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How to model spring in solidworks ?

By mohkaseb on 24 Sep 13:53 3 answers 0 comments

solid works

3 answers

  • Luis Arias
    Luis Arias almost 2 years ago

    I know two ways to do a spring in SolidWorks, one is using Helix and Spiral with Swept Boss/Base and the other option is using only Swept Boss / Base.
    I goin to explaine Helix and Spiral with Swept Boss/Base:
    1 paso_circulo
    Open a new part. Create a 2D sketch.Select the Top Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon. Create a circle 100 mm diameter and clic OK.
    2 paso_helice:
    Create a Helix / Spiral. Select the Constant Pitch option
    Set the Pitch length to 25 mm. Set the number of Revolutions to 10. Set the Start angle to 0 deg. Select the Clockwise option and clic OK.
    3 paso_espira:
    Create a 2D sketch. Select the Right Plane and create a sketch. Create another circle. Create a circle somewhere at the Right Plane as shown in the picture. Connect the Circle sketch with the Spiral Sketch. Select the midpoint of the circle, hold down the Control key and select the Spiral sketch. Click at Pierce.The circle is now connected with the Spiral sketch. Change the diameter of the circle into Ø15 mm by clicking at the dimension button and clic OK.
    Create a Swept Boss/Base. Select profile Sketch2 and select path Helix/Spiral1 and select OK.
    And ready model spring in Solidworks.

  • Luis Arias
    Luis Arias almost 2 years ago

    I going to explaine other way to do spring using only Swept Boss/Base:
    1_paso largo
    Open a new part. Create a 2D sketch.Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon. Create a vertical line 100 mm long and clic OK.
    2_paso_espira
    Select again the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon. Create a circle 15 mm diameter, add horizontal relation and fix the diameter of spring as shown in the picture and clic OK.
    3_paso vueltas
    Create a Swept Boss/Base. Select profile Sketch2 and select path Sketch1, Clic in Options, select Twist Along Path in Orientation/twist type, Select Turns in Define by, set the number of turns in 5 and clic as shown in the picture an clic OK.
    And ready model spring in Solidworks.

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