CATIA V5 Assembly Design

Assembly Design 

IBM Product Lifecycle Management Solutions / Dassault Systemes 

Page 1 

© 1997 – 2001 DASSAULT SYSTEMES

Tutorial Objectives 

Description 

? This Tutorial is an introduction to Assembly Design. 

Message 

? Assembly Design is easy to use and powerful. The basics of product 

structure, constraints, and moving assemblies and parts can be learned 

quickly. 

? In this tutorial you will understand the power of associativity in CATIA V5, 

creating design in context and realising operations directly in the assembly 

design. 

? We will see the facility to use sub assemblies and constraints. 

Duration 

? 45 minutes 

Product Coverage 

? Assembly Design, Part Design 


Page 2 


Here are the major steps of the tutorial: 

Step 1 

? Add a part into an assembly 

Step 2 

? Fix create constraints between this new part and other parts 

Step 3 

? When the tweeter is inserted, repeat this operation with the woofer 

Step 4 

? Create Holes in the Box to add screws 

Step 5 

? Add screws from a catalog 

Step 6 

? Modify the size of the Box and check the associativity 

Step 7 

? Assembly Feature 

Step 8 

? Manipulation with respect to the constraints 

Step 9 

? Exploded view 

Step 10 

? Hyperlinks 


Tutorial Major Steps 

Page 3 


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 Design\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 

Settings 

? 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 50 onwards 

IBM Product Lifecycle Management Solutions / Dassault Systemes Page 4 


Settings 2/2 

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 


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 


Page 5 


Start Scenario 

We will work on the product that appears when 

CATIA starts 

? CATIA starts in the Product Structure 

workbench with Product1 selected in the tree 

?Select Start + Mechanical Design + 

Assembly Design to access the assembly tools 

? Here we will change the name of the product 

?Click on the “Product1” name in the 

specification tree 

?Click MB3 + Properties to display the 

Properties dialogue box 

?Select Product tab 

?Double-Click in the Part Number field 

?Enter “Loudspeaker” instead of Product1 

?Click OK 


Page 6 


Step 1: Open the Box 

Opening an existing part 

? Opening Two_Way_Box.CATPart 

?File + Open in the Menu Bar 

? CATIA also supports Windows 

standard hotkeys such as +O 

for open and +N for new 

?Select Show Preview to preview a 

part or an assembly 

? You can preview your models 

before you open them. Notice the 

preview is very fast. This is because 

you are only reading the image in the 

NT metafile 

?Select Two_Way_Box.CATPart in 

the … \Assembly Design \Data\ 

directory 

? The path will depend on where you 

installed the data 

?Click Open 


Page 7 


Step 1: Customise a Hotkey 

Customising a Hotkey 

? You could use the pulldown Window-Tile 

Vertically to do this action, but we would like you 

to take a moment to see how easy it is to create 

a Hotkey 

? Click MB3 on any icon and choose 

Customize from the contextual menu 

? You can also use Tools + Customize in 

the Menu bar 

? Select the Commands tab 

? Select Window on the left part of the 

window 

? Select Tile Vertically on the right part of 

the window 

? Click on Show Properties button 

? Enter F4 into Accelerator 

? Click Close 

? You can check the result of your customisation 

? Hit F4 to tile your windows vertically 


Page 8 


Step 1: Add first part to assembly 

Dragging and dropping the part into the product 

? You will insert the Part into the Assembly 

? Select the side or front face of the Box and drag it 

onto the top of the tree in the assembly window 

(holding MB1) 

? You will see a ‘+’ on your cursor as shown 

? You could also have selected Two_Way_Box at the 

top of the part tree and dragged it onto Loudspeaker at 

the top of the Assembly tree 

? Now you will continue inserting and constraining further 

parts in the assembly window 

? Maximise the assembly window (Product.1) 

? Select Fit all in 

? Select Fix Component icon 

?If you don’t see the icon, it means that the 

corresponding toolbar is hidden due to your display 

settings. To find it, drag and drop the empty area from 

the bottom right side to the centre of the 3D view. 

Repeat this operation until you find the right toolbar. To 

put it back, do the reverse operation 

? Two_Way_Box.CATPart is already selected 

? Click on the ‘+’ sign of the Constraint line to display 

the constraints you have created 


Page 9 


Step 1: Use the Hide/Show mode 

? You will now see that you can use 2 layers in 

the 3D view: the Show view and the No Show 

view. The No Show view is used to store all the 

unneeded elements. 

