More on design approach

Discussion in 'SolidWorks' started by Martin, Feb 14, 2005.

  1. Martin

    Martin Guest

    In general terms, is it better to create an assembly out of individual parts
    or should one strive to use sub-assemblies?

    Of course, if you are building a very complex design the sub-assembly
    approach might be the only way out. A car transmission, for example. This
    question might be more applicable where you do have choices. Small projects
    with a few dozen parts where you could consider going either way.

    In the case of using the parts-only approach you'd endup with a directory
    full of parts and one assembly file.

    In the case of using sub-assemblies you'd have the same number of part
    files. A few assembly files that are sub-assemblies and then your final
    assembly file.

    I can see that a real mess could be had if you are not careful about
    in-context mates and how assemblies might drive the final model. It could
    very well turn into a real mess. I would also add that such an approach
    would no-doubt necesitate a project description file to let the next person
    know what the intent was.

    The parts-only approach might be cleaner, but the abstraction level of
    logical sub-assemblies is lost.

    Not sure...

    Martin, Feb 14, 2005
  2. Martin

    daniel Guest


    you actually cover the pros and cons well. From my point of view
    (remembering I am an industrial desiogner who gets too technical...) it
    depends... :) How is that for a difinitive answer!

    Seriously, my approach is to try and work with logical subassemblies as
    the product would be produced and assembled. Yes there are pros and
    cons, but I think in the long run it is clearer and has advantages in
    the master assembly to reduce clutter and confusion.

    As for in-context relations, this is why you should look at assembly
    layout sketches. The principly being to define the key geometry and
    features as a sketch in the master assembly, and or subassemblies, and
    only linking to those. Generally I avoid working on part in the
    assembly to avoid unintended relations. In 2005 there is also a button
    to "turn of external references". In that case you can use the geometry
    to create a sketch, but the relation is imediatly broken to the
    orignating feature.

    You also ask out how to transfer the intent of the assembly to someone
    else. Here is where the subassemblies help. looking at the feature
    manager you can see exactly the history and intent the designer had (or
    mistakes they made...). Also, if you are using 2005 there is a a
    feature in the FM caller the Design Binder. In that is a Word.doc - you
    can use that to document your design process and intent, including
    equations and screenshots - very useful. Also, if you RMB on
    features/parts/assemblies in the FM, you can add a "Comment", which
    makes a pop-up yellow sticky type call out when you mouse over the
    feature - also useful.

    Hope that helps,
    daniel, Feb 14, 2005
  3. Basically I was going to same the same thing. My first criteria is usually
    how is it going to be produced? Are you going to want to detail out a wlmt
    ? How about something that will have bearings pressed in first, then taken
    to another station? You might also have shipping issues as in want to ship
    some of it separately. Just thoughts.

    Wayne Tiffany, Feb 14, 2005
  4. Martin

    daniel Guest

    Pardon my ignorance Wayne... what is "wlmt"? I am sure one you tell me
    I will say "do'h... !"
    daniel, Feb 14, 2005
  5. Short for weldment - weld some parts together, paint it, then bolt on the
    other stuff.

    Hey, a question not asked may cause you to not know when you are in the
    company of more important people. Ask away - we're friends! (But sometimes
    wear your fireproof underwear...) :)

    Wayne Tiffany, Feb 14, 2005
  6. Martin

    Martin Guest

    I finally had a look at this. I rebuilt one of the parts (the PCB) using
    this approach. The holes I need are square. Because of this the hole
    wizard couldn't be used. Regardless of this, using a sketch with points was
    vastly superior to the two approaches I took intially: 1- manually placing
    each copy of some sixty holes. 2- Using patterns.

    [1] was just a dumb excercise
    [2] worked well, but several clusters of patterns had to be created

    The layout sketch approach works very well and is very easy to maintain.
    Thanks for pushing me in that direction.

    However...(always one of those)... it seems that there is not simply way (if
    at all) to use the sketch-driven-pattern approach within an assembly. The
    context is this:

    A master layout sketch now defines the intersections where each button goes.
    These are construction lines.

    I then created several sketches of points to mark off where different
    key/LED arrangments go. For example, there are round buttons with red
    LED's; square buttons with blue LED's, etc. By creating a sketch for each
    logical grouping I reasoned that I could very easily pattern the
    button/dome/LED/hole stack.

    I can insert and mate a single LED by hand, but it seems that I can't use
    the point sketches to pattern that LED (say, all blue LED's). The only
    approach that seems to be available within an assembly seems to be to create
    a pattern and suppress selected entities. The point-sketch approach would
    be vastly superior.

    Martin, Feb 14, 2005
  7. Martin

    daniel Guest

    glad it is working... however... :)

    I think I have my head around what you mean. Without trying it myself,
    the goal is that if you have one pattern feature established in one
    part, you can patter components in the assembly by using the pattern at
    the part level to populate.

    For example, if you have your PCB, and there happens to be a hole
    pattern (a) corresponding to the position of your keys, and (b) to your
    LEDs, place one of your snap domes and mate it. Now select the snap
    part and use the Insert > Component Pattern > Feature Driven. for the
    driving feature, select the pattern (a) or (b) from the PCB. Bingo!

    However.... the only problem is that you may not have a pattern on your
    PCB.... so mate your rubber keypads first! I think it is not possible
    to place a component patten based on a sketch - it must be a feature.
    But someone else can prove me wrong... please!

    daniel, Feb 14, 2005
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