Drawing
Apply a Title Block
Create Views
Create Dimensions and Annotations
Save the Drawing
Print the Drawing
Duration: Approximately 0.25 day
Lesson content:
Lesson Content
Student Guide: Lesson 10: Drafting
Introduce the lesson. Present the lesson objectives and topics.
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Case Study: Drafting
The case study for this lesson is the Base part used in the Drill Press assembly, shown
below. This case study focuses on incorporating the design intent when creating the drawing
for the part.
Case Study: Drafting
Student Guide: Lesson 10- Case Study: Drafting
Introduce the case study for the lesson.
The base is part of the stand sub-assembly.
Locate where the base is in the sub-assembly and where the sub-assemlby is in the
main assembly.
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Design Intent
The drawing should be created using
an ANSI standard.
The drawing should contain one view
that shows hidden lines and axis.
The drawing should contain a title
block.
The base drawing must meet the following
design intent requirements:
Case Study: Drafting
Student Guide: Lesson 10- Design Intent
Identify the design intent for this model.
1. Standards are predefined formats for dimensions, annotations, and
views, which provide a consistent interpretation of information.
2. The display of these items in a single view enables a better
understanding of the model by showing depth and internal features.
3.This is typically required with any drawing.
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CATIA V5 Fundamentals - Lesson 10: Drafting
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Stages in the Process
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and annotations.
5. Save the drawing.
6. Print the drawing.
The following steps will be used to create the detail drawing of
the base part:
Case Study: Drafting
Student Guide: Lesson 10- Stages in the Process
Identify the stages in the process.
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CATIA V5 Fundamentals - Lesson 10: Drafting
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Introduction to Generative Drafting
The 3D environment gives designers a very efficient and
flexible tool to create parts and assemblies; however, it is
often necessary to convey this information with 2D
drawings of the components to communicate manufacturing
information.
Introduction to Generative Drafting
Student Guide: Lesson 10- Introduction to Generative Drafting
Introduce the concept of Generative drafting.
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General Process
Part Design
Assembly Design
Generative
Drafting
Sketcher
Associative link
General Process
Student Guide: Lesson 10- General Process
The creation of a drawing for parts and assemblies can begin at any time in the design
process.
CATIA maintains an associative link between a drawing and the parts and assemblies it
references.
As the 3D part and assembly models evolve, the drawings automatically show the
updated geometry.
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CATIA V5 Fundamentals - Lesson 10: Drafting
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Accessing the Workbench
B
C
A
Accessing the Workbench
Student Guide: Lesson 10- Accessing the Workbench
The drawings of parts and assemblies are created in CATIA using the Drafting
workbench. It can be accessed in the following three ways:
A. Start menu
B. File menu
C. Workbench icon
D. New icon
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CATIA V5 Fundamentals - Lesson 10: Drafting
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The Drawing Environment
A
B
C
D
The Drawing Environment
Student Guide: Lesson 10- The Drawing Environment
The drawing environment, accessed through the Drafting workbench, consists of the
following components:
A. Specification tree: Contains sheet and view information.
B. Sheet: Contains the drawing views, title block, annotations,
dimensions, etc. The active view is underlined in the tree and enclosed in a red frame.
C. Prompt: Displays instructions and requirements for tools as they are
activated. Command line entries are also made here.
D. Toolbars: Contains the Drafting workbench tools
Note the file extension at the top of the interface. A CATIA drawing is saved as a file
with the .CATDrawing file name extension.
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CATIA V5 Fundamentals - Lesson 10: Drafting
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Step 1: Start a New Drawing
In this section, you will learn to create a
new drawing.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 1 - Start a New Drawing
Student Guide: Lesson 10- Step 1: Start a New Drawing
Introduce the step.
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CATIA V5 Fundamentals - Lesson 10: Drafting
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Starting a Drawing with a Blank Sheet
2
1
1. Change to the Drafting workbench from the
Part workbench.
2. Set the properties of the drawing in the
New Drawing window.
3. Select OK.
Use the following steps to create a new blank
drawing:
Step 1 - Start a New Drawing
Student Guide: Lesson 10- Setting the Drawing Sheet Format and Drafting Standards,
Lesson 10- Starting a Drawing with a Blank Sheet
Identify the steps to create a new drawing.
Step2: Once a new drawing is started, you are prompted to define
properties of the drawing. You can set the following items:
==> Standard: ISO, ANSI, or JIS standards
==> Paper format: A, B, C, or A0, A1, A2, etc.
==> Orientation: Landscape or portrait
Ensure there are no questions before moving onto the next step
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Step 2: Apply a Title Block
In this section, you will learn about title
blocks and how to insert one into a
drawing.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 2 - Apply a Title Block
Student Guide: Lesson 10- Step 2: Apply a Title Block
Introduce the step.
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CATIA V5 Fundamentals - Lesson 10: Drafting
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Drawing Title Blocks (1/2)
A. Manually create a template drawing using geometry tools.
B. Customized macros
Title blocks in CATIA can be generated in two ways:
Step 2 - Apply a Title Block
Student Guide: Lesson 10- Drawing Title Blocks (1/2)
Title blocks in CATIA can be generated in two ways:
A. You can manually create a template drawing using geometry tools.
You can then use the template as a start drawing for all new drawings. Click File > New
From in the menu bar to create a file from a template.
B. You can enter customized macros to generate the title block. CATIA
supplies some sample title blocks that can be used as a starting point to generate unique
ones for your company.
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CATIA V5 Fundamentals - Lesson 10: Drafting
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Drawing Title Blocks (2/2)
2
3
4
5
6
1. Click Edit > Background to enter the
frame and title editor mode of CATIA.
2. Select the Frame Creation icon.
3. Select the type of title block in the Style of
Titleblock pull-down menu.
4. Select Creation as the Action to apply.
5. Select Apply.
6. Select OK.
Use the following steps to insert a title block
into a drawing:
Step 2 - Apply a Title Block
Student Guide: Lesson 10- Drawing Title Blocks (2/2)
Identify the steps to apply a title block.
Step 2: The Insert Frame and Title Block window appears, displaying
the default styles and sample macros.
Ensure there are no questions before moving onto the next step
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Step 3: Create Views
In this section, you will learn how to create
basic drawing views.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 3 - Create Views
Student Guide: Lesson 10- Step 3: Create Views
Introduce the step.
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Types of Views
A
B
Two types of views can be created in CATIA:
A. Associative
B. Non-associative
Step 3 - Create Views
Student Guide: Lesson 10- Types of Views
Views represent a part in different orientations such that its design intent can be fully
conveyed.
Two types of views can be created in CATIA:
A. Associative (i.e., linked to 3D models), which are called Generated
Views.
B. Non-associative (i.e., not linked to 3D models), which are called Draw
Views.
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Creating Views …
A
B
Fly-out menus
A. Individually
• Many types of views can be created one
by one in an “as needed” approach.
B. View Wizard
• The View Wizard is a quick way to select
predefined view layouts, or define a
customized view configuration.
Views can be created in two ways:
Step 3 - Create Views
Student Guide: Lesson 10- Creating Views …
Identify the ways to create a view.
In this course, you will learn how to create a front view, projection view, and use the View
Wizard.
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Creating a Front View (1/2)
2
3
1
1. Start the drawing with a blank sheet.
2. Select the Front View icon.
3. Activate the CATPart by clicking Window >
Sample.CatPart.
4. Move the mouse cursor over a plane or
planar surface to define the front view.
A preview will appear.
Use the following steps to create a front view:
4
Step 3 - Create Views
Student Guide: Lesson 10- Creating a Front View (1/2)
When you create views individually, you typically create a front view first. It can be
created from a part, sub-body of a part, product, or sub-part of a product.
Identify the steps to create a front view.
The Front View is used as the defining view when creating projection views.
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Creating a Front View (2/2)
6
5
5. Once you are satisfied with the preview,
select the reference and you will
automatically be placed in the drawing with
a preview of the view displayed. You can
manipulate and tweak the orientation using
the compass.
