Elrick said:
Lew_Merrick said:
is any of your detail part reference geometry "sourced" to the assembly?
Lew, you mean making geometry references from other part in the assemblies by using the same window to edit a part? (right click on part in design explorer, Edit here, and use something like project to sketch on a different part in the assembly?) If thats what you mean then yes! I enjoy doing this. Project to sketch is my most favorate tool. But I never use other parts in assemblies for reference geomtry such as points axes and planes. I would rather use the measurement tool to get proper dimensions to insert points, axes and planes. I've learned that my assemblies crash when I make changes to parts used as reference geometry for other parts or assembly constraints. The reoson why I choose a longer but safer way. I only recently learned when youre applying dimensions in 2d scetch mode that it picks up linear geometry from other parts in an assembly. Just like the spline recognizes edges and vertices in 3d drawings. I really love this coz it makes things so much easier. As far as possible I always delete references that are linked to other parts in an assembly (Shouldnt it only be relevant when you choose to maintain associativity?? I seldomly choose this when using project to scetch). Just to avoid the havoc.
The area where
I most commonly shoot myself in the short & curlies in
top down design is adding a centerline to a part that is actually
defined by a (say) hole in another part. So long as the two parts are
linked such that they are only
seen in the
assembly situation, all is fine. However, when you go to work on the part that references another as a
stand-along part, problems result as the CAD system (Alibre/Geomagic or otherwise) no longer "knows" where that
reference geometry (centerline in my example) is actually located. The solution, such as it is, is to use that
location of the "external part reference" to
define reference geometry within the coordinate context of the "using part.
Similarly, you need to be very careful with
Project to Sketch at the "assembly situation." Do
not use the
Maintain association to source entity option as this will leave "references" that are not always "available" to you in all situation. Instead, project the geometry and then
define it through dimensions & constraints within the context of the part you are working on.
Elrick said:
Lew_Merrick said:
(or, somewhat less likely, the basis for reference geometry lies in a part file that was edited to delete base reference definitions)
Could you please elaborate on this Lew?
If you define
sketch on a surface of a part that is later "removed" (for whatever reason), the
context of that sketch is lost -- and an error results. To use the example that drove this home to me most clearly, consider a revolved surface that must be given
Draft. The
Draft tool requires a planar surface from which to determine semi-automatic
Draft. Thus, I started off with a
straight sided revolve volume for my part. I added a bunch of
features based on the "edge" of that revolved volume. Later, I added a
revolved volume to the "sides" of the part
and I "cut away" (
Extrude cut) either "end" to provide draft. All my previous
features gave me an
error because the "source" for their definitions no longer existed. Most of the time this is a non-fatal error, but it
can become a fatal error as things progress. Taking the time to construct (and
name!)
reference geometry from which to "base" the "features" is the solution -- though you need to locate it by dimensions and/or
Equation Editor values to be safe.
Does that help?
I wouldve lost it if it did! This is my third attempt to improve its functionality. Theres one thing Ive noticed so far; When I remove the anchor from the parts the red cross dissapears at some constriants?