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This extract from the CATIA V5 Introduction User Guide
z Includes the contents and index pages, together with the full initial worked example , overviews and summary of all examples, of the complete 134 page spirally bound manual.
z Provides an illustration of the style and content of this and other CATIA V5 User Guides compiled and published by The CAD/CAM Partnership - the leading independent CATIA specialist in the UK.
z Assumes the availability of a CATIA V5 workstation with a configuration license (such as ‘MD2’) and also familiarity with the CATIA V5 interface, such as use of the mouse buttons and command icons, in order to follow the initial worked example provided as an isolated sample.
® CATIA is a registered trademark of Dassault Systèmes
© The CAD/CAM Partnership, 2004 i
CCARDS Sample -
Nov 04
Overview Page
Welcome to............................................................ i Table of Contents.................................................... ii
1. Getting Started
Starting CATIA for the first time...................................... 1- The Mouse Buttons.................................................. 1- Setting Useful Options............................................... 1- File Locations....................................................... 1- The Workbench Toolbars.............................................. 1- Help with the Command Icons.......................................... 1-
2. Overview Example
Engine Mechanism................................................... 2-
- Conrod (Part).................................................... 2-
- Block (Part)..................................................... 2-
- Piston (Part).................................................... 2-
- Crankshaft (Part)................................................ 2-
- Engine Assembly (Product)......................................... 2-
- Drawing Generation............................................... 2-
- Simple Modifications............................................. 2- Questions and Answers............................................. 2-
3. Sketcher Profiles
Plate Profile....................................................... 3- Questions and Answers.............................................. 3- Handbrake Profiles................................................. 3-
Table of Contents
ii © The CAD/CAM Partnership, 2004
- Planar Support Bracket 4-
- Suspension Bracket 4-
- Handbrake Plate 4-
- Questions and Answers 4-
- Patterns of Objects 4-
- Sports Car Wheel 4-
- Draughting Basics 5- 5. Draughting and Plotting
- Sheet Frame and Title Block 5-
- Creating a Section View 5-
- Draw Details 5-
- Questions and Answers 5-
- Plotting 5-
- Overview 6- 6. External References
- Designing ‘in Context’ 6-
- Inserting Parts in a Part 6-
- Duplicating Parts within a Product 6-
- Modifying a Referenced Part 6-
- Questions and Answers 6-
- On-line Help 7- 7. Miscellaneous Page
- Exchanging V5 Documents 7-
- Using a V4 Model as a V5 Component 7-
- Migrating Multiple V4 Models 7-
- Messages Explained 7-
- Questions and Answers 7-
- Just Testing 7-
- The CATIA V5 Advanced User Guide 7-
- The CATIA V5 Digital Mockup User Guide 7-
- The CATIA V5 Administration User Guide 7-
- Basic Points to Remember 8- 8. Summary
- A Review of Examples 8-
- Modified Options Settings 8-
- Index Index-
- iv © The CAD/CAM Partnership, Table of Contents
2. Overview Example
Engine Mechanism
Objective: To introduce the Part Design , Assembly Design and Drafting modules. To model 3 simplified engine components, plus part of the engine block, so that the components can then be intelligently assembled, and animated. A drawing will be produced with views of the Crankshaft and the assembly, and the Crankshaft component subsequently modified to illustrate how the assembly model and the drawing reflect these changes.
Approach: A new Part document (file) will be created for each component. The defining profiles will be created and dimensionally/geometrically constrained, typically in the yz 2D plane. The assembly is a Product document which will reference the Part documents.
Comments: In this example, each component is created independently , i.e. no reference is made to geometry in the other Part documents. Changes to one Part document will therefore not affect the other Parts. (It is possible for changes in one Part to automatically be reflected in all related Parts).
