Tutorial sobre software Catia

Tutorial sobre software Catia

(Parte 1 de 4)

zCCARD Ltd is an independent consultancy offering CAE hardware and software installation and customisation services, specialising in CATIA and I-DEAS systems.

zCCARD also specialises in Electronic Data Interchange (EDI), and supplies, installs and supports OFTP/Odette based ISDN or TCP/IP solutions.

zIn order to continue to provide its customers with the best products and support,

CCARD has negotiated exclusive access to a CATIA V5 Introduction User Guide, of unique quality and effectiveness, which is ideal as a cost-effective self-study tutorial.

zCCARD can be contacted either by telephone on 024-76-226888 by emailing info@ccard.co.uk or via our website at w.ccard.co.uk

This extract from the CATIA V5 Introduction User Guide zIncludes 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.

zProvides 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.

zAssumes 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, 2004i a mp le - Nov 04

Welcome toi
Table of Contentsi

Overview Page

Starting CATIA for the first time1-1
The Mouse Buttons1-1
Setting Useful Options1-2
File Locations1-3
The Workbench Toolbars1-4
Help with the Command Icons1-6

1. Getting Started

Engine Mechanism2-1
1. Conrod (Part)2-2
2. Block (Part)2-5
3. Piston (Part)2-6
4. Crankshaft (Part)2-8
5. Engine Assembly (Product)2-10
6. Drawing Generation2-13
7. Simple Modifications2-18
Questions and Answers2-20

2. Overview Example

Plate Profile3-1
Questions and Answers3-6
Handbrake Profiles3-7

3. Sketcher Profiles Table of Contents ii© The CAD/CAM Partnership, 2004

1. Planar Support Bracket4-1
2. Suspension Bracket4-7
3. Handbrake Plate4-15
Questions and Answers4-21
4. Patterns of Objects4-24
5. Sports Car Wheel4-29

4. Prismatic PartsPage

Draughting Basics5-1
1. Sheet Frame and Title Block5-2
2. Creating a Section View5-7
3. Draw Details5-8
Questions and Answers5-10
4. Plotting5-13

5. Draughting and Plotting

1. Designing ‘in Context’6-2
2. Inserting Parts in a Part6-8
3. Duplicating Parts within a Product6-12
4. Modifying a Referenced Part6-15
Questions and Answers6-16

6. External References Table of Contents

© The CAD/CAM Partnership, 2004iii

1. On-line Help7-2
2. Exchanging V5 Documents7-4
3. Using a V4 Model as a V5 Component7-5
4. Migrating Multiple V4 Models7-6
5. Messages Explained7-8
6. Questions and Answers7-10
7. Just Testing7-14
8. The CATIA V5 Advanced User Guide7-16
9. The CATIA V5 Digital Mockup User Guide7-17
10. The CATIA V5 Administration User Guide7-18

7. Miscellaneous Page

1. Basic Points to Remember8-1
2. A Review of Examples8-2
3. Modified Options Settings8-4

8. Summary Table of Contents iv© The CAD/CAM Partnership, 2004

2. Overview Example Engine Mechanism

Objective:To introduce the Part Design, Assembly Design and Drafting modules.

the components can then be intelligently assembled, and animatedA drawing

To model 3 simplified engine components, plus part of the engine block, so that 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.

made to geometry in the other Part documentsChanges to one Part document
will therefore not affect the other Parts(It is possible for changes in one

Comments:In this example, each component is created independently, i.e. no reference is Part to automatically be reflected in all related Parts).

© The CAD/CAM Partnership, 20012-1

CCARDS Sam p le -

Nov 04

Assembly ConrodEngine Block

Piston New Crankshaft

1. Activate Part Design2. Choose working 2D plane 3. Create top hole

1. Conrod (Part)

1.Start CATIA

If the Welcome to CATIA V5 window is displayed, then...

