Which method is best, Top-Down or Bottom-Up

Discussion in 'SolidWorks' started by Gromit, Jun 11, 2007.

  1. Gromit

    Gromit Guest

    My company is converting/implementing SolidWorks and I wonder which
    method is best, Top-Down or Bottom-Up. Understand the assemblies I
    speak of have existed for many years. We re-configure them daily for
    orders. They are built from many inventoried parts that contain
    slight differences between them. Many parts are used in many
    different assemblies. Any guidance would be greatly appreciated.

    Gromit, Jun 11, 2007
  2. If you're using models of existing parts, it would seem that bottom up
    is the way to go.
    Bruce Bretschneider, Jun 11, 2007
  3. Gromit

    TOP Guest

    The assumption here is that you don't have pre-existing SW parts, but
    do have many parts in some other system. Not knowing specifics as to
    what it is you are really talking about makes it a bit hard to
    generalize, but generalize we will.

    Do you have an existing PDM system? That might play into the answer.

    How many parts in the typical assembly? High range and low range
    please. Do the assemblies have many sub assemblies? Of the parts in an
    assembly how many are those that contain slight differences?

    There would be two approachs to implementing SW in the scenario you
    have presented. Neither really has much to do with top down or bottom
    up design.

    1. For the parts with slight differences use Design Tables. This will
    generate many configurations and this might impact performance and the
    ability of your PDM to handle those parts. Ditto for assemblies, they
    can also be made with design tables.

    2. For the parts with slight differences use a database to create each
    part from a generic part. This requires use of the API and is similar
    to how the Toolbox works for fasteners. Each part will have one
    configuration. Most PDM systems will be able to deal with the
    subsequent parts.

    and of course you could just model each part separately which is the
    third and most basic method.

    In general you use top down to control the geometry of parts related
    by geometry through an assembly or inserted part. Since your parts are
    already defined this would not be appropriate unless the pre-existing
    parts in some way drive the sizing of parts in a top level assembly.
    Then you would have to create a new configuration or a copy of the
    assembly for each variation.

    Using parts and assemblies that are configured assures that things
    that are supposed to be common remain common. Using copies gives the
    best performance and is easiest to manage files.
    TOP, Jun 11, 2007
  4. Gromit

    Bo Guest

    In addition to what other experienced users of SolidWorks in a company
    environment have noted, I wonder whether you have considered hiring a
    SolidWorks consultant to go over your specific company's needs so you
    can get to bottom line "must avoid" and "must have" and then the grey
    area decisions.

    A number of people here on this board are consultants and their
    websites list their type of work. Your VAR ought to know who is
    available in your region.

    These guys hired for 2 days might save you man months of wasted time
    in the next year, and a large amount of frustration. Their fees may
    be high, but they earn it by keeping you from avoiding the worst of
    the known mistakes.

    Bo, Jun 11, 2007
  5. Gromit

    solidsmack Guest

    The quick way to know which route to go:

    Is the part specific to that assembly?
    That piece should be created top-down. Example: some edging

    Is the part used in multiple assemblies?
    Best to use bottom-up. Example: A screw

    Even if it just has slight variations, it's best to use top-down
    instead of configs. However, it is possible to tie those two together
    and have a really fancy top-down assembly. How? Make an assembly that
    is driven by a sketch, then tie the sketch to the top assembly. Sound
    complicated a little I guess, but that will keep you from having to
    make new drawings everytime and you can work configs into that
    solidsmack, Jun 11, 2007
  6. Gromit

    TOP Guest


    I just worked a project that was entirely top down and will add a few
    observations here on the subject that I haven't heard mentioned

    The model I built is for all practical purposes a simple open topped
    box. The design intent is for the box's internal volume to meet
    certain criteria. The criteria are contained in a spreadsheet from the
    customer in the form of length, width and depth.

    Step 1. Build a part with a design table driving this simple "box".
    Cut and paste the customer's criteria into the design table

    Step 2. Insert the "box" model into an assembly as an envelope.

    Step 3. Model all the components off the envelope using in-context
    references for all the features that might be driven by the "box"
    geometry. This means the sides and bottom.

    Step 4. Create a design table in the assembly and cut and paste the
    customer's information into that table as well using the DT in the
    assembly to drive which configuration of the "box" envelope part is
    being used.

    The assembly will now cause all the parts to change depending on which
    configuration of the "box" envelope is being used. Note that the parts
    in the assembly have only one configuration except for the envelope
    part which has multiple configurations. This means that it would not
    be possible to make a standalone drawing of the in-context parts
    without also having the assembly also in the drawing to drive which
    configuration is being used. For this project that is OK because the
    customer only want's drawings of the entire assembly.

    This excercise also demonstrates why having in-context features in
    general can be very dangerous. When there is an in-context feature
    driven by a configuration of another part through an assembly that
    feature's dimensions will require the assembly to be open to update
    and will not be controlled by anything in that part. The part with the
    in-context reference will therefore have multiple configurations
    without having them explicitly managed by the configuration manager in
    that part. Instead they may be managed by configurations in either the
    referenced part or the assembly. In fact the parts with in-context
    references will only show one configuration and "Find External
    References" will only show the currently referenced configuration for
    that part.

    TOP, Jun 17, 2007
  7. Gromit

    fcsuper Guest


    As Top's example shows, there's no hard and fast rule that everything
    must be one way or the other. Each situation has to be judged based
    on the requirements of what is being created in SolidWorks. Also, Top-
    Down is a tool for design of an assembly, but it can be dismantled
    once the assembly is complete (e.g., remove all in-context
    requirements after assembly desgin is complete). If you do have
    common assemblies slighted edited to suit each customer, perhaps
    consider an even more robust approach by controlling design with a
    macro that gets minimal input from the user and automatically
    generates the expected results. Just some ideas.

    fcsuper, Jun 18, 2007
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