6. Select anywhere on the drawing sheet to
generate the view.
Use the following steps to create a front view
(continued):
Step 3 - Create Views
Student Guide: Lesson 10- Creating a Front View (2/2)
Identify the steps to create a front view.
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CATIA V5 Fundamentals - Lesson 10: Drafting
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Using the Compass
right arrow
click
The compass enables you to reorient a view as needed for your design intent. This
functionality only exists during the creation of the front view.
center left
arrow click
Step 3 - Create Views
Student Guide: Lesson 10- Using the Compass (1/3), (2/3), (3/3)
The compass enables you to reorient a view as needed for your design intent. This
functionality only exists during the creation of the front view.
You can perform the following actions using the compass:
A. Click the up, down, left, and right arrows to flip the background plane
view 90 degrees.
B. Click the center left and right arrows to rotate the view 30 degrees on
the same plane. The 30 degrees increment can be changed by right mouse clicking the
dial, which accesses the contextual menu.
C. You can rotate the view by setting a rotation angle or rotating freely.
When finished setting the view, click on the dial center or anywhere on sheet to generate
the front view.
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Adding Projection Views
1
2
3
1. Select the Projection View icon.
2. Place the mouse cursor in the area of the
drawing where you want to create the
view. A preview of the projection view
appears.
3. Click on the drawing to place the view.
Use the following steps to add a projection
view:
Step 3 - Create Views
Student Guide: Lesson 10- Adding Projection Views
After placing the initial front view, projection views (e.g., top, bottom, right, and left) can
be added quickly using the front view as a reference.
Identify the steps to place a projection view.
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Adding an Isometric View
3
2
1
1. Select the Isometric View icon.
2. Select a face on the part in the part or
product document. A preview of the
isometric view appears.
3. Select anywhere on the drawing to
generate the view.
Use the following steps to add an isometric
view:
Step 3 - Create Views
Student Guide: Lesson 10- Adding an Isometric View
The isometric view that is created in a drawing is solely dependant on the orientation of
the model in part mode and the reference surface selected.
Identify the steps to add an isometric view.
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Copyright DASSAULT SYSTEMES
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Generating views using the View Wizard (1/2)
2
3
1
4
1. Select View Wizard icon.
2. Select one of the view configurations and
select Next for additional views.
3. Select and place additional views (e.g.,
isometric view) in the existing view
configuration.
4. Select Finish.
Use the following steps to define a view layout:
A
B
Step 3 - Create Views
Student Guide: Lesson 10- View Wizard, Lesson 10- Generating views using the View
Wizard (1/3)
The View Wizard enables you to quickly create the following:
A. Standard view layouts, including:
a. Front, Top, Left
b. Front, Bottom, Right
c. All views
B. Custom view layouts, including:
a. Adding views to create a specific view configuration.
b. Deleting, and rearranging the views as needed.
The View Wizard enables you to quickly define a view layout using only an initial plane or
planar surface to define the front view.
Identify the steps used to define a view layout.
Views can be removed from the layout by right clicking on the view and clicking Delete
from the contextual menu.
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CATIA V5 Fundamentals - Lesson 10: Drafting
Copyright DASSAULT SYSTEMES
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Generating views using the View Wizard (2/2)
5
6
5. Select the face on the 3D part for the front
view background plane.
6. A preview of your view configuration
appears on the drawing sheet.
7. Select anywhere on the drawing to
generate and modify the individual view
location as needed.
Use the following steps to define a view layout
(continued):
7
Step 3 - Create Views
Student Guide: Lesson 10- Generating views using the View Wizard (2/3), (3/3)
Identify the steps used to define a view layout.
Step 5: A preview of the Front view appears in the Part Design
workbench when pre-selected (i.e., highlighted) by the cursor.
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Repositioning Views (1/5)
• Set Relative Positioning
• Position Independently of Reference View
• Superpose
• Align Views Using Elements
You can modify the position of a view after placing it
in the drawing. Select the view frame and drag the
view to move it to another location. The projection
view is constrained by its parent view.
In addition to simply dragging and dropping, views
can be repositioned in four other ways:
Step 3 - Create Views
Student Guide: Lesson 10- Repositioning Views (1/5)
Identify the ways to reposition a view.
More detail on each method is provided on the next slides.
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Repositioning Views (2/5)
2
3
4
1. Activate the view you want to move.
2. Right mouse click the view frame and
click Set Relative Position. A direction
positioning line appears relative to the
view.
3. Select the direction line black reference
point, the icon will change to a blinking
red endpoint until another point is
selected to move relative to.
4. The green end point of the direction
line can be moved to different anchor
points of the view or dragged free
hand.
Use the following steps to reposition a view
using the Set Relative Position option :
Step 3 - Create Views
Student Guide: Lesson 10- Repositioning Views (2/5)
The Set Relative Positioning option enables you to move a view based on its relative
location to various elements (e.g., point, line, view frame).
Identify the steps used to reposition a view using the Set Relative Position option.
The direction positioning line itself can be used to align the view with respect to an edge.
Select the line and then the corresponding edge you want to align the view to.
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Repositioning Views (3/5)
2
1
Moving a Dependent Projection View
Moving an Independent Projection View
3
1. Activate the view you want to move.
2. Right mouse click the view frame and
click Position Independently of
Reference View.
3. Drag and drop the view.
Use the following steps to reposition a
view independent of the reference view :
Step 3 - Create Views
Student Guide: Lesson 10- Repositioning Views (3/5)
The Position Independently of Reference View option enables you to reposition a view
without it being constrained by its parent view.
Identify the steps to position a view independently.
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Repositioning Views (4/5)
1
2
3
1. Activate the view you want to move.
2. Right mouse click the view frame and
click Superpose.
3. Select the view onto which you want
to superimpose the first view.
Use the following steps to superimpose
a view:
Step 3 - Create Views
Student Guide: Lesson 10- Repositioning Views (4/5)
The Superpose option enables you to superimpose a view onto another view.
Identify the steps to superimpose a view.
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Repositioning Views (5/5)
2
3
4
1
1. Right mouse click the view frame and
click Align Views Using Elements.
2. Select an edge from the view you
wish to align.
3. Select an edge from the view you
wish to align the previous view to.
4. The view moves accordingly. In this
example, they are aligned based on
the edge of a part.
Use the following steps to reposition a
view using the Align Views Using
Elements option :
Step 3 - Create Views
Student Guide: Lesson 10- Repositioning Views (5/5)
The Align Views Using Elements option enables you to align a view with another view
based on similar geometry between the two.
Identify the steps used to align views.
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Deleting Views
A
B
Views can be selected from the specification tree or directly on the drawing.
Step 3 - Create Views
Student Guide: Lesson 10- Deleting Views
Once you select the view(s) you want to remove, use one of the following methods to
delete the view(s):
A. Click Edit > Delete to delete the selected view(s).
B. Click Delete from the contextual menu.
C. Press the key on the keyboard to delete the selected views.
In CATIA you are able to delete views that have children views associated to it. The child
view becomes an independent view once its parent is deleted.
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View Properties
1
2
3
Step 3 - Create Views
Student Guide: Lesson 10- View Properties
Use the following steps to modify the properties of a view:
1. Right click on a view in the specification tree or in the view frame.
Click Properties from the pop-up menu. The Properties window appears.
2. Use the View and Graphic tabs to change the required options. The
following properties are modified in this example:
==> View name
==> Fillets on dress-up features
==> Visualization to remove the frame
3. The view is modified as shown.
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Sheet Properties
2
1
Step 3 - Create Views
Student Guide: Lesson 10- Sheet Properties
Use the following steps to modify the properties of a sheet:
1. Right click on the sheet in the specification tree. Click Properties from
the pop-up menu.
2. In the properties window, you can make modifications to the sheet,
such as the sheet name, scale, and the projection method (ANSI or ISO).
Use the Third angle standard option generate the views on the sheet using the 3rd angle
projection method (ANSI).
