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  1. #1
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    Default Drive feature dimensions with sketch dimensions?

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    Hi all,

    How do I go about using sketch dimensions to drive feature dimensions?

    For example, I have a sketch with a driven dimension D2@Sketch9 which contains an angle I want to use in a SketchedBend feature as the bend angle. Nothing I've tried thus far has worked.

    What's the go?

    Cheers
    Gerrard Hickson
    G.Hickson@tpg.com.au
    Inventor 2010 Certified Professional | BTech(Mech)
    PointZero Design & Drafting
    Brisbane, QLD, Australia

  2. #2
    Forum Deity shift1313's Avatar
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    If you right click on the dimension in your sketch you can "Link Value". this will put it in list that you can easily access later. After you complete your feature you can double click on it in the feature tree to display all its dimensions on the screen. Blue dimensions are the ones associated with the feature. Black dimensions will be with the sketch. If you right click on your angle value you can "link value" then use the drop down box and select the sketch angle.

    Hopefully that made sense.
    Matt - Certified Solidworks Expert -Advanced Surfacing, Mold Tool and Sheet Metal Specialist
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  3. #3
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    Matt - Thanks for the reply. Unfortunately the dimension I'm using to drive my bend angle is itself driven by a linear dimension, and it seems that 'Link Values' isn't available...

    In the image below, I have the sketch in blue which is intended to provide the angle, by specifying the bend distance (in this case, 30). In Inventor I would normally just use the driven dimension to drive the bend angle... In Solidworks I can't figure it out.

    Gerrard Hickson
    G.Hickson@tpg.com.au
    Inventor 2010 Certified Professional | BTech(Mech)
    PointZero Design & Drafting
    Brisbane, QLD, Australia

  4. #4
    Senior Member bhamze's Avatar
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    Try this. Right click the equations folder and select add equation. Type in "Angle=" then select your driven dimension. In this example the driven dimension (angle dimension) is "D4@Sketch1". Now when you create a sketched bend you will have the option of linking to Angle. In this case angle = to our driven dimension. Does this help?

    angle2.jpg
    Certified SolidWorks Expert -Advanced Surfacing, Mold Tool, Weldments, Drawing Tool and Sheet Metal Specialist

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  5. #5
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    Got it... Thanks for that.
    Gerrard Hickson
    G.Hickson@tpg.com.au
    Inventor 2010 Certified Professional | BTech(Mech)
    PointZero Design & Drafting
    Brisbane, QLD, Australia

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