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Thread: Custom Shaping

  1. #1
    rwanttaja's Avatar
    Join Date
    Jul 2011

    Custom Shaping

    I'm always in the need for small plastic boxes to house electronics projects. With the departure of Radio Shack, these have to be ordered.

    Instead, I've designed a box in SW where all the dimensions are keyed to a single set of height, width, and length dimensions. This lets me build custom boxes.
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    Now: Doing the cover based on this is trivial....but what I'd like is a section attached to the lid that fits into the opening. This minimizes any leakage (although I know it's not going to be water or air-tight). Obviously, I need to design a thick lid and carve away a section that fits into the opening. It won't be very deep, just an eighth of an inch or so.

    What would be a good way to use the existing opening to shape the lid? I could give up on the fillets on the lower bit and make it angular (which would make it simple to reference) but I'd like something a bit more elegant.

    Ron Wanttaja

  2. #2
    cwilliamrose's Avatar
    Join Date
    Nov 2013
    SW Florida
    If you design the lid within an assembly containing the box you can simply offset the geometry to create the nesting feature. This assumes the box geometry uses the same entities for all the various sizes. And it also assumes the various box sizes are configurations of the base size. The assembly would then also have a configuration for each size and the lid in each assembly configuration would fit the box.

  3. #3
    SOLIDWORKS Support Volunteer Jeffrey Meyer's Avatar
    Join Date
    Nov 2011
    You can also use the "box" part as a multi-body part - no assembly necessary.
    Add a Derived Configuration of the box, calling it the "lid".
    On the top surface of the box create a sketch of the opening and offset as per Bill's instructions. Extrude it downwards as much as you want while making sure that you uncheck the merge result checkbox. You now have a multi-body part. Under Solid Bodies you now have at least 2 bodies. Right-click on the one representing the box, and select Delete/Keep Body. Thereafter finish the design of the lid. You now have a single multi-body part representing both box and lid, that are 100% associative with regards to the box dimensions and topology. You can add a design table with configurations representing as many box configurations as you want - the lids will update automatically.
    Hope I understood your requirements correctly.

  4. #4
    vondeliusc's Avatar
    Join Date
    Nov 2011
    Kalispell, MT
    To expand on what Jeffrey Meyer said:
    If you click on the 'Configuration Manager' tab above the feature tree,
    you can right click on the top-most item and 'add configuration'.
    There is the 'default' configuration, so say you add 'box' and 'lid'.
    Create the box, and then create the lid TO the box, but do not merge it.
    Then, when you double-click the Box configuration, you can hide the solid body which is the Lid.
    Conversely, when you double-click the Lid configuration, you can hide the solid body which is the Box.
    You must right click on the feature tree to enable viewing the 'Solid Bodies' section of the feature tree.
    (this goes for surface bodies, and tables and other items SW chose to hide for some reason; I just un-hide them ALL in my template documents)
    I have all bodies showing in my default config; If you double-click the Box config, you only see the box body,
    and vice-versa for the Lid config.
    Also, if you are creating multiple sizes, I would explore Table-Driven Configurations, so for each box, all you enter are dimensions into Excel, and BOOM!
    you select the version of box you require, and it auto-magically updates to that size, IN ONE PART :-)

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