Ensure there are no questions before moving onto the next step.
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Step 4: Create Dimensions and Annotations
In this section, you will learn to create
dimensions and annotations.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Step 4: Create Dimensions and Annotations
Introduce the step.
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CATIA V5 Fundamentals - Lesson 10: Drafting
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Dimensions
Dimensions define the size and functional intent of a part, often required to create a
fabrication drawing for a manufacturer. Dimensions can be manually created on the drawing
or shown from Part mode.
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensions
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Types of Manual Dimensions
A
B
C
A
B
C
D
E
D
F
E
F
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Types of Manual Dimensions (1/2), (2/2)
Identify the types of dimensions. Detail on each type is provided on the next slides.
Using the Dimensions toolbar, you can create the following types of dimensions:
A. Linear
B. Angular
C. Radius
D. Diameter
E. Chamfer
F. Thread
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Dimensions System
A
B
C
C
B
A
A. Chained
B. Cumulated
C. Stacked
Using the Dimensions toolbar, you can create
the following types of dimension systems:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensions System
Identify the types of dimenisoning systems possible.
Detail on each will be provided in the next slides.
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Types of Dimension Locators (1/2)
Cursor position
Cursor position
Cursor position
A
B
A B
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Types of Dimension Locators (1/2)
When applying a manual dimension, depending on the geometry, there is the possibility
that many different types of dimensions can be created to describe the same entity.
When a manual dimension icon is selected the Tools Palette toolbar appears to further
refine the type of dimension to be created.
CATIA enables you to locate manual dimensions with five types of positioning tools:
A. Projection Dimensions: The placement of the cursor determines the
dimension that will be created.
B. Forced on element: Regardless of the cursor placement, the
dimension is forced to be parallel with the element selected.
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Types of Dimension Locators (2/2)
C D E F G
C
D
F
E
G
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Types of Dimension Locators (2/2)
CATIA enables you to locate manual dimensions with five types of positioning tools:
C. Forced Horizontal: Regardless of cursor placement, the dimension is
forced horizontal to the element selected.
D. Forced Vertical: Regardless of cursor placement, the dimension is
forced vertical to the element selected.
E. Force Dimension along a direction: Place the dimension with respect
to other entities.
F. True length: Regardless of the view orientation, the dimension is the
exact length of the 3D element selected.
G. Intersection Point Detected: Create a dimension based on
intersection of geometry.
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Creating Dimensions
A
B
C
D
A.
Linear
B.
Angular
C.
Radius
D.
Diameter
E.
Chamfer
F.
Thread
G.
Coordinate
Using the Dimensions toolbar, you can create
the following types of dimensions:
E
F
G
Step 4 - Create Dimensions and Annotations
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Dimensioning a Length
1
2
3
4
1. Select the Length/Distance dimensions
icon with the Projected placement option.
2. Select the edge you want to dimension.
3. Select the dimension line and drag it to the
desired position (hold down the left mouse
button while dragging).
4. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension a length:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Length
Identify the steps used to create a length dimension.
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Dimensioning a Distance
2
3
4
1
5
1. Select the Length/Distance Dimensions
icon with the Projected placement option.
2. Select the first edge.
3. Select the second edge.
4. Select the dimension line and drag it to the
desired position (hold down the left mouse
button while dragging).
5. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension a
distance:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Distance
Identify the steps used to create a distance dimension.
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Dimensioning a Hole
2
3
1
4
5
1. Select the Dimensions icon with the
Projected placement option.
2. Select the first circle.
3. Select the second circle.
4. Select the dimension line and drag it to the
desired position (hold down the left mouse
button while dragging).
5. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension holes:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Hole
Identify the steps used to dimenison holes.
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Dimensioning a True Length
1
4
3
2
1. Select the Dimensions icon.
2. Select the True Dimension Length
dimension mode.
3. Select an element in an Isometric View.
4. Select the dimension line and drag it to the
desired position (hold down the left mouse
button while dragging).
5. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension the true
length of an edge:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a True Length
Identify the steps used to dimenison true length.
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Dimensioning a Simple Angle
1
2
3
4
5
1. Select the Angle Dimensions icon.
2. Select the first edge.
3. Select the second edge.
4. The angle dimension is created. To change
the sector that it describes, right mouse
click the dimension and click Angle Sector
in the contextual menu.
5. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension an angle:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Simple Angle
Identify the steps used to dimension an angle.
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Dimensioning a Simple Radius
1
2
3
4
5
1. Select the Dimensions icon.
2. Select the radius you want to dimension. The
dimension may appear by default as a
diameter dimension; if that is the case, you
must change it to a radius dimension.
3. Select the dimension, right mouse click, and
click Radius Center in the contextual menu.
4. Select the dimension line and drag to rotate
the dimension to the desired position (hold
down the left mouse button while rotating).
5. Select anywhere on the drawing to complete
the dimension creation.
Use the following steps to dimension a radius:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Simple Radius
This dimension could also be created by using the Radius Dimensions icon.
Identify the steps used to create a radius dimension.
Most dimensions can be created using the Dimensions icon and contextual menus.
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Dimensioning a Diameter
1
2
4
3
1. Select the Diameter Dimensions icon.
2. Select the circle to dimension. The
diameter dimension appears as shown.
3. Select the dimension line and drag to
rotate the dimension to the desired position
(hold down the left mouse button while
rotating).
4. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension a
diameter:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Diameter
Identify the steps used to create a diameter dimension.
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Dimensioning a Chamfer
1
2
3
1. Select the Chamfer Dimensions icon,
then select the Chamfer format from the
Tools Palette toolbar.
2. Select a chamfer line or surface to be
dimensioned.
3. Select anywhere on the drawing to
complete the chamfer dimension creation.
Use the following steps to dimension a
chamfer:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Chamfer
Identify the steps used to create a chamfer dimenison.
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Dimensioning a Thread
1
A
B
Use the following steps to create a thread
dimension:
1. Select the Thread Dimension icon.
2. Select the Thread representation to
dimension.
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Thread
Thread features need to be created in the model to create this type of dimension.
Thread dimensions can be created for:
A. Top views.
B. Side views.
Identify the steps used to dimension a thread.
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Chain Dimensions
1
2
3
4
5
1. Select Dimensions icon.
2. Select the first edge.
3. Select the next edge.
4. Select the next edge.
5. Select the next edge.
6. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to create a chain
dimension:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Chain Dimensions
Identify the steps used to create chain dimensions.
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Stacked Dimensions
1
2
3
3
3
1. Select the Stacked Dimensions icon.
2. Select the origin point or edge of your
cumulated system.
3. Select all the other points or edges of your
cumulated system (as many as you
require).
4. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to create a stacked
dimension:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Stacked Dimensions
Identify the steps used to create stacked dimensions.
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Cumulated Dimensions
1
2
3
3
3
4
Use the following steps to create a cumulated
dimension:
1. Select the Cumulated Dimensions icon.
2. Select the origin point or edge of your
cumulated system.
3. Select all the other points or edges of your
cumulated system (as many as you
require).
4. Select anywhere on the drawing to
complete the dimension creation.
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Cumulated Dimensions
Identify the steps used to create cumulated dimensions.
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Dimension Properties
A
B
C
D
E
A. Dimension line
B. Tolerance description
C. Tolerance
D. Numerical display description
E. Precision
You can control the display of dimensions by
using the Dimension Properties toolbar. You
can customize the following areas of a
dimension:
Step 4 - Create Dimensions and Annotations
Student Guide: 10-57
You can control the display of dimensions by using the Dimension Properties toolbar.
You can customize the following areas of a dimension:
A. Dimension line: Set the display of the dimension line with respect to
the dimension.
B. Tolerance description: Displays the dimension using a tolerance
scheme.
C. Tolerance: Changes the tolerance value for the dimension.
D. Numerical display description: Displays the dimension in a particular
unit.