? Select the Anchor in the 3D view or the 

Fix.1 (Two_Way_Box.1) line in the tree 

? Click on the Hide/Show icon on the 

bottom toolbar to hide the constraint 

visualisation 

? We will temporarily hide this constraint. 

Notice the constraint is now greyed out in the 

tree as well as hidden in the geometry view 

? Click on the Swap visible space icon 

? This displays the No Show layer 

? You should now see the constraint and the 

geometry used to create the box 

? Click Swap visible space again to go 

back to the Show view 

? Select Fit All In 


Page 10 


Step 2: Add the Tweeter to the Assembly 

Adding the Tweeter to the Loudspeaker 

? Now you are in the right workbench, you 

can insert the tweeter 

?Click MB3 on Loudspeaker at the 

top of the tree or the Existing 

Component icon 

?In the contextual menu choose 

Components + Existing 

Component… 

?In the Insert an Existing 

Component window, Open 

…\Assembly Design \Data\ 

tweeter\tweeter.CATProduct 


Page 11 


Step 2: Move tweeter in assembly 

Moving the Tweeter 

? You can roughly position a part using the 

Compass ( At the top right of the screen ) 

? Place the mouse cursor on the red dot of 

the Compass 

? When the cursor becomes a cross, hold 

down MB1 

? Drag the Compass onto the front face of 

the tweeter sub-assembly then release MB1 

? The compass will turn bright green, 

indicating that it can be used to move the part 

? Place the mouse cursor on the vertical 

axis and when it turns orange, hold MB1 

and drag the tweeter outside the box 

? Using the other axis of the Compass, 

repeat the operation to position the tweeter 

as shown 


Page 12 


Step 2: Move tweeter in assembly 

Moving the Tweeter 

? You can also rotate a part… 

?Select here to rotate the tweeter 

~30° clockwise about the x axis 

?Drag the red dot compass away 

from the tweeter holding MB1 and 

shift 

? Shift resets the compass (z axis 

up) 

?Click MB3 on the face of the 

tweeter. Select Reframe On to zoom 

in on the tweeter 

?Click off the geometry to deselect 

the tweeter face 


Page 13 


Step 2: Add constraints 

Creating Coincidence Constraints 

? You’ll now fix some assembly constraints 

? Select Coincidence Constraint icon 

? Select these 2 cylindrical surfaces (both 

internal hole faces) 

? DO NOT HESITATE TO ZOOM on these 

faces to be sure you select them (please 

refer to the Get Started scenario to find out 

about zooming) 

? The tweeter will snap into place 

? Select these 2 cylindrical surfaces (both 

internal hole faces) while holding 

? Select Coincidence Constraint again 

? The tweeter will rotate into place 

? You have seen two ways for the creation 

of a constraint : icon – object / object - icon 


Page 14 


Step 2: Add Constraints 

Creating Contact Constraints 

? Now you have created some 

coincidence constraints, you will create a 

contact constraint to finish mounting the 

tweeter on the box 

?Click on the Contact Constraint 

icon 

?Select this face on the tweeter 

?Select this face on the box 

? The tweeter will snap into place 


Page 15 


Step 2: Hide Constraints 

Hiding constraints and planes 

? As before, you can make the view 

clearer by moving the new constraints 

onto the No Show layer 

?Holding the key Select 

Constraints from the tree and this 

plane from the geometry 

?Select Hide/Show icon 


Page 16 


Step 2: Assembly level associativity 

Modification of one part 

? You will now use both views: The Assembly 

context view and the Part context view. You need 

to modify the dimension between the two holes 

because they are too close 

? Windows + Tile Vertically in the menu 

bar or Hit F4 key if you already have gone 

through the Part Design scenario where you 

learn how to create a Hotkey 

? In the Part window (Two_way_box 

.CATPart ) double-click the internal face of 

the tweeter hole 

? Double-click the 223 dimension value 

? Move the definition panel to see the 223 

dimension value. 

? Modify it from 223mm to 240mm and 

press 

? Select OK in Hole Definition dialog box 

? Click inside the assembly window 

? “Notice the tweeter automatically moves to 

fit the hole. This is an example of Assembly 

level associativity. 

