7-tips Sketcher Part Design CATIA R19x

The tutorial deals with Sketcher Application in CATIA 3DExperience R19x.

I have listed 7-tips that could be useful in Part Design or Generative Shape Design. Some of them are also very known in CATIA V5 as well!

This list is non exhaustive, there are always other tips in CATIA! So feel free to comment the video :)

Here is the summary:
#1 Triangle & Polygons (0:48)
#2 Equal dimension feature (1:56)
#3 Automatic Sketch Constraints (2:56)
#4 Text (4:01)
#5 Silhouette for Cylinder (5:22)
#6 Output Feature (6:50)
#7 Opened Sketches (7:54)

If you have any questions, do not hesitate to reach us via our website (http://www.plm-technology.com) or via the YouTube Channel.

Please like, comments, share and subscribe ;)

  1. Step 1: Video

  2. Step 2: Triangles and Polygons

    Create a 3DPart

    Create a Sketch on a plane

    In Action bar, under rectangle icon, click on Polygon feature

    Create an Hexagon (6-edges)

    Redo the step, but click on the "N" icon

    Create another Polygon with the number of edges you want

    -> For instance 3edges give you a triangle

  3. Step 3: Equal Feature

    On the same part, create another sketch

    Draw a circle A

    Draw another circle B

    Apply a diameter to the the circle A

    Then click on the equal feature to give the same diameter to circle B

    * You can do the same for any kind of dimension *

  4. Step 4: Automatic Sketch Constraints

    On the same part, create another sketch

    Draw a spline

    * tips: click on SHIFT to remove the magnet effect on the grid *

    * it takes time to manually constraint the spline points by points *

    Use the rectangle selection to select the whole spline

    Under constraints icon, click on auto constraint icon

    A panel appears, select the Horizontal and Vertical axis to execute the command

    * the spline will be constrained along H and V axis *

  5. Step 5: Text

    On the same part, create another sketch

    Draw a spline

    Change the spline as construction element

    Click on Text feature

    Right the text you want, choose the font, the size, etc.

    click on the spline

    * the text will be generated and will follow the spline curvature *

    * you can put the text over, under or in the middle of the spline *

    * Tips: the text feature is not associate, meaning that you cannot edit the text once it is created. therefore it is better to keep this feature at the END of your design *

  6. Step 6: Silhouette Cylinder

    On the same part, create another sketch

    Draw a rectangle passing on the middle axis

    Draw an axis line in the middle

    Exit the sketch

    Create a Shaft using the rectangle and the axis

    Draw another sketch in the same plane as the first one.

    Draw another rectangle on the edge of the cylinder

    * in order to make a shaft *

    * if you select the external surface of the cylinder, the software will actually select the axis of the cylinder. Therefore you need to create a silhouette *

    Under project icon, click on silhouette feature

    Select the surface of the cylinder

    * the contour will be generated and will be colored in yellow *

    Transform the contour in construction element

    Add a coincidence with the rectangle and the contour

    Exit the sketch

    Create a groove with the rectangle and the axis

    * the result should be like that *

  7. Step 7: Output feature

    On the same part, create another sketch

    Draw a centered circle A

    Transform it as a construction element

    Draw another circle B on the circle A

    Exit the sketch

    * when exiting the sketch, the construction elements are not visible, therefore circle A is not visible *

    * Only circle B is visible *

    Edit the sketch

    Right click on the circle A

    In the bottom list of contextual menu, click on output feature

    The circle A will become brass

    Exit the sketch

    * Circle A is now visible in the 3D *

  8. Step 8: Opened sketches

    On the same part, create another sketch

    Draw a profile

    -> do not close the sketch on purpose

    * in order to simulate an opened sketch *

    Exit the sketch

    -> you cannot create a pad with the profile

    Edit the sketch

    in Analysis tab of action bar, click on sketch analysis icon

    A panel will appears, it will tell you

    • if the sketch is constrained, under constrained or over constrained
    • if it is opened or closed
    • the list of all the elements in your sketch (points, lines, arc, splines, etc.)

    Since the sketch is opened, click on close opened profile feature

    ! Warning ! this will close the profile but also change the geometry of your sketch

    * The sketch is now close, you can exit the sketch and make a pad *

    • End of Tutorial