In my continuous mission to explore far galaxies, I stumbled on the top-down
assembly construction method explanation on the sw2006 help documentation.
so please correct me if I'm wrong:
"external references on parts can be created only in the top-down modeling
technique by referencing a new feature or sketch in a new part to an
old/already-existing one which is open simultaneously on the same assembly
(part modeling within assembly modeling)."
is this statement true or false?
please help me remove the dust in front of my eyes!
Forget what they wrote and say to yourself, "Well, duh, how else would
one do it?!".
If one part has entities that are constrained to another part, where
would these constraints be made? In an assembly, of course. You can
not convert (another part's) edges in a sketch or extrude to (another
part's) surface or plane unless the two parts are residing in the same
As far as the new part-old part thing, basically SW is trying to tell
you that if part "A" references part "B", then you shouldn't also have
part "B" reference part "A".
sorry, but I still don't understand:
is it possible to reference a part in an assembly externally using regular
assembling by entering existing parts? (traditional bottom-up assembling)
or is it only possible when creating a new part inside an assembly which
already has at least one part? (top-down assembling)
The statement is false, but contains some truth. It is false insofar as
external references on parts can be created through splitting a part,
deriving a part or mirroring a part as well as through an assembly. If
the context of the statement was within assemblies then it is true.
Thinking back to the days of tracing paper, an external reference is
like making a drawing of a part by placing tracing paper over the
layout and getting key features through the tracing paper. The part
getting external references can be an existing part or a new part. See
the post a day or so ago about removing external references.
Forget "top-donw" and "bottom-up". An external reference is simply
when a feature or sketch in one part is dependent on an entity in
another part. In nearly all cases, this dependence happens in an
assembly, with one component referencing another.
Any part mated in an assembly can have external references created WRT
other parts in the assembly. In fact when a part is created in an
assembly a special inplace mate is created to hold it still while
references are made. So for example, when doing bottom up modeling,
mate a piece of "precut" sheet metal into an assembly. Locate some
matching holes and cut them while editing the part in the assembly.
Then open the part outside the assembly and remove references and
create dimensions automagically.