? Maximise the assembly window 

? Zoom out or Fit All In to show the entire 

speaker 


Page 17 


Step 3: Add Woofer to assembly 

Adding the Woofer to the Loudspeaker 

? Now you will repeat the operation for the 

Woofer 

? Click MB3 on Loudspeaker at the top of 

the tree 

? Click the Existing Component icon 

? Preview the parts that make up the woofer 

? Select … \Assembly Design\ 

Data\250mm Driver.CATProduct 

? Click Open 

Moving the woofer 

? Drag the compass onto the Diaphragm of the 

woofer 

? The compass should be as shown 

? Click MB3 on the compass and choose 

Edit 

? Type in 350 

? The x direction is already selected. 

? Click Apply new position 

? Select Close in Compass Manipulation 

dialog box 

? Drag the compass away from the woofer 

? Click anywhere in the background to deselect 

the geometries 


Page 18 


Step 3: Constrain woofer 

Creating Coincidence Constraint 

? Adding a coincidence constraint 

?Select Coincidence Constraint 

icon 

?Click MB1 to select this cylindrical 

surface on the Diaphragm 

?Click MB1 to select this cylindrical 

surface on the box 

Creating Contact Constraint 

? Adding a Contact constraint 

?Select Contact Constraint icon 

?Select this face on the woofer 

? If the orientation of the view is not 

as shown, you can rotate the view 

?Select this face on the box 

? The woofer should snap into place 


Page 19 


Step 3: Parallelism Constraint 

Creating Parallelism Constraint 

? To show you some other possibilities, 

we will create a parallelism constraint to 

orientate the Woofer into the Box 

?Select Angle Constraint icon 

?Select the plane from the box 

?Select the plane from the woofer 

?In the Constraint Properties 

window, check Parallelism 

? If this were not a symmetrical part 

you could select the green arrow to 

rotate it 

?Click OK 


Page 20 


Step 3: Hide constraints and planes 

Hiding constraints and planes 

? You can now Hide the new constraints 

?Holding ( on the key 

board ) select the plane on the woofer 

and the 3 constraints at the bottom of 

the tree 

?Click MB3 and select Hide/Show 

?Hit F3 to hide the tree 

?Double-click the box in the 

geometry view 

? This will bring us into the part 

Design workbench. 

? We are now editing the box in the 

the assembly view 

? Click MB2 on the hole to re-centre on it 

?Zoom in on this hole 


Page 21 


Step 4: Part Design in the assembly view 

Making a hole in the box 

? Use the assembly view to create the corresponding 

holes in the Box part 

? Select this edge 

? Hold and select this surface 

? We are going to put a hole in the box that will stay 

concentric to this hole in the woofer 

? Select Hole icon 

? Answer Yes to the question if it appears 

? The link between the hole of the Box and the circle of 

the Woofer hole will remain. Any modification made to the 

hole in the box will also be applied to the hole in the 

woofer 

? Select Up To Next 

? Selecting Up To Next means that if we modify the 

thickness of box, the hole will be adjusted accordingly 

? Enter 4mm in the Diameter field 

? Select Positioning Sketch to check the 

concentricity 

?You can see that a coincidence constraint has been 

automatically created 

? Select Exit Workbench icon to exit the sketcher 

? Click OK to close the Hole Definition window 


Page 22 


Step 4: Part Design in the assembly view 

Patterning the hole 

? You will now create a series of holes around the woofer 

axis 

? Click and hold MB1 on the black arrow at the 

bottom right of the Rectangular Pattern icon 

? Drag the mouse then release MB1 on the Circular 

Pattern icon 

? Select Complete Crown in the Parameters field 

? Click MB3 on Instance(s) field and select Edit 

Formula 

? Select one of the 3 other holes on the woofer (not 

where the hole is apply ). 