E. Precision: Sets the precision of the dimension.
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Annotations
A
B
C
D
E
F
A. Text
B. Text with Leader
C. Replicate text
D. Balloons
E. Datum Target
F. Text template
In addition to creating dimensions in a drawing,
you can add notes and annotations to it. The
Text toolbar contains the following tools:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Annotations
In addition to creating dimensions in a drawing, you can add notes and annotations to it.
The Text toolbar contains the following tools:
A. Text: Create a textbox with no leader.
B. Text with Leader: Create a textbox with a leader.
C. Replicate text: Create a copy of an existing text box and attribute link
it to geometry.
D. Balloons: Creates a text balloon.
E. Datum Target: Creates a datum target.
F. Text template: Place a predefined text template.
Ensure there are no questions before moving onto the next step.
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Step 5: Save the Drawing
In this section, you will learn to save a
drawing.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 5 - Save the Drawing
Student Guide: Lesson 10- Step 5: Save the Drawing
Introduce the step.
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Matching Drawing with Modified 3D Part
60
40
Step 5 - Save the Drawing
Student Guide: Lesson 10- Matching Drawing with Modified 3D Part
Before saving any drawing, it is a good idea to make sure that it is up to date with the
most recent information.
If the Update icon (shown) is highlighted, this means that the drawing must be updated to
reflect the changes that were made on the 3D part it represents.
In the part shown, for example, the width dimension has been changed from 40 to 60.
Selecting the Update icon regenerates the view with the new dimensions.
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Checking Links to 3D Parts (1/2)
1
1. Click Edit > Links in the menu bar, as
shown.
2. All the drawing views are missing the
same referenced part.
Use the following steps to load a missing
document that is linked to a view:
Step 5 - Save the Drawing
Student Guide: Lesson 10- Checking Links to 3D Parts (1/2)
Its possible that a drawing may be opened without its referenced documents being
loaded in session. This could be caused by a missing file or a global CATIA setting, the
tree identifies this with broken icons.
To update the drawing correctly the links of the drawing need to be verified.
Identify the steps to load a missing document.
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Checking Links to 3D Parts (2/2)
3
4
2
3. Select the Pointed
Documents tab.
4. Select Load to load the part.
5. Update the drawing.
Use the following steps to load a
missing document that is linked
to a view (continued):
Step 5 - Save the Drawing
Student Guide: Lesson 10- Checking Links to 3D Parts (2/2)
Identify the steps to load a missing document.
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Saving a Drawing
• You save a drawing the same way you
would any other CATIA file.
• You can also use the Save As and Save
management tools to store the drawing.
• A drawing is dependent on the 3D part(s) it
represents.
Step 5 - Save the Drawing
Student Guide: Lesson 10- Saving a Drawing
You save a drawing the same way you would any other CATIA file.
You can also use the Save As and Save management tools to store the drawing.
Keep in mind that a drawing is dependent on the 3D part(s) it represents; therefore, it is
important to verify that the parts and drawing is up to date with the most current
information.
Ensure there are no questions before moving onto the next step.
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Step 6: Print the Drawing
In this section, you will learn to print a
drawing.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 6 - Print the Drawing
Student Guide: Lesson 10- Step 6: Print the Drawing
Introduce the step.
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Printing a Drawing
•
Click File > Print or select the Print icon to print your drawing.
Step 6 - Print the Drawing
Student Guide: Lesson 10- Printing a Drawing
Click File > Print or select the Print icon to print your drawing.
The Print window contains enables you to customize the layout, page setup, and options.
It also shows a print preview of the drawing.
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Print User Interface (1/2)
A
B
C
D
E
MultiDocuments Tab
Step 6 - Print the Drawing
Student Guide: Lesson 10- Print User Interface (2/2)
The Print window contains the following information, which you can modify:
A. Printer: Select the printer or key in a file name to print to.
B. Position and Size: Define the position and size of the geometry on
the page.
C. Print Area: Define the area to print.
D. Page Setup: Define the page size and characteristics.
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Print User Interface (2/2)
Step 6 - Print the Drawing
Student Guide: Lesson 10- Print User Interface (2/2)
Select the Options button from the Print window to open the Options dialog box:
A. Color
B. Banner
C. Various
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To Sum Up…
Creation of a new drawing
Insertion of a title block
Creation of basic views
Dimensioning and annotating
Saving and Printing
Using the knowledge learned in this lesson, you
should be able to create the drawing of the Base part.
The drawing requires the following details:
Step 6 - Print the Drawing
Student Guide: Lesson 10- To Sum Up…
Review the process to create the drawing.
Ensure there are no questions before starting the exercises.
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Exercise Overview
You will practice what you have learned by working through three exercises.
Exercise 10C
Exercise 10A
Exercise 10B
Exercise Overview
Student Guide: Lesson 10- Exercise 10A, Lesson 10- Exercise 10B, Lesson 10- Exercise
10C
* Demonstrate the topics learned in this part of the lesson before or after students work
on the exercises. Decide when to do the demonstration based on the class. Some will
prefer to see you do a demonstration before, some will prefer to struggle with the
exercises and then see a demonstration after. A demonstration of the topics covered
should include, creating an empty drawing, and front, projection, and isometric views.
Demonstrate the use of the compass and that the isometric view is based on the
orientation of the 3D model. Using a different part, create another drawing, this time
generate the views using the View Wizard. Add the overall dimensions and a title block
to one of the drawings.
* Present the exercises available to practice creating drawings.
* As a class discuss what will be involved in completing the exercises. What tools will
they need to use?
* Tell students where they will be saving the models to and where the required start parts
are located. State that they are to move from one exercise to the next and complete all
three exercises and the case study (time permitting).
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Case Study: Drafting
Using the techniques you have learned in this and previous lessons
create the model without detailed instruction.
You will practice what you learned by completing the case study
model using only a detailed drawing as guidance.
Recall the design intent of this model:
The drawing should be created using an ISO standard.
The drawing should contain one view that shows hidden lines and the axis.
The drawing should contain a title block.
Case Study: Drafting
Student Guide: Lesson 10- Case Study: Drafting
Review the requirements for the case study.
Discuss as a class how the drawing will be created, what tools are needed to create the
case study?
Have the students begin the exercises and note the time.
Assist students as needed with the exercises.
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Exercise 10A: Recap
Create a new drawing
Apply a title block
Add views
Create dimensions
Save a drawing
Exercise 10A: Recap
Student Guide: Lesson 10- Exercise 10A: Recap
Review the Exercise Recap slides after the students have attempted the exercises.
Discuss the different tools used in this exercise.
Ask if there are any questions about this exercise, any difficulties?
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Exercise 10B: Recap
Create a drawing
Insert a title block
Create views using the view wizard
Move and delete views
Dimension geometry
Exercise 10B: Recap
Student Guide: Lesson 10- Exercise 10B: Recap
Discuss the different tools used in this exercise.
Ask if there are any questions about this exercise, any difficulties?
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Exercise 10C: Recap
Create a new drawing
Insert a title block
Add views
Dimension and annotate the drawing
Save the drawing
Exercise 10C: Recap
Student Guide: Lesson 10- Exercise 10C: Recap
Discuss the different tools used in this exercise.
How did the students create the views (using the view wizard or manully)?
What tools did the students use to dimension the drawing. Did they use the Dimension
tool for all of them or did they use the specific tool for the type of dimenion needed?
Ask if there are any questions about this exercise, any difficulties?
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Case Study: Base Recap
The drawing should be created using an
ANSI standard.
The drawing should contain one view that
shows hidden lines and the axis.
The drawing should contain a title block.
Case Study: Base Recap
Student Guide: Lesson 10- Case Study: Base Recap
Discuss the objectives of the case study.
Review the process used to create the drawing.
Ensure the students understand the process used to create the case study before
beginning the master project.
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Lesson 10: Drafting
In this lesson, you will learn to create a drawing of a part.