Use MB1 to activate Do not show this dialog at start up Select Close to remove this window

Close the proposed Assembly Design workbench window... Select File + Close to close the Product1 window

SelectStart + Part Design to activate the Part Design workbench

A ‘specification tree’ displays: Part1 - the default new Part document name 3 datum planes - which are also displayed as geometry An empty ‘Body’ in which Part geometry can be created

2.Select Sketcher: and then the yz reference plane (or vice-versa)

Note: The yz reference plane can be selected as geometry, or via the specification tree The Sketch plane, by default, rotates to display normal to the screen, as shown

3.Double-click (so as to use more than once) Circle:

First create the top hole for the gudgeon pin... Select the origin point (a temporary blue circular icon must be displayed) as the centre Indicate (using MB1) any point at the approximate location of the circle circumference

Overview Example

2-2© The CAD/CAM Partnership, 2001xy plane yz plane zx plane



4. Create other circles5. Fillet left then right 6. Correct the radius values

1. Conrod (Part) (continued)

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

select the Tools + Options+ Parameters and Measure Parameters Tolerance

Note:Should the radii Constraint values be displayed with a ± tolerance symbol, then tab, and deactivate Default tolerance (for future Constraints)

6.Double-click a fillet curve dimension value Enter the required value (140mm) in the Constraint Definition window

Similarly correct the other fillet curve dimension value

NOTE:As geometry is fully constrained it turns from white to greenWhite geometry

therefore indicates that additional geometrical or dimensional constraints are required to completely specify the profile...

Chapter 2

© The CAD/CAM Partnership, 20012-3

7. Constrain the profile8. Correct the dimensions 9. Create the solid Pad

1. Conrod (Part) (continued)

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 25mm and Ø25mm, vertical offset 150mm, lower: radius 40mm and Ø50mm)

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 16mm (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 Asto 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

1. Create block profile2. Create cylinder shaft 3. Create crankshaft hole

Part of an engine block will be required to support the intelligent assembly of the engine parts...

1.Select Start + Sketcher and select the yz reference plane Note:Starting the Sketcher workbench creates a new Part document

Select Profile: and create orthogonal line segments, ending at the first point

Double-click Constraint: to create dimensional constraints for the profile Double-click each dimension value, and enter the correct/required value (as shown)

2.Select Exit: and then select Pad: Create a prism with a ( -X direction) depth of 70mm

For a new Sketch (you can select the command icon and then a plane, or vice-versa)... Select Sketcher: and then the xy plane (or an existing face parallel to the xy plane)

Select Circle: to define a Ø100mm circle centred at the origin (and then Exit: )

Select Pocket: with Limit Type set as Up to last(Reverse Direction if required)
Use Pocket: with Limit Type set as Up to last(Reverse Direction if required)

3.Create a new Sketch containing a Ø50mm circle centred at the origin on the zx plane

4.Optionally, to define the material of the part...

Select the Part and then select Apply Material: (or vice-versa) Select Metal + Aluminium from the Library window

Use MB3 to select Part1 via the specification tree, and select Properties

Change the Product Part Number to Block Select OK

Select File + Save Asto save the Part as Block

Select File + Close to close the Block document

Chapter 2

© The CAD/CAM Partnership, 20012-5

1. dimension cylinder profile with axis2. Create 360º solid of revolution

3. Piston (Part)

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

reselect (to deactivate) the Profile: command icon

Note:To end the definition of a Profile (which does not finish at its start point),

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 50mm and 35mm, and horizontal offset 50mm)

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 360º, and select OK

Overview Example

2-6© The CAD/CAM Partnership, 2001

3. Define shell thickness operation4. Create gudgeon pin hole and 2mm chamfer

3. Piston (Part) (continued)

3.Select Shell:

Select the bottom face (for removal) Enter an Inside thickness of 10mm

4.Select the yz reference plane and then Sketcher: (or vice-versa)

Select Circle Using Coordinates: Define a 12.5mm radius circle at coordinates 0,0

Note:This circle centre point is fixed - but independent of the origin pointThe

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 2mm chamfer at 45º

Select File + Save Asto save the Part as Piston

5.Use MB3 and Properties to change the Product Part Number to Piston Select File + Close to close the Piston document

Chapter 2

© The CAD/CAM Partnership, 20012-7

1. Define the 35mm oblong profile2. Create Pad and define an R25mm circle

1.Select Start + Sketcher and then select the yz reference plane (This is the most efficient way to start a Sketch for a new Part)

NOTE:Rather than literally sketch geometry, and then return to constrain and correct the arbitrary dimension values, it is possible to enter specific values via the

Sketch tools toolbar menu (which is the one including the Grid icon ).