? You will need to pan down 

? Select Number of Holes 

? External parameter selection dialogue box 

? Select OK to close External Parameter selection 

window 

? Select OK to close Formula Editor window 

? Select the Reference element field 

? Select the cylindrical surface of the box shown as 

the reference element 

? You may have to zoom in on this area to select the right 

face 

? Select YES 

? Select OK 

? The hole pattern on the box is driven by the hole pattern on 

the woofer 


Page 23 


Step 4: Assembly Level associativity 

Illustrating assembly level associativity 

? As the number of holes are linked, any 

modification of the number of Woofer holes will 

have the same result for the Box ones 

? Double click the hole in the woofer 

?The hole you are already zoomed in on 

? This brings us into Part design for the 

woofer 

? Double click again on it to edit the 

definition of the circular pattern 

? Zoom out to see the holes 

? Change Instances from 4 to 6 

?Use the up arrow or enter the value 

? Select OK 

? Notice the box has turned bright red 

indicating the hole pattern should be updated 

to match the pattern in the woofer 

? Hit F3 to show the tree 

? Double click Loudspeaker at the top of 

the tree 

? the links are automatically updated and 

you enter the Assembly Design workbench 

? Zoom in to add the first screw to the hole 

as shown 

? Next we will add screws to the assembly 

using a standard parts catalog 


Page 24 


Step 5: Insert screw from catalog 

Inserting screw from catalog 

? You will now insert some screws into the 

series of holes 

? Select the Catalog Browser icon 

? Remember to put the bottom toolbar out to 

find the missing icons… 

? Select Browse another catalog button 

? Find and Double-click … \Assembly 

Design\Data\ISO_4762.catalog 

? You don’t have access to the Standard 

Part catalog because you are in a 

Demonstration Mode. If you want to use 

the Full provided Catalog, do not hesitate 

to contact your Business Partner 

? Drag and drop ISO 4762 screw M5x20… 

into Loudspeaker at the top of the tree 

? You see the screw in the tree but not in 

the 3D view. This is normal… In fact, the 

screw is inside the Loudspeaker… In the 

next step, we will move it. 

? Close the Catalog 


Page 25 


Step 5: Assembly Constraints 

Moving the screw 

? Position the screw to create the 

constraints 

?Drag the compass onto the front of 

the speaker 

?Select Screw from tree 

?If not already selected 

?Dragging the compass, select 

either a green axis or a blue plane 

and move the screw to its 

approximate position 

?When you are satisfied with the 

position of the screw, drag the red dot 

of the compass away from the 

tweeter holding MB1 + shift 

? Shift resets the compass (z axis 

up) 