© The CAD/CAM Partnership, 2001 2-
CCARDS Sample - Nov 04
Assembly
Engine Block Conrod
Piston New Crankshaft
1. Conrod (Part) (continued)
- Create other circles 5. Fillet left then right 6. Correct the radius values 4. Similarly, create a concentric circle by first selecting the existing centre point ( Hold MB2 and click MB1 , and then move the mouse vertically to zoom out as required) Create a third circle by first selecting a centre point vertically below the origin
(a temporary blue vertical line must be displayed below the V axis)
Note: The ‘ Coincidence ’ of this lower centre point with an extension of the vertical axis
is automatically created as a geometrical constraint (the green circle symbol),
but only if the Geometrical Constraints icon: is active (the default setting)
Create another concentric circle by first selecting the second centre point
5. Double-click Corner:
Select each outer circle and indicate a point to approximately define the left fillet curve Similarly define the right-hand fillet curve
Note: Should the radii Constraint values be displayed with a ± tolerance symbol, then
select the Tools + Options ... + Parameters and Measure Parameters Tolerance
tab, and deactivate Default tolerance (for future Constraints)
6. Double-click a fillet curve dimension value Enter the required value ( 140 mm) in the Constraint Definition window Similarly correct the other fillet curve dimension value
NOTE: As geometry is fully constrained it turns from white to green. White geometry
therefore indicates that additional geometrical or dimensional constraints are
required to completely specify the profile...
Chapter 2
© The CAD/CAM Partnership, 2001 2-
R 109.934 R 113.
H
V H
V
R 140 R 140
H
V
1. Conrod (Part) (continued)
- Constrain the profile 8. Correct the dimensions 9. Create the solid Pad 7. Double-click Constraint:
Select each circular curve and indicate to create radius and hole diameter dimensions
Note: These dimensional constraint values will be arbitrary, for example as shown
Select the horizontal axis and the lower centre point to create the vertical dimension
8. Double-click each dimension value, and enter the required value (as shown) (Top: radius 25 mm and Ø 25 mm, vertical offset 150 mm, lower: radius 40 mm and Ø 50 mm)
Select Exit: to leave the Sketcher and to enable 3D geometry creation...
9. Select Pad: and in the Pad Definition window... Specify a Length of 16 mm (in the positive X direction)
To define the material of the part...
Select the Part and then select Apply Material: (or vice versa) Select Metal + Steel from the material Library window and select OK
Use MB3 to select Part1 from the specification tree Select Properties Select the Mass tab to review the Mass Properties
Select the Product tab, and change the Part Number to Conrod
Select OK
10. Select File + Save As... to display the Save As window
Save the Part as Conrod in the default location (e.g.E:\Catdata\My_work)
Select File + Close to close the Conrod document
Overview Example
2-4 © The CAD/CAM Partnership, 2001
R 140 R 140
R 25 D 25
D 50 R 40
150
H
V
R 140 R 140
R 48. D 67.
D 98. R 71.
H
V
3. Piston (Part) 1. dimension cylinder profile with axis 2. Create 360º solid of revolution 1. Select New: and Part and then select OK
(This is yet another way of starting a new Part)
Select the yz reference plane and then Sketcher: (or vice-versa)
Select Profile: and create line segments with endpoints inline with the vertical axis
Note: To end the definition of a Profile (which does not finish at its start point),
reselect (to deactivate) the Profile: command icon.
Select Axis: and define a line joining the endpoints (Press MB1 to deselect the line)
Double-click Constraint: and create the 3 distance dimensions from the axis Double-click each dimension value, and enter the required value (as shown) (Vertical offsets 50 mm and 35 mm, and horizontal offset 50 mm)
Note: The Axis line is not fixed (it could be dragged away from the vertical axis)
2. To create a solid of revolution from the Sketch profile...
Select ( Exit: and) Shaft:
Note: If the Sketch did not contain an Axis type line, then it would be necessary to
select an axis of revolution, for example the vertical (V) axis.
Verify that the proposed First angle limit is 360 º, and select OK
Overview Example
2-6 © The CAD/CAM Partnership, 2001
50
35
50 H
V
3. Piston (Part) (continued)
- Define shell thickness operation 4. Create gudgeon pin hole and 2mm chamfer 3. Select Shell: Select the bottom face (for removal) Enter an Inside thickness of 10 mm 4. Select the yz reference plane and then Sketcher: (or vice-versa) Select Circle Using Coordinates: Define a 12.5 mm radius circle at coordinates 0 , 0
Note: This circle centre point is fixed - but independent of the origin point. The
location of the circle centre can be moved by modifying the offset dimensions.
Although the circle has been created efficiently, the circle is unlikely to be
moved from the origin in this example, and therefore would have been more
appropriately created as a Circle: using the origin as its centre point.