Case Study: Drafting
Design Intent
Stages in the Process
Start a New Drawing
Apply a Title Block
Create Views
Create Dimensions and Annotations
Save the Drawing
Print the Drawing
Duration: Approximately 0.25 day
Lesson content:
Lesson Content
Student Guide: Lesson 10: Drafting
Introduce the lesson. Present the lesson objectives and topics.
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Case Study: Drafting
The case study for this lesson is the Base part used in the Drill Press assembly, shown
below. This case study focuses on incorporating the design intent when creating the drawing
for the part.
Case Study: Drafting
Student Guide: Lesson 10- Case Study: Drafting
Introduce the case study for the lesson.
The base is part of the stand sub-assembly.
Locate where the base is in the sub-assembly and where the sub-assemlby is in the
main assembly.
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Design Intent
The drawing should be created using
an ANSI standard.
The drawing should contain one view
that shows hidden lines and axis.
The drawing should contain a title
block.
The base drawing must meet the following
design intent requirements:
Case Study: Drafting
Student Guide: Lesson 10- Design Intent
Identify the design intent for this model.
1. Standards are predefined formats for dimensions, annotations, and
views, which provide a consistent interpretation of information.
2. The display of these items in a single view enables a better
understanding of the model by showing depth and internal features.
3.This is typically required with any drawing.
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Stages in the Process
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and annotations.
5. Save the drawing.
6. Print the drawing.
The following steps will be used to create the detail drawing of
the base part:
Case Study: Drafting
Student Guide: Lesson 10- Stages in the Process
Identify the stages in the process.
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Introduction to Generative Drafting
The 3D environment gives designers a very efficient and
flexible tool to create parts and assemblies; however, it is
often necessary to convey this information with 2D
drawings of the components to communicate manufacturing
information.
Introduction to Generative Drafting
Student Guide: Lesson 10- Introduction to Generative Drafting
Introduce the concept of Generative drafting.
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General Process
Part Design
Assembly Design
Generative
Drafting
Sketcher
Associative link
General Process
Student Guide: Lesson 10- General Process
The creation of a drawing for parts and assemblies can begin at any time in the design
process.
CATIA maintains an associative link between a drawing and the parts and assemblies it
references.
As the 3D part and assembly models evolve, the drawings automatically show the
updated geometry.
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Accessing the Workbench
B
C
A
Accessing the Workbench
Student Guide: Lesson 10- Accessing the Workbench
The drawings of parts and assemblies are created in CATIA using the Drafting
workbench. It can be accessed in the following three ways:
A. Start menu
B. File menu
C. Workbench icon
D. New icon
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The Drawing Environment
A
B
C
D
The Drawing Environment
Student Guide: Lesson 10- The Drawing Environment
The drawing environment, accessed through the Drafting workbench, consists of the
following components:
A. Specification tree: Contains sheet and view information.
B. Sheet: Contains the drawing views, title block, annotations,
dimensions, etc. The active view is underlined in the tree and enclosed in a red frame.
C. Prompt: Displays instructions and requirements for tools as they are
activated. Command line entries are also made here.
D. Toolbars: Contains the Drafting workbench tools
Note the file extension at the top of the interface. A CATIA drawing is saved as a file
with the .CATDrawing file name extension.
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Step 1: Start a New Drawing
In this section, you will learn to create a
new drawing.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 1 - Start a New Drawing
Student Guide: Lesson 10- Step 1: Start a New Drawing
Introduce the step.
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Starting a Drawing with a Blank Sheet
2
1
1. Change to the Drafting workbench from the
Part workbench.
2. Set the properties of the drawing in the
New Drawing window.
3. Select OK.
Use the following steps to create a new blank
drawing:
Step 1 - Start a New Drawing
Student Guide: Lesson 10- Setting the Drawing Sheet Format and Drafting Standards,
Lesson 10- Starting a Drawing with a Blank Sheet
Identify the steps to create a new drawing.
Step2: Once a new drawing is started, you are prompted to define
properties of the drawing. You can set the following items:
==> Standard: ISO, ANSI, or JIS standards
==> Paper format: A, B, C, or A0, A1, A2, etc.
==> Orientation: Landscape or portrait
Ensure there are no questions before moving onto the next step
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Step 2: Apply a Title Block
In this section, you will learn about title
blocks and how to insert one into a
drawing.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 2 - Apply a Title Block
Student Guide: Lesson 10- Step 2: Apply a Title Block
Introduce the step.
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Drawing Title Blocks (1/2)
A. Manually create a template drawing using geometry tools.
B. Customized macros
Title blocks in CATIA can be generated in two ways:
Step 2 - Apply a Title Block
Student Guide: Lesson 10- Drawing Title Blocks (1/2)
Title blocks in CATIA can be generated in two ways:
A. You can manually create a template drawing using geometry tools.
You can then use the template as a start drawing for all new drawings. Click File > New
From in the menu bar to create a file from a template.
B. You can enter customized macros to generate the title block. CATIA
supplies some sample title blocks that can be used as a starting point to generate unique
ones for your company.
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Drawing Title Blocks (2/2)
2
3
4
5
6
1. Click Edit > Background to enter the
frame and title editor mode of CATIA.
2. Select the Frame Creation icon.
3. Select the type of title block in the Style of
Titleblock pull-down menu.
4. Select Creation as the Action to apply.
5. Select Apply.
6. Select OK.
Use the following steps to insert a title block
into a drawing:
Step 2 - Apply a Title Block
Student Guide: Lesson 10- Drawing Title Blocks (2/2)
Identify the steps to apply a title block.
Step 2: The Insert Frame and Title Block window appears, displaying
the default styles and sample macros.
Ensure there are no questions before moving onto the next step
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Step 3: Create Views
In this section, you will learn how to create
basic drawing views.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 3 - Create Views
Student Guide: Lesson 10- Step 3: Create Views
Introduce the step.
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Types of Views
A
B
Two types of views can be created in CATIA:
A. Associative
B. Non-associative
Step 3 - Create Views
Student Guide: Lesson 10- Types of Views
Views represent a part in different orientations such that its design intent can be fully
conveyed.
Two types of views can be created in CATIA:
A. Associative (i.e., linked to 3D models), which are called Generated
Views.
B. Non-associative (i.e., not linked to 3D models), which are called Draw
Views.
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Creating Views …
A
B
Fly-out menus
A. Individually
• Many types of views can be created one
by one in an “as needed” approach.
B. View Wizard
• The View Wizard is a quick way to select
predefined view layouts, or define a
customized view configuration.
Views can be created in two ways:
Step 3 - Create Views
Student Guide: Lesson 10- Creating Views …
Identify the ways to create a view.
In this course, you will learn how to create a front view, projection view, and use the View
Wizard.
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Creating a Front View (1/2)
2
3
1
1. Start the drawing with a blank sheet.
2. Select the Front View icon.
3. Activate the CATPart by clicking Window >
Sample.CatPart.
4. Move the mouse cursor over a plane or
planar surface to define the front view.
A preview will appear.
Use the following steps to create a front view:
4
Step 3 - Create Views
Student Guide: Lesson 10- Creating a Front View (1/2)
When you create views individually, you typically create a front view first. It can be
created from a part, sub-body of a part, product, or sub-part of a product.
Identify the steps to create a front view.
The Front View is used as the defining view when creating projection views.
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Creating a Front View (2/2)
6
5
5. Once you are satisfied with the preview,
select the reference and you will
automatically be placed in the drawing with
a preview of the view displayed. You can
manipulate and tweak the orientation using
the compass.
6. Select anywhere on the drawing sheet to
generate the view.
Use the following steps to create a front view
(continued):
Step 3 - Create Views
Student Guide: Lesson 10- Creating a Front View (2/2)
Identify the steps to create a front view.
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Using the Compass
right arrow
click
The compass enables you to reorient a view as needed for your design intent. This
functionality only exists during the creation of the front view.
center left
arrow click
Step 3 - Create Views
Student Guide: Lesson 10- Using the Compass (1/3), (2/3), (3/3)
The compass enables you to reorient a view as needed for your design intent. This
functionality only exists during the creation of the front view.