(To ensure that all of the numerical value entry fields of this menu are visible, then it should be dragged into the main window to create a separate window)

Change the ‘type of profile’ (i.e. fromor etc.) to Oblong:

First select the origin point Enter a length L: of 35mm and then select a point horizontally to the right Enter a radius R: of 35mm

2.Select Exit: and then Pad: Enter a Length (i.e. a ‘thickness’, in the -X direction) of 16mm

Select Sketcher: and then the front face of the pad (or vice-versa)

Select Circle: Select a centre point (anywhere!) and enter a radius R: of 25mm

Overview Example

2-8© The CAD/CAM Partnership, 2001

4. Create concentric R25 x 20mm cylinder5. Create an R25 x 60mm cylinder

4. Crankshaft (Part) (continued)

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 20mm

parallel to the screen so as to be viewed orthogonallyOn leaving the Sketch,
the previous (typically isometric) viewpoint will be reinstatedThis automatic

5.NOTE:Whenever a working plane for a Sketch is defined, it may be rotated to be 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 25mm radius circle centred at the origin

Select Exit: , select Pad: , and then enter a Length (thickness) of 60mm

Select File + Save Asto save the Part as Crankshaft

6.Use MB3 and Properties to change the Product Part Number to Crank Select File + Close to close the Crankshaft document

Chapter 2

© The CAD/CAM Partnership, 20012-9

1. Assemble existing components2. The display mode can be changed

5. Engine Assembly (Product)

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...)

place and constrain a componentHowever, the more flexible approach is to

Note:Alternatively, Existing Component with Positioning: will additionally both 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

3. Fix Block and link Piston/Conrod 4. Move Piston/Conrod 5. Link Parts and rotate

5. Engine Assembly (Product) (continued)

3.Select Fix Component: and then the Block Part (or vice-versa)

Note:By default the component will be fixed absolutely - as indicated by a lock symbol on the fix icon in the specification tree. (MB3 + Properties and the Constraint tab and deactivating Fix in space would instead define the Fix to be only relative to other referenced components)

Select Coincidence Constraint: (the geometry may have to be rotated first...) Select the Piston hole (horizontal proposed axis) and the Conrod top hole (proposed axis)

NOTE:The Piston (first selected Part) would have moved to share axis with the Conrod (second selected Part) if required unless the first Part had been previously fixed

4.Select Manipulation:(or, use the Compass and Shift to drag both components)

Select Drag along Z axis and set With respect to constraints Select either the Conrod or Piston Part, and drag the pair vertically upwards

5.Select Coincidence Constraint: Select the Piston (proposed axis) and then the Block shaft (proposed axis)

Note:The Crankshaft, Conrod and Piston must be rotated together through 90º clockwise before the Crankshaft can be linked to the Block...

Select Contact Constraint: Select the Conrod (rear face) and then the Crankshaft (front face), or vice-versa

Select Manipulation:

Select Drag around Z axis and set With respect to constraints

Select the Crankshaft and drag so as to rotate the 60mm cylinder towards the hole Note that this is very approximate so that part of the hole remains for selection!

Chapter 2

© The CAD/CAM Partnership, 20012-1

Shading with Edges Display mode:

6. Define Crank rotation7. Link Conrod/Crankshaft 8. Centre the Conrod

5. Engine Assembly (Product) (continued)

6.Double-click Coincidence Constraint:

To align the Crankshaft with the Block... Select the Crankshaft (60mm Cylinder) and then the Block (horizontal hole)

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