Select Exit: and then select Pocket: Select More>> to set both Limit Types to Up to last Select OK
Select Chamfer: and the top face or edge (or vice versa) Define a 2 mm chamfer at 45 º
5. Use MB3 and Properties to change the Product Part Number to Piston
Select File + Save As... to save the Part as Piston
Select File + Close to close the Piston document
Chapter 2
© The CAD/CAM Partnership, 2001 2-
4. Crankshaft (Part) (continued)
- Create concentric R25 x 20mm cylinder 5. Create an R25 x 60mm cylinder
4. The circular profile can be defined to be always concentric with an edge of the Pad...
With the circle still highlighted as the current element...
Select Constraint: Select the semi-circular right-hand edge of the Pad Select the proposed dimension value , using MB3 , to replace it with a Concentricity
Select Exit: , select Pad: , and then enter a Length (thickness) of 20 mm
5. NOTE: Whenever a working plane for a Sketch is defined, it may be rotated to be
parallel to the screen so as to be viewed orthogonally. On leaving the Sketch,
the previous (typically isometric) viewpoint will be reinstated. This automatic
presentation of an orthogonal viewpoint does not help to clarify the location of
the Sketch, and is therefore optional...
Select Tools + Options... + Mechanical Design + Sketcher , and in the Sketcher tab... Deactivate Sketch Plane Position sketch plane parallel to screen Select OK to close the Options window
( Normal View: and Isometric View: can obtain the same effect when required )
Select Sketcher: and then the rear face of the 16mm pad (or vice-versa) Create a 25 mm radius circle centred at the origin
Select Exit: , select Pad: , and then enter a Length (thickness) of 60 mm
6. Use MB3 and Properties to change the Product Part Number to Crank
Select File + Save As... to save the Part as Crankshaft
Select File + Close to close the Crankshaft document
Chapter 2
© The CAD/CAM Partnership, 2001 2-
5. Engine Assembly (Product) 1. Assemble existing components 2. The display mode can be changed
The origin/datum of each Part component is initially superimposed...
1. Select Start + Assembly Design to create a new Product (assembly) Document
Select Product1 using MB3 and select Properties
Select the Product tab and change the Part Number to Engine_assy
To assemble the required components...
Select Existing Component: (to be inserted into the current Engine_assy Product...)
Note: Alternatively, Existing Component with Positioning: will additionally both
place and constrain a component. However, the more flexible approach is to
create the relationships between components later, particularly in this example,
where the position/orientation of the components are interrelated...
Ctrl-select the Piston, Crankshaft, Conrod and Block Part documents Select Open
2. Note that at any time the Display Mode can be changed...
Select the current setting, for example, Shading with Edges: and... Select Shading (SHD): for shading without edges Similarly change the Display Mode to Shading with Edges and Hidden edges:
Note: To obtain the Hidden Line Removal type display used to illustrate this manual:
Select Customize View Parameters: for the Custom View Modes window Activate Dynamic hidden line removal and then select OK
Select Shading with Edges: , or, Shading with Edges without Smooth Edges:
Note: Customize View Parameters: also provides an option for another similar
display, but with z Half visible smooth edges , for a less prominent display of
internal ‘edges’ at tangential boundaries
Caution: Engine_assy must remain as the ‘current object’ in the Specification Tree, otherwise,
if instead a Part is current, then the Constraints Toolbar will be dimmed/unavailable...
Overview Example
2-10 © The CAD/CAM Partnership, 2001
5. Engine Assembly (Product) (continued)
- Define Crank rotation 7. Link Conrod/Crankshaft 8. Centre the Conrod 6. Double-click Coincidence Constraint:
To align the Crankshaft with the Block...
Select the Crankshaft (60mm Cylinder) and then the Block (horizontal hole)
7. To connect the Conrod and Crankshaft...
Select the Crankshaft (20mm Cylinder) and then the Conrod (lower hole)
8. The Conrod/Crankshaft are not correctly centred with respect to the Piston...
Select Offset Constraint:
Select the Conrod (face) and then the Block (outer face)
Enter an Offset of 62 mm
9. Select File + Save As... (or Save ), or select the equivalent Save: command icon
If a Save Management window is presented, then select Save As... for the Engine_assy
A Save As window is always presented the first time a document is saved...
