CATIA V5 Assembly Drafting

Speaker Drafting 

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© 1997 – 2001 DASSAULT SYSTEMES

Description 

� This Tutorial is an introduction to Assembly Drafting. 

Message 

� To show how CATIA V5 allows the user to automatically generate 

associative drafting from 3D mechanical assemblies produced with CATIA V5. 

� To show a higher productive environment for drawings dress-up and 

annotation 

Duration 

� 45 minutes 

Product Coverage 

� Assembly Design, Generative Drafting 

Tutorial Objectives 

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Step 1 

Here are the major steps of the tutorial: 

� Preparing the assembly 

Step 2 

� Generating projection views 

Step 3 

� Generating a section view 

Step 4 

� Adding dimensions 

Step 5 

� Creating an isometric view 

Step 6 

� Generating an exploded view 

Step 7 

� Generating balloons 

Step 8 

� Inserting a bill of material 

IBM Product Lifecycle Management Solutions / Dassault Systemes 

Tutorial Major Steps 

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Settings 1/2 

Depending on your needs, you may have to modify the CATIA V5 settings (units, default 

directory, visualisation parameters, etc…) 

In order to use the appropriate settings for this tutorial, you have two possibilities: 

1. Do the following operations (simplest one): 

�BEFORE STARTING YOUR CATIA V5 SESSION: 

� Copy or replace the directory ..\Assembly Drafting\Data\CATSettings in: 

For NT users 

For Windows 2000 

or XP users 

For Windows 

98 users 

C:\Winnt\Profiles\XXXXX\Application Data\DassaultSystemes 

C:\Documents and settings\Profiles\XXXXX\Application Data\DassaultSystemes 

C:\Windows\Profiles\XXXXX\Application Data\DassaultSystemes 

XXXX is the name used to log on to your computer 

� Do not forget to put this folder (CATSettings) in read mode: 

� Select the folder (CATSettings) 

� Click mouse button 3 then click on Properties and 

uncheck the Read-only Attribute 

� Select all the files in the folder 

� Click mouse button 3 then click on Properties and uncheck the Read-only 

Attribute 

2. Set them manually: 

� Launch your CATIA V5 session and do the operations from page 32 onwards 

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For this tutorial you also need to install a material catalogue: 

� Do not do this step if you have already done it in getting started or in a previous tutorial 

� Copy the ..\Getting Started\Catalog.CATMaterial file under ..\Program 

Files\Dassault Systemes\M07\intel_a\startup\materials\French directory 


Files\Dassault Systemes\M07\intel_a\startup\materials\German directory 

Settings 2/2 


Files\Dassault Systemes\M07\intel_a\startup\materials\Japanese directory 


Files\Dassault Systemes\M07\intel_a\startup\materials directory 

� Answer Yes in order to replace the old catalogue 

You are now ready to launch your CATIA V5 session 

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� Opening the assembly 

�In the menu bar select File/Open 

�Select 250mm 

Speaker.CATProduct file and click 

on Open button 

� Choosing the Visualisation mode 

�In the menu bar select 

View/Render Style/Customize View 

� Check Edges points, Shading 

and Materials boxes 

� Click on OK button 

� Changing of workbench 


Start/Mechanical Design/Assembly 

Design 

Step 1: Preparing the assembly 

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� Generating numbers 

�Click on Generate Numbering 

icon 

� Select in the specification tree the 

root of the assembly structure 

(250mm Speaker) 

� In the Generate Numbering 

dialogue box panel check the Letters 

option 


�Numbering assembly components 

will allow us later on to generate the bill 

of material in the drawing 


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� Customising the display of the Bill of Material 

� In the menu bar, select Analyse/Bill of 

Material 

� Click the Define formats button to 

customise the display of the Bill of Material. 

�In this panel you can choose the 

properties you want to display for the Bill of 

Material and Recapitulation sections. 

�The Bill of Material (BOM) lists all parts 

and sub-products one after the other. The 

Recapitulation displays the total number of 

parts used in the product 

� In the properties for the Bill of Material 

section click on the Hide all properties icon 

� In the Properties for the Recapitulation 

section, select Number and click on Show 

properties icon 


� Click on OK button to close the Bill Of 

Material panel 


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� Creating an exploded 3D view 

�Click on Create Scene icon 

� Key in Explode in the Edit Scene 

panel 

�Click on Explode icon 


� Click on OK button in the 

information box 

�Exploded views can be used for 

technical documentations to show how 

the assembly components are mounted 

together 

�Click Mouse button 3 (MB3) on the 

3D compass red dot 

� Select Snap Automatically to 

Selected Object option 


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�Expand the specification tree 