Page 26 


Step 5: Assembly Constraints 

Constraining the Screw 

? Create a Coincidence constraint between the 

screw and the hole axis 

?Select the Coincidence Constraint icon 

?Select the cylindrical surface of the screw 

?Select the internal cylindrical surface on 

woofer 

? The screw snaps into place 

?Select the Contact Constraint icon 

?Select the flat face on the woofer hole 

?Select the flat face on the screw 

? Don’t hesitate to rotate the assembly using 

MB2 + MB1 (see Get Started exercises) then 

select the back face of the screw 


Page 27 


Step 5: Align screws with reference pattern 

Aligning the screws with the reference 

pattern 

? Here you will reuse the existing pattern to 

create as many screws as you have holes 

? Select the screw in 3D Geometry View 

? Select Reuse Pattern icon 

? Select here 

? Select this hole on the woofer 

? Check All under Re-use Constraints 

? Select OK 

? We now have 6 screws with their 

constraints. You cam reduce the Constraints 

tree by clicking on the (-) sign 

Creating another series of screws 

? Duplicate the screw using an existing one 

? Hit F3 to show the tree 

? Drag the last screw into Loudspeaker in 

the tree holding key 

? You should see a “+” sign 

? This will create another series of screws 

? Move the compass onto the face of the 

box 

? Select the last screw in the tree 

? Hit F3 to hide the tree 

? Drag the compass to move the screw 

near the tweeter 


Page 28 


Step 5: Screw in the Tweeter 

Constraining the screw 

? Creating the constraints 

?Select Coincidence Constraint 

icon 

?Select the cylindrical surface on the 

screw 

?Select the cylindrical surface on the 

tweeter 

?This time we are using the top left 

hole, which is #4 in the pattern 

? The screw snaps into place 

?Select Offset Constraint icon 

?Select the flat surface on the 

tweeter 

?Select the flat surface on the far 

side of the screw 

?Rotate the view if necessary 

?Set Orientation to Opposite 

?Set Offset to 0 

?Click OK 


Page 29 


Step 5: Align screws with reference pattern 

Aligning the screws 

? Creating and positioning the 3 other screws 

? The coincidence constraint is already 

selected 

? Select Reuse Pattern icon 

? Select All under Re-use Constraints 

? Click OK 

? We now have 10 screws with their 

constraints 

? This time we did not have to select the 

pattern, as the hole in the tweeter is already a 

member of the pattern 

? Hiding all the constraints 

? In the tree, select all the constraints you 

have just created and the three planes. Use 

the key (for multi selection) and 

click on the Hide/Show icon 

? The speaker is now complete. Let’s see 

what it looks like with another box 

configuration 


Page 30 


Step 6: Design Table 

Designing Table 

? Modify the height of the Box 

? Double-click the side of the box 

? This brings us into Part Design 

? Double-click on Configuration in the 

tree 

? Select this button in the window 

? Double click on line 2 

? Click OK 

? The assembly needs to be updated 

? Double-click on Loudspeaker at the top 

of the tree 

? This will update the locations of the 

woofer, tweeter and the screws 


? Play a MP3 on your PC 

? Select View + Full Screen 

? Click MB3, then select Full Screen again 

to exit the Full Screen view 


Page 31 


Step 6: Design Table 

Designing Table 

? Return to the first size: 

? Double-click the side of the box 

? This brings us into Part Design 

? Double-click on Configuration in the 

tree 

? Select this button in the window 

? Double click on line 1 

? Click OK 

? The assembly needs to be updated 

? Double-click on Loudspeaker at the top 

of the tree 

? This will update the locations of the 

woofer, tweeter and the screws 


? Play a MP3 on your PC 

? Select View + Full Screen 

? Click MB3, then select Full Screen again 

to exit the Full Screen view 


Page 32 


Step 6: Facultative point 

Facultative point: 

? If you had not enough time or if you had 

failed the steps before, you can load the 

following file: 

?Close all the windows present in 

CATIA V5 

?Select file open 

? Find Loudspeaker product 

?Click Open or double click on 

Loudspeaker.CATProduct in 

../Assembly Design/Data/Step 7. 

? You are now able to continue the 

script. 

End of the facultative point 


Page 33 


Step 7: Assembly Feature 

Insert a support 

? Import the support: 

?Re-size the view 

?Double-click on Loudspeaker at 

the top of the tree 

? It will be highlighted in orange 

?Use the contextual menu on the 

Loudspeaker to insert a component. 

? MB 3 on Loudspeaker, and then 

Component/Existing Component 

?Select the Support.CATProduct 

In …\Assembly Design\Data\ 

? You can focus your research on 

CATProducts, using “Files of type” : 

Products(*.CATProduct) 

?Click OK 

? The support is on the speaker. 


Page 34 



? Delete the fix constraint on the box 

?Click on the constraint in the tree 

? It will be highlighted in orange 

?Press the key < Delete > on your 

keyboard. 


Page 35 



Positioning 

? Move the imported product: 


?Drag and drop the compass on the 

support in the 3D view 

? Place the compass on the 3D 

geometry. 

?Click on support in the tree to 

highlight it 

? The support can be now moved 

entirely. 

?Select the z axis on the compass 

to move down the support 

? Drag and drop the compass until 

it’s in the right place. 

?With a drag and drop, replace the 

compass on the bottom right axis. 


Page 36 



? Create automatically the coincidence 

constraints: 


?Click on the Quick Constraint icon 

? This is a smart tool, which will 

recognise automatically the type of 

constraint regarding the type of 

geometry chosen. 

?Click the constraints: 

? You must zoom on the holes, as in 

the picture. When you approach the 

cylinder, CATIA will automatically 

detect the axis 

?Click on the two holes, as in 

picture 1 

?Click again on the Quick 

Constraint Icon 

?Click on the two holes, as in 

picture 2 


1 

2 

Page 37 



? Create automatically the contact 

constraints: 

?Click on the Quick Constraints 

?Click on the first face, as in the 

picture. 

? You must move the geometry to 

have a good view. 

?Stay at the “3D view” and approach 

the cursor on the second face, use 

the up arrow on the keyboard once, 

and then approach the cursor on the 

centre of the arrows. A circle will 

appear, click on it to accept the 

selection. 

? You can turn the assembly around 

1 

and select the face directly. 


2 

Page 38 



Split 

? Select the cutting element: 

?Open the tree, as in the picture 

?Click on the Split icon and select 

the join in the open body of Rotator 

Axis 

? This join will be the cutting 

element 


Page 39 



? Impact the Box : 

?Select the Two_Way_Box in the 

top panel. 