Select OK to confirm that the Product document is to be saved as Engine_assy
Optionally temporarily change the Display Mode to Shading with Material:
Select Manipulation: Select Drag around any axis and activate With respect to constraints Select (the proposed axis of) the Crankshaft (60mm Cylinder) Select the Crankshaft and drag so as animate the piston mechanism Select File + Close to close (without saving) the Engine_assy window
Overview Example
2-12 © The CAD/CAM Partnership, 2001
62
6. Drawing Generation 1. New sheet with front view 2. Define plan view 1. Open: the Crankshaft Part
Select Start + Drafting ( + Empty sheet ) and Modify...
Verify that the Standard is ISO and set the Format to A2 ISO (594x420mm)
Also verify that Orientation is Landscape and Scale of sheets is 1 (Select OK in the New Drawing window and OK in the Create New Drawing window)
To determine the Projection Method, select Sheet.1 using MB3 + Properties Verify that the z Create projection views using third angle standard option is current Select OK
Deactivate the Sketcher grid: and Snap to point: options
Select Window + Tile Horizontally to display both Crankshaft.CATPart and Drawing
windows -(the currently active window always displays above the other window)
Select Tools + Options... + Mechanical Design + Drafting and the Layout tab Deactivate View Creation Scaling factor (the display of the View Scale) Select the View tab Verify that the Generate axis and Generate center lines options are active Select OK
Select Front View: and then the front face of the Crankshaft
Optionally select the view frame (using MB1) and drag to a more appropriate location Select the proposed view geometry to generate the Front view
2. Select Projection View: (available in same the group of icons as Front View)
Position the cursor above the Front View Select the proposed view to generate the Top view
Note that the Front view is still the current view (with the red frame)...
Chapter 2
© The CAD/CAM Partnership, 2001 2-
Front view
Top view
Front view
6. Drawing Generation (continued)
- Automatically generated dimensions 6. Redefine the dimensions in the front view 5. Select Generating Dimensions:
The Generated Dimensions Analysis window displays the number of constraints found
(e.g. 7), and how many dimensions were created (e.g. 6) from these constraints.
Select OK
6. In the Top view:
Select the 60 mm dimension ( value ) and then drag the dimension line to the left Ctrl-select the 16 and 20 mm dimensions Use MB3 to select Line-Up and select the 60 mm dimension as the reference Verify that Offset to reference is 0 (in the Line Up window) and select OK
In the Front view:
Select and Delete the vertical 35 mm dimension
To be able to indicate the initial location of a dimension as it is created...
Select Tools + Options... + Mechanical Design + Drafting and the Dimension tab Activate the Dimension following the mouse (ctrl toggles) and select OK
Note that small symbols will indicate the geometry (line, arc or circle) being detected...
Select Dimension: and select the left-hand semicircle Indicate a point to locate the radius dimension Change the Dimension Line format from to
(via the Dimension Properties toolbar - displayed at the top of the screen)
Select Dimension: to create the 35mm dimension between the 2 vertical centrelines
Select and relocate both of the 25mm radius dimensions and their values, and... Change their Dimension Line format to
Chapter 2
© The CAD/CAM Partnership, 2001 2-
6. Drawing Generation (continued)
- Modify view texts, and switch off frames 8. Define tolerance and associated text 7. Ctrl-select the 4 View title texts Set the Font Size to 5 mm and select Bold: and Underline:
To switch off the boundary frames...
Ctrl-select the 4 View frames (or the 4 Views listed under Sheet.1) Use MB3 to select Properties Within the View tab, deactivate Visualisation and Behavior Display View Frame
Note: In fact, the View Frames do not plot, and can optionally remain displayed - since
they are the most efficient means of repositioning a View.
8. In the Top view:
Select (using MB3 ) the 60 mm dimension, and select Properties Within the Value tab... Set the Format Precision (Main value) to 0. Select the Tolerance tab and... Set the Main Value to the TOL_NUM2 format Set the tolerances Upper value: 0.003 , Lower value: -0.002 , Select OK
To enable movement of the dimension value only along the dimension line...
Select Tools + Options... + Mechanical Design + Drafting and the Manipulators tab Activate Move value: during Modification and select OK Select the dimension and then the arrows symbol to move the value vertically upwards
Select (using MB3 ) the 20 mm dimension, and select Properties
Select the Dimension Texts tab and enter (Varies) below the Main Value
Select OK
Overview Example
2-16 © The CAD/CAM Partnership, 2001
Top view
3 5 R2 5 R2 5
R3 5
Front view
Top view
Right view
Isometric view