�Select in the specification tree the 

Voicecoil part 

�The 3D compass turns to green and 

is snapped automatically onto the part 

�Drag the compass u/x axis to move 

the voicecoil part inside the basket as 

shown in the picture 


Former part 


the Former part on the left of the 

basket part as shown in the picture 


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Spider part 

�Drag the compass u/x axis to 

move the Spider part on the left of the 

Former part as shown in the picture 


Diaphragm part 


the Diaphragm part on the left of the 

Spider part as shown in the picture 


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Surround part 


the Surround part on the left of the 

Diaphragm part as shown in the 

picture 


Dustcap part 


the Dustcap part on the left of the 

Surround part as shown in the picture 


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Magnet part 


the Magnet part on the right of the 

Basket part as shown in the picture 

�Select in the specifications tree the 

Pole Piece part 


the Pole Piece part on the right of the 

Magnet part as shown in the picture 

�Click on Exit from scene icon 

�The scene is now stored in the 

assembly tree under the 

Applications/Scene branch 


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� Generating a front view 

�In the menu bar select File/New 

� In the New panel, select Drawing 


� In the New drawing panel check 

that the standard is ISO, the format 

A0 ISO and the orientation 

Landscape and click on OK button 

�De-activate the Sketcher Grid icon 

from the bottom tool bar 

�Click on Front View icon 

Step 2: Creating projections views 

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� Select Window in the menu bar 

� Select 250mm Speaker.Product 

� In the 3D geometry select the 

planar face of the Basket part 

� Click on the sheet to generate the 

view 

�Drag the red frame of the Front 

view (with MB1) to the lower left 

corner of the sheet 

� Generating a left view 

�Click on Projection View icon 

� Move the mouse cursor on the 

right of the front view and click on the 

sheet to generate the view 

Step 2: Generating projections views 

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� Generating a back view 

�Double click on the blue frame of 

the left view 

�The frame turns to red, meaning that 

it is the active view 

�Click on Projection View icon 

� Move the mouse cursor on the 

right of the left view and click on the 

sheet to generate the view 

Step 2: Generating projections views 

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� Generating a section view 

� Double click on the front view blue frame 

to make it the active view 

� In the menu bar select Windows/Tile 

Horizontally 

� Click on the Offset Section View icon 

� Zoom in on the front view 

� Select the two circles 

� Notice that the section plane appears at 

the second point you select and moves 

dynamically on the 3D part as you create the 

cutting profile on the drawing. This section 

plane will automatically disappear as you will 

double-click to end the cutting profile 

� Double-click to end the cutting profile 

creation 

� Maximize the drawing window by clicking 

on maximize button 

� Zoom out to see the whole page 

� Move the mouse cursor above the front 

view and click to generate the view 

Step 3: Generating a section view 

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� Modifying the section view 

�Even after creation you are still able to 

modify the cut elements of section views 

� Double-click the section view frame to 

activate it 

� MB3 click on the section view frame (or 

in the tree) 

� In the contextual menu select Section 

view AA object & Overload Properties 

� Select the spider geometry on the section 

view (zoom in if necessary) 

� Click on Edit button 

� In the Editor panel uncheck the option Cut 

in section views 


� Click on OK button to close the 

Characteristics panel 

�The spider element is no more cut in the 

section view 

Step 3: Generating a section view 

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� Adding overall dimensions 

�Click on the Dimensions icon 

� Select the basket vertical edge 

�You get a 300mm diameter 

dimension 

� Moving the mouse cursor, drag the 

dimension to a location above the 

speaker geometry and click on the 

sheet 

�Click on the Dimensions icon 

� Select the magnet vertical edge 

�You get a 160mm diameter 

dimension 


dimension to a location below the 

speaker geometry and click on the 

sheet 

Step 4: Adding dimensions 

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� Double-Click on Dimensions icon 

�When you double-click an icon, you keep 

the functionality active 

� Select the horizontal edge of the basket 

� Select the horizontal edge of the pole 

piece 

�You get a 132.8mm distance dimension 


dimension to a location on the right of the 

speaker geometry and click on the sheet 




dimension to a location on the right of the 

speaker geometry and click on the sheet 

�You get a 10.8mm distance dimension 


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Finally, you should have the 

following 4 dimensions on the section 

view 

�Click on the yellow arrow at the top 

right of your toolbars 

�Zoom out to see the whole page 


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�Double-click on the blue frame of 

the front view to activate it 

�Click on Dimensions icon 

(dimensioning toolbar) 

�Zoom in and select the upper right 

external circle as shown 

�Click on the sheet to create the 

dimension 

�In the top toolbar, click on the 

second Dimension Line (dimension 

properties toolbar) icon to change the 

dimension line type 

�MB3 click on the dimension 

� Select Properties 

� Select the Dimension Texts tab 

� In the first field of the Associated 

Text area key in « 6 X » 



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� You get the diameter dimension as 

shown on the figure 

� Click on Centre Line with Reference 

icon (Dress Up toolbar) 

�Please refer to the Getting Started 

scenario to extract the non visible toolbars 

due to the display settings of your screen. 

