Make a shower drain with Flanged Hole

Small

https://youtu.be/gyzdFPjSGXc

Here is a demonstration showing you the design of a shower drain grid in CATIA 3DExperience.

The Sheet Metal Design application, based on industry process features, allows you to create quickly a plate that you can bend and add stamp, dowel, bridges, etc.
This video is divided in two parts. First you see how to design the outer plate (using walls, flange and corner relief). The second part deals about the grid's design. In this Part, you will use GSD to create a repetition of points that will allows you to pattern the Flanged Hole Feature.

  1. Step 1: Video


  2. Step 2: Create the plate [Part 1]

    * Better to watch the video *

    Create a new product called "Shower Drain"

    insert a new 3DPart called "plate"

    -

    double click on the 3DShape

    Switch to Sheet Metal Application

    * in Sheet metal, you need to set up the global parameters *

    Click on Sheet metal parameters

    set the thickness to: 0.2mm

    set the bend raidus to: 0.5mm

    -

    Add an offset plane from XY plane

    put 5mm and reverse the direction

    * this will help you during your design *


  3. Step 3: Create the plate [Part 2]

    sketch a centered square 200*200m

    in the same sketch, add a centered circle Ø160mm

    exit the sketch

    Click on the feature "Wall definition"

    * the thickness is automatically set up to 0,2mm *

    select the top direction and lick on OK

    * the result should be this one *

    Create a wall on the plate's edges

    -> Click on CTRL + Click to do a multi selection of the 4 edges

    keep the angle to 90deg

    for the length right click on value

    add the formula

    * a panel appears *

    double click on the value of the offset plane (5mm)

    * in that way, when you move the plane all the wall will have the same length *

    In the extremities tab of the Wall panel, add -0,5mm on the left and right side

    * from this *

    * to this *





  4. Step 4: Create the plate [Part 3]

    Add a Flange on the hole's edge

    Keep the angle to 90deg

    Right click on the value and add a formula

    select the dimension of the offset plane (5mm)

    * in that way the flange and the wall have the same length *

    Modify the value of the offset plane to 2mm

    -> Flange and the wall are updated in the same time

    -

    Refine the part using the Corner Relief feature

    * it changes the straight corner into a round corner *

    Select the 2 bend radius of the 2 walls that makes the corner

    Set the value on 1mm

    Click on OK

    * from this *

    * to this *

    Continue with the other corners

    -

    (optional)

    You can unfold/fold the part to see if it is correct

    * unfolded plate *

    -

    Hide the Planes



  5. Step 5: Create the drainer [Part 1]

    Go back to the top product in Assembly Design

    * it can help to hide the plate part *

    Insert a new 3DPart called "drainer"

    -

    Double click on the 3DShape

    Switch to Sheet Metal Application

    * in Sheet metal, you need to set up the global parameters *

    Click on Sheet metal parameters

    set the thickness to: 0.2mm

    set the bend raidus to: 0.5mm

    -

    Add an offset plane from XY plane

    put 2mm and reverse the direction

    * this will help you during your design *

  6. Step 6: Create the drainer [Part 2]

    Sketch a centered circle Ø155mm

    exit the sketch

    Click on the feature "Wall definition"

    * the thickness is automatically set up to 0,2mm *

    select the top direction and lick on OK

    * the result should be like this one *

    Create a Flange on the edge of the cylinder

    keep the angle to 90deg

    right click on the length value and add a formula

    select the dimension of the offset plane (2mm)

    -

    Create a sketch on the top surface of the drainer

    Draw 4 circles Ø50mm, Ø80mm, Ø110mm, Ø140mm

    Exit the sketch

    * the result should be this one *




  7. Step 7: Create the drainer [Part 3]

    Switch to Generative Shape Design application

    In transform tab of the action bar, click on Extract

    * a panel appears *

    Click on the marble bag and extract the 4 circles

    * the circles will now be 4 different entities *

    Hide the sketch

    -

    Create a point on the center of the top surface (0,0,0)

    Create a point repetition on the first circle Ø50mm

    add 8 points

    Create a point repetition on the first circle Ø80mm

    add 12 points

    Create a point repetition on the first circle Ø110mm

    add 16 points

    Create a point repetition on the first circle Ø140mm

    add 22 points

    * here is the result *


  8. Step 8: Create the drainer [Part 4]

    Switch back to Sheet Metal application

    Click on the centered point and add a Flanged Hole

    right click on the height value and add a formula

    select the offset plane dimension (2mm)

    Change the height type to the second mode

    keep angle to 90deg and diameter to 5mm

    Click on OK

    -

    In the transform tab of the action bar, select the User Pattern

    Select the flanged hole as the object

    Select the center point as the anchor point

    Select the Points repetition as the positions

    -> Click on the marble bag for multi selection

    -

    (optional)

    If you edit the sketch and change the diameter value

    -> the drainer will be updated

    Same, if you change the number of instances in the point repetitions

    -> the drainer will be updated

    -

    Change the view mode to custom view mode

    Hide the points, lines and plane

    -

    Go back to assembly and show the plate part

    * The result is this one *


    • End of tutorial


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