You can perform the following actions using the compass:
A. Click the up, down, left, and right arrows to flip the background plane
view 90 degrees.
B. Click the center left and right arrows to rotate the view 30 degrees on
the same plane. The 30 degrees increment can be changed by right mouse clicking the
dial, which accesses the contextual menu.
C. You can rotate the view by setting a rotation angle or rotating freely.
When finished setting the view, click on the dial center or anywhere on sheet to generate
the front view.
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Adding Projection Views
1
2
3
1. Select the Projection View icon.
2. Place the mouse cursor in the area of the
drawing where you want to create the
view. A preview of the projection view
appears.
3. Click on the drawing to place the view.
Use the following steps to add a projection
view:
Step 3 - Create Views
Student Guide: Lesson 10- Adding Projection Views
After placing the initial front view, projection views (e.g., top, bottom, right, and left) can
be added quickly using the front view as a reference.
Identify the steps to place a projection view.
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Adding an Isometric View
3
2
1
1. Select the Isometric View icon.
2. Select a face on the part in the part or
product document. A preview of the
isometric view appears.
3. Select anywhere on the drawing to
generate the view.
Use the following steps to add an isometric
view:
Step 3 - Create Views
Student Guide: Lesson 10- Adding an Isometric View
The isometric view that is created in a drawing is solely dependant on the orientation of
the model in part mode and the reference surface selected.
Identify the steps to add an isometric view.
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Generating views using the View Wizard (1/2)
2
3
1
4
1. Select View Wizard icon.
2. Select one of the view configurations and
select Next for additional views.
3. Select and place additional views (e.g.,
isometric view) in the existing view
configuration.
4. Select Finish.
Use the following steps to define a view layout:
A
B
Step 3 - Create Views
Student Guide: Lesson 10- View Wizard, Lesson 10- Generating views using the View
Wizard (1/3)
The View Wizard enables you to quickly create the following:
A. Standard view layouts, including:
a. Front, Top, Left
b. Front, Bottom, Right
c. All views
B. Custom view layouts, including:
a. Adding views to create a specific view configuration.
b. Deleting, and rearranging the views as needed.
The View Wizard enables you to quickly define a view layout using only an initial plane or
planar surface to define the front view.
Identify the steps used to define a view layout.
Views can be removed from the layout by right clicking on the view and clicking Delete
from the contextual menu.
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Generating views using the View Wizard (2/2)
5
6
5. Select the face on the 3D part for the front
view background plane.
6. A preview of your view configuration
appears on the drawing sheet.
7. Select anywhere on the drawing to
generate and modify the individual view
location as needed.
Use the following steps to define a view layout
(continued):
7
Step 3 - Create Views
Student Guide: Lesson 10- Generating views using the View Wizard (2/3), (3/3)
Identify the steps used to define a view layout.
Step 5: A preview of the Front view appears in the Part Design
workbench when pre-selected (i.e., highlighted) by the cursor.
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Repositioning Views (1/5)
• Set Relative Positioning
• Position Independently of Reference View
• Superpose
• Align Views Using Elements
You can modify the position of a view after placing it
in the drawing. Select the view frame and drag the
view to move it to another location. The projection
view is constrained by its parent view.
In addition to simply dragging and dropping, views
can be repositioned in four other ways:
Step 3 - Create Views
Student Guide: Lesson 10- Repositioning Views (1/5)
Identify the ways to reposition a view.
More detail on each method is provided on the next slides.
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Repositioning Views (2/5)
2
3
4
1. Activate the view you want to move.
2. Right mouse click the view frame and
click Set Relative Position. A direction
positioning line appears relative to the
view.
3. Select the direction line black reference
point, the icon will change to a blinking
red endpoint until another point is
selected to move relative to.
4. The green end point of the direction
line can be moved to different anchor
points of the view or dragged free
hand.
Use the following steps to reposition a view
using the Set Relative Position option :
Step 3 - Create Views
Student Guide: Lesson 10- Repositioning Views (2/5)
The Set Relative Positioning option enables you to move a view based on its relative
location to various elements (e.g., point, line, view frame).
Identify the steps used to reposition a view using the Set Relative Position option.
The direction positioning line itself can be used to align the view with respect to an edge.
Select the line and then the corresponding edge you want to align the view to.
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Repositioning Views (3/5)
2
1
Moving a Dependent Projection View
Moving an Independent Projection View
3
1. Activate the view you want to move.
2. Right mouse click the view frame and
click Position Independently of
Reference View.
3. Drag and drop the view.
Use the following steps to reposition a
view independent of the reference view :
Step 3 - Create Views
Student Guide: Lesson 10- Repositioning Views (3/5)
The Position Independently of Reference View option enables you to reposition a view
without it being constrained by its parent view.
Identify the steps to position a view independently.
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Repositioning Views (4/5)
1
2
3
1. Activate the view you want to move.
2. Right mouse click the view frame and
click Superpose.
3. Select the view onto which you want
to superimpose the first view.
Use the following steps to superimpose
a view:
Step 3 - Create Views
Student Guide: Lesson 10- Repositioning Views (4/5)
The Superpose option enables you to superimpose a view onto another view.
Identify the steps to superimpose a view.
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Repositioning Views (5/5)
2
3
4
1
1. Right mouse click the view frame and
click Align Views Using Elements.
2. Select an edge from the view you
wish to align.
3. Select an edge from the view you
wish to align the previous view to.
4. The view moves accordingly. In this
example, they are aligned based on
the edge of a part.
Use the following steps to reposition a
view using the Align Views Using
Elements option :
Step 3 - Create Views
Student Guide: Lesson 10- Repositioning Views (5/5)
The Align Views Using Elements option enables you to align a view with another view
based on similar geometry between the two.
Identify the steps used to align views.
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Deleting Views
A
B
Views can be selected from the specification tree or directly on the drawing.
Step 3 - Create Views
Student Guide: Lesson 10- Deleting Views
Once you select the view(s) you want to remove, use one of the following methods to
delete the view(s):
A. Click Edit > Delete to delete the selected view(s).
B. Click Delete from the contextual menu.
C. Press the
In CATIA you are able to delete views that have children views associated to it. The child
view becomes an independent view once its parent is deleted.
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View Properties
1
2
3
Step 3 - Create Views
Student Guide: Lesson 10- View Properties
Use the following steps to modify the properties of a view:
1. Right click on a view in the specification tree or in the view frame.
Click Properties from the pop-up menu. The Properties window appears.
2. Use the View and Graphic tabs to change the required options. The
following properties are modified in this example:
==> View name
==> Fillets on dress-up features
==> Visualization to remove the frame
3. The view is modified as shown.
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Sheet Properties
2
1
Step 3 - Create Views
Student Guide: Lesson 10- Sheet Properties
Use the following steps to modify the properties of a sheet:
1. Right click on the sheet in the specification tree. Click Properties from
the pop-up menu.
2. In the properties window, you can make modifications to the sheet,
such as the sheet name, scale, and the projection method (ANSI or ISO).
Use the Third angle standard option generate the views on the sheet using the 3rd angle
projection method (ANSI).
Ensure there are no questions before moving onto the next step.
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Step 4: Create Dimensions and Annotations
In this section, you will learn to create
dimensions and annotations.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Step 4: Create Dimensions and Annotations
Introduce the step.
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Dimensions
Dimensions define the size and functional intent of a part, often required to create a
fabrication drawing for a manufacturer. Dimensions can be manually created on the drawing
or shown from Part mode.
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensions
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Types of Manual Dimensions
A
B
C
A
B
C
D
E
D
F
E
F
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Types of Manual Dimensions (1/2), (2/2)
Identify the types of dimensions. Detail on each type is provided on the next slides.
Using the Dimensions toolbar, you can create the following types of dimensions:
A. Linear
B. Angular
C. Radius
D. Diameter
E. Chamfer
F. Thread
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Dimensions System
A
B
C
C
B
A
A. Chained
B. Cumulated
C. Stacked
Using the Dimensions toolbar, you can create
the following types of dimension systems:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensions System
Identify the types of dimenisoning systems possible.
