Instructions for Designing a Wheel in CATIA V5

Required tools

-Must have access to a working computer
-Computer must have CATIA V5
-Computer must be equipped with a keyboard and a 3 button mouse


-User must be acquainted with simple computer navigation
-User must follow each step in the specified order

Step 1: Start CATIA V5 on Your Computer

Home Screen opens upon startup – CLOSE THE SMALLER WINDOW

Step 2: Naming the Part

Select Start > Mechanical Design > Part Design

Name your part and click OK

NOTE: All boxes must remain checked/unchecked as shown in the image

Step 3: A New PART Window Will Open

A new PART window will open – This is where we do all our designing

Step 4: Navigation Control in CATIA

1.   Click WHEEL and move mouse to PAN

2.   Click WHEEL AND RIGHT and move mouse to ROTATE

3.   Click WHEEL AND RIGHT, Release RIGHT and move mouse to ZOOM

Step 5: Standardize the Control Setup

Click Tools > Customize > Toolbars > Standard > Restore all Contents
Click OK
Click Restore Position
Click OK

Step 6: Starting First Sketch

Click ZX plane from Top Left >  (sketch icon) from the Top Right Corner of the Page

Step 7: Deselect the Snap to Point Option From Bottom of the Screen

Make sure that the other options of the sketch tools toolbar are selected/deselected as shown

Step 8: The Sketch Screen Opens

Double Click  the Profile icon from the Profiles toolbar on the Right Side of the screen

Step 9: Draw the Straight Part of the Wheel Profile

Click in the sketch region to start profile > drag horizontally right > click
drag vertically down > click > drag horizontally right > click
drag vertically down > click > drag horizontally right  !!Do NOT Click Further!!

Step 10: Draw the Curved Part of the Wheel Profile

Click and Hold > drag towards the top right >  Release Hold > click and Hold at an
upward curve > drag top right again !!Do NOT Release Yet!!

Step 11: Draw the Straight End Part of the Wheel Profile

Release Hold > click at a downward curve > drag vertically upward > click > drag
Horizontally right > click > Press Esc on Keyboard twice

Step 12: Finished Profile Sketch

Step 13: Dimensioning the Sketch

Double Click the Constrain Icon from the Constraints Toolbar on the right side of the page

Step 14: Dimensioning the Sketch

Step 15: Positioning the Sketch

Click first flat line > click ‘H’ > drag > click > Click first Vertical line > click ‘V’ > drag > click  >> double click and change values for both

Step 16: Dimensioning the Sketch

Click Start point of curved section > click End point of curved section > drag away > Right click > select Horizontal Measure > click

Double click new horizontal dimension > set to 80 

>> Press Esc twice on Keyboard

Step 17: Fully Constrained Sketch

NOTE:  A fully dimensioned and positioned sketch is GREEN in color

Step 18: Exiting the Sketch

Click the Exit Sketch Icon from the Workbench Toolbar on the right side of the page

Step 19: The Main View With Sketch Selected

Click the Sketch name from the Part Tree on the Left side >> sketch turns Orange

Step 20: Creating the Wheel Rim

Click the Shaft icon from the Features toolbar on the right side of the page

Step 21: Creating the Wheel Rim

In the Dialogue Box for Shaft Definition :     Click Thick Profile > click Selection > click on ‘H’

Step 22: Creating the Wheel Rim

Select OK

Step 23: Sketching the Central Lug

Select the Highlighted Planar surface > Click the Sketch Icon from the right side toolbar

Step 24: Sketching the Central Lug

Click on the Circle tool from the Profile Toolbar > Click on the center point (intersection of ‘V’&’H’) > Drag away as shown > click

>> Press Esc twice on your keyboard

Step 25: Dimensioning the Sketch

Click the Constrain Icon from the Constraints Toolbar on the right side of the page
> Click on the circle > drag away > click > double click dimension > correct dimension > click OK
>> Press Esc twice on your keyboard >> select Exit Sketch from right side

Step 26: Making the Central Lug From Sketch

Select the sketch > Click Pad icon from features toolbar

Step 27: Making the Central Lug From Sketch

Correct the dimension > Reverse Direction if required (needs to point into the wheel) > click OK

Step 28: Sketching the Spoke

Rotate : Press mouse wheel and right button > drag mouse

Rotate to back view > Select back face of lug > select sketch icon from the toolbar

Step 29: Sketching the Spoke

Double Click on the Project 3D elements tool from the Operation Toolbar > Click on the innermost diameter of the Rim (should turn YELLOW)

>> Press Esc twice on your keyboard

Step 30: Sketching the Spoke

Double Click the Line button from Profile toolbar > Click the VH Intersection > click the yellow line (it will change color when accurate) towards the left of the ‘V’ > click the VH intersection again > Click the yellow line (changes color) towards the right of the ‘V’

Step 31: Dimensioning the Sketch

Click the Constrain Icon from the Constraints Toolbar > Click the left line > click the ‘V’ > drag away > click > double click dimension > correct dimension > press OK

   >> repeat for the right line

Step 32: Editing the Sketch

Click the Black triangle below the Trim icon from the Operation Toolbar > Click the Quick trim icon from sub options

Step 33: Editing the Sketch

With quick trim Click the yellow line OUTSIDE the Triangular region
> Click Exit Sketch icon from the workbench toolbar

Step 34: Sketching the Spoke

Select the sketch > Click Pad icon from features toolbar > Correct dimension > reverse direction if required (should go towards front of the wheel) > press OK

Step 35: The Main Wheel Spoke

To View in the correct orientation > select Isometric icon from view toolbar at bottom

The main spoke has been created!

Step 36: Creating Spoke Pattern

Click Insert > Transformation > Circular Pattern > Change instances to 5 > change spacing to 72

Step 37: Creating Spoke Pattern

Click on Reference Elements > click on the central lug > Press OK

Step 38: Creating Spoke Pattern

The Wheel Spokes are complete!

Step 39: Sketching the Central Hole

Select the Highlighted Planar surface > Click the Sketch Icon from the right side toolbar

Step 40: Sketching the Central Hole

Click on the Circle tool from the Profile Toolbar > Click on the center point (intersection of ‘V’&’H’) > Drag away as shown > click

Step 41: Dimensioning the Sketch

Click the Constrain Icon from the Constraints Toolbar on the right side of the page
> Click on the circle > drag away > click > double click dimension > correct dimension > click OK
>> select Exit Sketch from right side

Step 42: Creating the Central Lug Hole From the Sketch

Click the Pocket icon from the Features toolbar on the right side of the page

Step 43: Making the Central Lug Hole From Sketch

Click the type pull down menu > select ‘Up to Last’ > reverse direction if required (needs to be into the wheel) > select OK

Step 44: Congratulations! the Wheel Design Is Complete

Save your work – you can now use the features learnt today for designing various 3-D objects

Step 45: Saving a CATIA Part File

Click File > Save As > Select an appropriate name > Select Type as CATPart >  click Save