CATIA V5 Assembly Design

Transcription

© 1997 – 2001 DASSAULT SYSTEMES
Assembly Design
IBM Product Lifecycle Management Solutions / Dassault Systemes
Page 1
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
Tutorial Major Steps
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
Page 3
Settings
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):
? 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
Page 4
?BEFORE STARTING YOUR CATIA V5 SESSION:
? Copy or replace the directory ..\Assembly Design\Data\CATSettings in:
For NT users
C:\Winnt\Profiles\XXXXX\Application Data\DassaultSystemes
For Windows 2000
C:\Documents and settings\Profiles\XXXXX\Application Data\DassaultSystemes
or XP users
For Windows
C:\Windows\Profiles\XXXXX\Application Data\DassaultSystemes
98 users
XXXX is the name used to log on to your computer
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 <CTRL>+O
for open and <CTRL>+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 <CTRL>
? 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 <CTRL> 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 <Enter>
? 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 <CTRL> ( 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 <CTRL> 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 <CTRL> 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 <CTRL> 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:
?Re-size the view
?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:
?Re-size the view
?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:
1
2
? 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
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.
1
? You can turn the assembly around
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

Transcription

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