Detail on each will be provided in the next slides.
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Types of Dimension Locators (1/2)
Cursor position
Cursor position
Cursor position
A
B
A B
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Types of Dimension Locators (1/2)
When applying a manual dimension, depending on the geometry, there is the possibility
that many different types of dimensions can be created to describe the same entity.
When a manual dimension icon is selected the Tools Palette toolbar appears to further
refine the type of dimension to be created.
CATIA enables you to locate manual dimensions with five types of positioning tools:
A. Projection Dimensions: The placement of the cursor determines the
dimension that will be created.
B. Forced on element: Regardless of the cursor placement, the
dimension is forced to be parallel with the element selected.
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Types of Dimension Locators (2/2)
C D E F G
C
D
F
E
G
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Types of Dimension Locators (2/2)
CATIA enables you to locate manual dimensions with five types of positioning tools:
C. Forced Horizontal: Regardless of cursor placement, the dimension is
forced horizontal to the element selected.
D. Forced Vertical: Regardless of cursor placement, the dimension is
forced vertical to the element selected.
E. Force Dimension along a direction: Place the dimension with respect
to other entities.
F. True length: Regardless of the view orientation, the dimension is the
exact length of the 3D element selected.
G. Intersection Point Detected: Create a dimension based on
intersection of geometry.
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Creating Dimensions
A
B
C
D
A.
Linear
B.
Angular
C.
Radius
D.
Diameter
E.
Chamfer
F.
Thread
G.
Coordinate
Using the Dimensions toolbar, you can create
the following types of dimensions:
E
F
G
Step 4 - Create Dimensions and Annotations
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Dimensioning a Length
1
2
3
4
1. Select the Length/Distance dimensions
icon with the Projected placement option.
2. Select the edge you want to dimension.
3. Select the dimension line and drag it to the
desired position (hold down the left mouse
button while dragging).
4. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension a length:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Length
Identify the steps used to create a length dimension.
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Dimensioning a Distance
2
3
4
1
5
1. Select the Length/Distance Dimensions
icon with the Projected placement option.
2. Select the first edge.
3. Select the second edge.
4. Select the dimension line and drag it to the
desired position (hold down the left mouse
button while dragging).
5. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension a
distance:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Distance
Identify the steps used to create a distance dimension.
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Dimensioning a Hole
2
3
1
4
5
1. Select the Dimensions icon with the
Projected placement option.
2. Select the first circle.
3. Select the second circle.
4. Select the dimension line and drag it to the
desired position (hold down the left mouse
button while dragging).
5. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension holes:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Hole
Identify the steps used to dimenison holes.
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Dimensioning a True Length
1
4
3
2
1. Select the Dimensions icon.
2. Select the True Dimension Length
dimension mode.
3. Select an element in an Isometric View.
4. Select the dimension line and drag it to the
desired position (hold down the left mouse
button while dragging).
5. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension the true
length of an edge:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a True Length
Identify the steps used to dimenison true length.
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Dimensioning a Simple Angle
1
2
3
4
5
1. Select the Angle Dimensions icon.
2. Select the first edge.
3. Select the second edge.
4. The angle dimension is created. To change
the sector that it describes, right mouse
click the dimension and click Angle Sector
in the contextual menu.
5. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension an angle:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Simple Angle
Identify the steps used to dimension an angle.
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Dimensioning a Simple Radius
1
2
3
4
5
1. Select the Dimensions icon.
2. Select the radius you want to dimension. The
dimension may appear by default as a
diameter dimension; if that is the case, you
must change it to a radius dimension.
3. Select the dimension, right mouse click, and
click Radius Center in the contextual menu.
4. Select the dimension line and drag to rotate
the dimension to the desired position (hold
down the left mouse button while rotating).
5. Select anywhere on the drawing to complete
the dimension creation.
Use the following steps to dimension a radius:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Simple Radius
This dimension could also be created by using the Radius Dimensions icon.
Identify the steps used to create a radius dimension.
Most dimensions can be created using the Dimensions icon and contextual menus.
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Dimensioning a Diameter
1
2
4
3
1. Select the Diameter Dimensions icon.
2. Select the circle to dimension. The
diameter dimension appears as shown.
3. Select the dimension line and drag to
rotate the dimension to the desired position
(hold down the left mouse button while
rotating).
4. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to dimension a
diameter:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Diameter
Identify the steps used to create a diameter dimension.
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Dimensioning a Chamfer
1
2
3
1. Select the Chamfer Dimensions icon,
then select the Chamfer format from the
Tools Palette toolbar.
2. Select a chamfer line or surface to be
dimensioned.
3. Select anywhere on the drawing to
complete the chamfer dimension creation.
Use the following steps to dimension a
chamfer:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Chamfer
Identify the steps used to create a chamfer dimenison.
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Dimensioning a Thread
1
A
B
Use the following steps to create a thread
dimension:
1. Select the Thread Dimension icon.
2. Select the Thread representation to
dimension.
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Dimensioning a Thread
Thread features need to be created in the model to create this type of dimension.
Thread dimensions can be created for:
A. Top views.
B. Side views.
Identify the steps used to dimension a thread.
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Chain Dimensions
1
2
3
4
5
1. Select Dimensions icon.
2. Select the first edge.
3. Select the next edge.
4. Select the next edge.
5. Select the next edge.
6. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to create a chain
dimension:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Chain Dimensions
Identify the steps used to create chain dimensions.
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Stacked Dimensions
1
2
3
3
3
1. Select the Stacked Dimensions icon.
2. Select the origin point or edge of your
cumulated system.
3. Select all the other points or edges of your
cumulated system (as many as you
require).
4. Select anywhere on the drawing to
complete the dimension creation.
Use the following steps to create a stacked
dimension:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Stacked Dimensions
Identify the steps used to create stacked dimensions.
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Cumulated Dimensions
1
2
3
3
3
4
Use the following steps to create a cumulated
dimension:
1. Select the Cumulated Dimensions icon.
2. Select the origin point or edge of your
cumulated system.
3. Select all the other points or edges of your
cumulated system (as many as you
require).
4. Select anywhere on the drawing to
complete the dimension creation.
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Cumulated Dimensions
Identify the steps used to create cumulated dimensions.
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Dimension Properties
A
B
C
D
E
A. Dimension line
B. Tolerance description
C. Tolerance
D. Numerical display description
E. Precision
You can control the display of dimensions by
using the Dimension Properties toolbar. You
can customize the following areas of a
dimension:
Step 4 - Create Dimensions and Annotations
Student Guide: 10-57
You can control the display of dimensions by using the Dimension Properties toolbar.
You can customize the following areas of a dimension:
A. Dimension line: Set the display of the dimension line with respect to
the dimension.
B. Tolerance description: Displays the dimension using a tolerance
scheme.
C. Tolerance: Changes the tolerance value for the dimension.
D. Numerical display description: Displays the dimension in a particular
unit.
E. Precision: Sets the precision of the dimension.
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Annotations
A
B
C
D
E
F
A. Text
B. Text with Leader
C. Replicate text
D. Balloons
E. Datum Target
F. Text template
In addition to creating dimensions in a drawing,
you can add notes and annotations to it. The
Text toolbar contains the following tools:
Step 4 - Create Dimensions and Annotations
Student Guide: Lesson 10- Annotations
In addition to creating dimensions in a drawing, you can add notes and annotations to it.
The Text toolbar contains the following tools:
A. Text: Create a textbox with no leader.
B. Text with Leader: Create a textbox with a leader.
C. Replicate text: Create a copy of an existing text box and attribute link
it to geometry.
D. Balloons: Creates a text balloon.
E. Datum Target: Creates a datum target.
F. Text template: Place a predefined text template.
Ensure there are no questions before moving onto the next step.