?Use the arrow to confirm your 

choice 

? The single arrow not the double 

?Change the direction by clicking on 

an orange arrow 

? As in the pictures 

?OK in the split Definition 

? If the panel Split Definition is not available 

move the Panel Assembly Feature Definition 

using a drag and drop on the top blue bar. 


Page 40 



See the result 

? Hide / Show the support to see the 

result: 

?Click on Support in the tree and 

then click on the Hide / Show icon 

? We see the impact of the split on 

the Two Way Box 

?Do the same 

? We have the entire Assembly now. 

?In the tree, select the 

Two_way_box, then with the 

contextual menu on it ( MB 3 ), select 

Components/Isolate Part. 

? You can isolate the parts from the 

links we created before at any time. 


Page 41 


Step 8: Manipulation with respect to the contraints 

Manipulation 

? Flexible Sub-Assembly: 

?Change the sub-product Support 

as a Flexible Sub-product, MB3 on 

Loudspeaker support in the tree, and 

click on Flexible/Rigid 

? We are now able to use the 

constraints inside the sub-product 

starting from the global product. 

? Also note that the icon in the tree 

has changed for another one in 

purple. 

?Select the manipulation Icon 

?Switch the button : 

With respect to constraints 

?Select the icon axis rotation. 

?And then select the axis as the 

picture by clicking on it. 

?Zoom back 


Page 42 


Step 8: Manipulation with respect to the contraints 

?Catch the two_way_box and turn it 

? You will perform a drag and drop, 

but without the drop. 

? When you find a position, just drop 

the cursor. 

?The manipulation is finished 


Page 43 


Step 9: Exploded View 

?We will create a scene where an 

exploded view will be realised. So 

click on this Icon 

?Select the name of your scene 

? Exploded view 

?Click OK twice. 

? You are now in the scene area, 

which has a green background 

?Select the exploded icon 

?Click on Loudspeaker in the tree 

? De-select the entire product 

?Select all the following designs by 

clicking on them in the tree: 

? You will obtain the following panel 


Page 44 



?Select the fixed product table 

? It will be highlighted in blue 

?Select the Two_Way_box in the 

tree 

?Change the Depth Definition for 

First level 

? The sub assembly will move as a 

whole - not as parts. 

?Click on Apply 

?Click on the left arrow to return to 

the previous step. 

?Click on the right arrow to chose 

the final exploded view and then click 

OK 


Page 45 



?Leave the scene by clicking on the 

exit Icon: 

? We are now in Assembly Design 

?We can now return at anytime to 

the exploded view by double clicking 

on the small view at the bottom left of 

the CATIA window. 

? The exit will be like before 


Page 46 


Step 10: Hyperlinks 

? Re-size the view 

? Select the Flag Note Icon 

? This item creates hyperlinks between 

CATIA and other Files 

? Select the top of the box 

? Change the Name of the Hyperlink 

? Change to “Hyperlink” 

? Click on the Browse… Button and open 

the following files : 

250mmPlan.pdf 

Characteristic.pdf 

In …\Assembly Design\Data\ 

? You can now switch the Go to button to 

activate the link and open the file. 

? Click on a line in the panel to activate 

the Go to button, and then click to active 

the link. 


Page 47 


Step 10: Hyperlinks 

?Click OK in the panel 

?MB3 on the Flag in the 3D view 

?Select the properties 


Page 48 


Manual Settings 


Page 49 


Settings 

Tools/Options 

? We will configure the environment of 

CATIA 

?Select Tools + Options menu 

? We will erase any previous 

configurations. 

?Click on General 

?Click on the Reset Bottom 

?Select for all the tabpages 

?Click YES 


Page 50 


Settings 

Tools/Options 

? Under General select Parameters on 

the tree 

?Select to check With value and 

With formula 

? Under Infrastructure select Product 

Structure on the tree 

?Select to check : 

Automatic Expand 

Parameters 

Relations 

Products 


Page 51 


Settings 

Tools/Options 

? Under Mechanical Design select Part 

Design on the tree 

?Select the General folder 

?Select Keep link with selected 

object 

?Select Confirm when creating a 

link … 

?Select the Display folder 

?Select Constraints, Parameters, 

Relations 

? That’s all for the configuration 

?Select OK at the bottom right 


Page 52 


CONGRATULATIONS 


Page 53

CATIA V5 Assembly Design

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