Top down design

Discussion in 'Pro/Engineer & Creo Elements/Pro' started by Sean Kerslake, Nov 25, 2004.

  1. We use the advanced assembly module and make particular use of the
    copy/publish geometry features to create associativity between model files -
    with or without assemblies.

    Some suggested to me in passing that there was a method of sharing geometry
    [surfaces in particular] and creating associativity between models just
    using the foundation modules, I think probably in an assembly - not using
    the adv ass mod.

    Can anyone enlighten me how you might do this?


    Sean Kerslake
    Dept. Design & Technology
    Loughborough University
    LE11 3TU

    01509 228317
    Sean Kerslake, Nov 25, 2004
  2. Sean Kerslake

    Jeff Howard Guest

    Some suggested to me in passing that there
    You can. The ways to go about it are version dependant, maybe even build
    dependant. What seems to work in several versions (WF & WF2, in
    particular, 2001 maybe?) is to simply copy geometry (generic meaning, not
    Copy Geom.... functions) from a part within the context of an assembly.
    Select the surface, quilt, curve, etc. (it's important to make sure it's
    "geometry" not "features" that are selected; cycle thru or set selection
    filter) and Edit / Copy. In WF this will initiate the function dialog
    (dashboard). WF2 you must Edit / Paste (or Paste Special will allow
    transforms in some cases) to initiate the dialog. (WF2 you can use ctrl+c
    and ctrl+v.)

    Hope that's enough to get you started.

    There's also some additional info in the thread "Skeleton model" by Andrea
    Willans 4/8/04 that pertains to WF.
    Jeff Howard, Nov 25, 2004
  3. Hi Sean,

    If your trying to do what it sounds like you're trying to do, you can
    do it using Relations. You can use relations in both Part and Assembly
    mode. We use them in big assemblies for build tooling: we run a Save
    As on a base assembly and then open the new assembly, change 6 or 7
    dims in the parameters box and then allow the software to regenerate
    the assembly and models and produce updated drawing sets.

    Sorry if I'm teaching you to suck eggs......

    Each dimension you put into a model is allocated a unique
    identification. If you're using Wildfire 2.0 you can either double
    click or right click the dim & choose properties. If you then go into
    Dimension Text there's a box at the bottom of the window called Name -
    this gives the Name of the dimension.

    As an aside, if you change the D in the above window to an S the
    dimension name will show up in the model & drawing - this can be
    useful, especially bearing in mind that you can change the name of the

    If you cancel out of this window and go Tools, Relations it opens a
    window which allows you to enter formulae to link dimensions together,
    eg Dim_1=Dim2+254. When you've entered you formulae, OK out of the
    window and regen the model. This will then regen the model with Dim_2
    254mm bigger than Dim_1. And if you change Dim_1 it will regen Dim_2.

    Check out the onboard help files on relations as well.

    Ivan Robinson.
    Senior Design Engineer.
    International Radiators, Leicester.
    Ivan Robinson, Nov 25, 2004
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