Top down design

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
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~ Sean Kerslake Dept. Design & Technology Loughborough University Loughborough LE11 3TU
01509 228317
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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. ============================
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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 dim!!
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.
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