You have to drag and drop the bottom right 

toolbars until you find the needed one. 

� Select the same circle as the one used 

before for the dimension creation 

� Select any concentric circle of the view as 

a reference 

� Click on Centre Line with Reference 

icon 

� Select the next circle 

� Select any concentric circle of the view as 

a reference 

� Click on Angle Dimensions icon 

� Select the two centre lines 

� Move the mouse cursor above the 

geometry 

� Click on the sheet to create the dimension 


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�MB3 on the angle dimension 

� Select Properties in the contextual 

menu 

� Select the Dimension Texts tab 

� In the first field of the Associated 

Text area key in 6 X 



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� Generating an isometric view 

�Click on New Sheet icon 


Windows/Tile Horizontally 

�In the 3D window, rotate the 

assembly to get a view as shown on 

the right 

�Click in the drawing window 

�Click on Isometric View icon 

(views toolbar) 

� Move the mouse cursor over the 

3D geometry till an axis is displayed. 

When you get this axis click with 

mouse button 1 

� In the drawing window, click 

anywhere on the sheet to generate 

the view 

�Move the isometric view to to the 

upper right corner of the sheet 

Step 5: Creating an isometric view 

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� Generating an exploded view 

�In the lower left corner of the 3D 

window, double click on the Explode 

window to open it 

�If no geometry is visible in the 

window, click on Fit All In icon 

�Click anywhere in the drawing 

window 

�Click on Isometric View icon 

� In the specification tree click on 

Explode 

� Click any planar face, the magnet 

face for example 

� In the drawing window click 

anywhere on the sheet to generate 

the exploded view 

� With mouse button 1 move the 

blue frame of the exploded view to the 

left as shown in the picture 

� Maximise the drawing window by 

clicking on maximize button 

Step 6: Generating an exploded view 

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� Generating balloons on the exploded view 

�Balloons are references defined on the 

different parts of an assembly. They will be 

useful later on when creating the bill of 

material 

� Activate the exploded view with a double 

click on the blue frame of the view 

� Click on Generate Balloons icon 

(Generation Toolbar) 

� Using MB1 move all balloons except B 

above geometry 

� Multi-select (Ctrl Key)all balloons except 

B 

� In the menu bar, select 

Tools/Positioning/Element Positioning 

� Click on Align to Top icon 


Step 7: Generating balloons 

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�You should finally get the following 

balloons disposition 

Step 7: Generating balloons 

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� Inserting a bill of material 

�The bill of material corresponds to 

information on the product element from 

which the views were generated.This Bill of 

Material, or parts list, consists of an 

itemised list of the several parts of a 

structure shown on a CATDrawing or on an 

assembly. 

� In the menu bar select 

Insert/Generation/Bill of Material 

� Click a point on the bottom right corner of 

the sheet to insert the bill of material 

�You can still move the table after the 

generation by dragging it with MB1 

� Changing the views properties 

� In the tree multi-select (Ctrl Key)the 6 

views (holding Mouse Button 1 and Shift 

key) 

� With MB3 select Properties 

� Uncheck Display view frame box 


Step 8: Inserting a bill of material 

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� Adding a title block 

�In the menu bar select File/Page Setup 

� In the Page Setup panel select All sheets 

in the list 

� Click on Insert Background View… 

button 

� Click on Browse button 

� Select A0 Title Block.CATDrawing file 

� Click on Open button 

� Click on Insert button 

� Click on OK button in the Page Setup 

panel 

�A previously defined A0 title block is inserted 

in the background view of the two drawing 

sheets 

�In the menu bar select Edit/Background 

�Double click on XXX characters in the 

DESIGNED BY area 

� In the Text editor panel, key in your name 


Step 9: Adding a title block 

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Manual Settings 

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� Setting the CATIA options 

�Start CATIA V5 


Tools/Options 

�Select Mechanical 

Design/Drafting chapter and Layout 

tab 

� Check/uncheck the boxes as 


Setting the CATIA options 

Page 32 


�Select Mechanical 

Design/Drafting chapter and 

Generation tab 

� Check/uncheck the boxes as 


Setting the CATIA options 

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Congratulations 

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