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Step 5: Save the Drawing
In this section, you will learn to save a
drawing.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 5 - Save the Drawing
Student Guide: Lesson 10- Step 5: Save the Drawing
Introduce the step.
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Matching Drawing with Modified 3D Part
60
40
Step 5 - Save the Drawing
Student Guide: Lesson 10- Matching Drawing with Modified 3D Part
Before saving any drawing, it is a good idea to make sure that it is up to date with the
most recent information.
If the Update icon (shown) is highlighted, this means that the drawing must be updated to
reflect the changes that were made on the 3D part it represents.
In the part shown, for example, the width dimension has been changed from 40 to 60.
Selecting the Update icon regenerates the view with the new dimensions.
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Checking Links to 3D Parts (1/2)
1
1. Click Edit > Links in the menu bar, as
shown.
2. All the drawing views are missing the
same referenced part.
Use the following steps to load a missing
document that is linked to a view:
Step 5 - Save the Drawing
Student Guide: Lesson 10- Checking Links to 3D Parts (1/2)
Its possible that a drawing may be opened without its referenced documents being
loaded in session. This could be caused by a missing file or a global CATIA setting, the
tree identifies this with broken icons.
To update the drawing correctly the links of the drawing need to be verified.
Identify the steps to load a missing document.
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Checking Links to 3D Parts (2/2)
3
4
2
3. Select the Pointed
Documents tab.
4. Select Load to load the part.
5. Update the drawing.
Use the following steps to load a
missing document that is linked
to a view (continued):
Step 5 - Save the Drawing
Student Guide: Lesson 10- Checking Links to 3D Parts (2/2)
Identify the steps to load a missing document.
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Saving a Drawing
• You save a drawing the same way you
would any other CATIA file.
• You can also use the Save As and Save
management tools to store the drawing.
• A drawing is dependent on the 3D part(s) it
represents.
Step 5 - Save the Drawing
Student Guide: Lesson 10- Saving a Drawing
You save a drawing the same way you would any other CATIA file.
You can also use the Save As and Save management tools to store the drawing.
Keep in mind that a drawing is dependent on the 3D part(s) it represents; therefore, it is
important to verify that the parts and drawing is up to date with the most current
information.
Ensure there are no questions before moving onto the next step.
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Step 6: Print the Drawing
In this section, you will learn to print a
drawing.
Use the following steps to
create the drawing:
1. Start a new drawing.
2. Apply a title block.
3. Create views.
4. Create dimensions and
annotations.
5. Save the drawing.
6. Print the drawing.
Step 6 - Print the Drawing
Student Guide: Lesson 10- Step 6: Print the Drawing
Introduce the step.
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Printing a Drawing
•
Click File > Print or select the Print icon to print your drawing.
Step 6 - Print the Drawing
Student Guide: Lesson 10- Printing a Drawing
Click File > Print or select the Print icon to print your drawing.
The Print window contains enables you to customize the layout, page setup, and options.
It also shows a print preview of the drawing.
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Print User Interface (1/2)
A
B
C
D
E
MultiDocuments Tab
Step 6 - Print the Drawing
Student Guide: Lesson 10- Print User Interface (2/2)
The Print window contains the following information, which you can modify:
A. Printer: Select the printer or key in a file name to print to.
B. Position and Size: Define the position and size of the geometry on
the page.
C. Print Area: Define the area to print.
D. Page Setup: Define the page size and characteristics.
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Print User Interface (2/2)
Step 6 - Print the Drawing
Student Guide: Lesson 10- Print User Interface (2/2)
Select the Options button from the Print window to open the Options dialog box:
A. Color
B. Banner
C. Various
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To Sum Up…
Creation of a new drawing
Insertion of a title block
Creation of basic views
Dimensioning and annotating
Saving and Printing
Using the knowledge learned in this lesson, you
should be able to create the drawing of the Base part.
The drawing requires the following details:
Step 6 - Print the Drawing
Student Guide: Lesson 10- To Sum Up…
Review the process to create the drawing.
Ensure there are no questions before starting the exercises.
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Exercise Overview
You will practice what you have learned by working through three exercises.
Exercise 10C
Exercise 10A
Exercise 10B
Exercise Overview
Student Guide: Lesson 10- Exercise 10A, Lesson 10- Exercise 10B, Lesson 10- Exercise
10C
* Demonstrate the topics learned in this part of the lesson before or after students work
on the exercises. Decide when to do the demonstration based on the class. Some will
prefer to see you do a demonstration before, some will prefer to struggle with the
exercises and then see a demonstration after. A demonstration of the topics covered
should include, creating an empty drawing, and front, projection, and isometric views.
Demonstrate the use of the compass and that the isometric view is based on the
orientation of the 3D model. Using a different part, create another drawing, this time
generate the views using the View Wizard. Add the overall dimensions and a title block
to one of the drawings.
* Present the exercises available to practice creating drawings.
* As a class discuss what will be involved in completing the exercises. What tools will
they need to use?
* Tell students where they will be saving the models to and where the required start parts
are located. State that they are to move from one exercise to the next and complete all
three exercises and the case study (time permitting).
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Case Study: Drafting
Using the techniques you have learned in this and previous lessons
create the model without detailed instruction.
You will practice what you learned by completing the case study
model using only a detailed drawing as guidance.
Recall the design intent of this model:
The drawing should be created using an ISO standard.
The drawing should contain one view that shows hidden lines and the axis.
The drawing should contain a title block.
Case Study: Drafting
Student Guide: Lesson 10- Case Study: Drafting
Review the requirements for the case study.
Discuss as a class how the drawing will be created, what tools are needed to create the
case study?
Have the students begin the exercises and note the time.
Assist students as needed with the exercises.
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Instructor Notes:
CATIA V5 Fundamentals - Lesson 10: Drafting
Copyright DASSAULT SYSTEMES
10-65
Copyright DASSAULT SYSTEMES
Exercise 10A: Recap
Create a new drawing
Apply a title block
Add views
Create dimensions
Save a drawing
Exercise 10A: Recap
Student Guide: Lesson 10- Exercise 10A: Recap
Review the Exercise Recap slides after the students have attempted the exercises.
Discuss the different tools used in this exercise.
Ask if there are any questions about this exercise, any difficulties?
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Instructor Notes:
CATIA V5 Fundamentals - Lesson 10: Drafting
Copyright DASSAULT SYSTEMES
10-66
Copyright DASSAULT SYSTEMES
Exercise 10B: Recap
Create a drawing
Insert a title block
Create views using the view wizard
Move and delete views
Dimension geometry
Exercise 10B: Recap
Student Guide: Lesson 10- Exercise 10B: Recap
Discuss the different tools used in this exercise.
Ask if there are any questions about this exercise, any difficulties?
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Instructor Notes:
CATIA V5 Fundamentals - Lesson 10: Drafting
Copyright DASSAULT SYSTEMES
10-67
Copyright DASSAULT SYSTEMES
Exercise 10C: Recap
Create a new drawing
Insert a title block
Add views
Dimension and annotate the drawing
Save the drawing
Exercise 10C: Recap
Student Guide: Lesson 10- Exercise 10C: Recap
Discuss the different tools used in this exercise.
How did the students create the views (using the view wizard or manully)?
What tools did the students use to dimension the drawing. Did they use the Dimension
tool for all of them or did they use the specific tool for the type of dimenion needed?
Ask if there are any questions about this exercise, any difficulties?
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Instructor Notes:
CATIA V5 Fundamentals - Lesson 10: Drafting
Copyright DASSAULT SYSTEMES
10-68
Copyright DASSAULT SYSTEMES
Case Study: Base Recap
The drawing should be created using an
ANSI standard.
The drawing should contain one view that
shows hidden lines and the axis.
The drawing should contain a title block.
Case Study: Base Recap
Student Guide: Lesson 10- Case Study: Base Recap
Discuss the objectives of the case study.
Review the process used to create the drawing.
Ensure the students understand the process used to create the case study before
beginning the master project.
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