How do you copy geometry?

When you have an assembly and you need to keep a relationship between
parts (say for example you have a molded enclosure with screw bosses)
how do you keep your parts parametric? Do you:

1. Use Copy Geometry from a master part in your assembly;
2. Use External Copy Geom and publish from a part that is not in your
assembly;
3. Use copy and paste from a master part in your assembly;
4. Use >Edit >Component Operations >Merge and merge an entire master
part into your child part.

Why do you prefer your particular method?

 

When you have an assembly and you need to keep a relationship between
parts (say for example you have a molded enclosure with screw bosses)
how do you keep your parts parametric? Do you:

1. Use Copy Geometry from a master part in your assembly;
2. Use External Copy Geom and publish from a part that is not in your
assembly;
3. Use copy and paste from a master part in your assembly;
4. Use >Edit >Component Operations >Merge and merge an entire master
part into your child part.

Why do you prefer your particular method?
I did something similar in a way that's not on your list. I use a skeleton model to communicate information between components in an assembly.

I had a relatively small component rack with a lot of cables and cable terminations, often more than one per cable: over 50 cables, over 120 terminations and routing between them. After someone else started the cable routing business and created half a dozen circular references, I decided there had to be a way to avoid this, to get component references into the cables without creating circular references and robust enough to update when component position changed.

That way was to create pub geoms on the component terminations, copy the pub geoms, with copy geometry, into the skeleton part, mate all the cables to the default location (comp csys to assem csys) so no circular refs were possible, and, ignoring how the components were assembled, built the cables with geometry refs copied from the skeleton model, through which the cable terminations stayed parametrically linked to the components. It was pretty robust, though somewhat labor intensive.

In addition to the component terminations, copied from pub geoms on the components, I also copied a lot of reference geometry from the rack to use for creating points for routing cables. So, in the end, this skeleton part had hundreds of features (surfaces, datum points/planes/axes and patterns) that could all be used for components references, especially thru point curve references. They could be directly created in the skeleton or be copied from component geometry or pub geoms (which are nice because you can include a range of geometry in one pub geom feature, e.g. surfaces, points, axes, planes.) And when you copy geom from a pub geom in a skeleton part, you get this geometry as a group.

In addition to the methods you mentioned, another I've heard of for molds, specifically, is Inheritance Features. Haven't used them, though they are reputed to avoid drawbacks of other methods.

David Janes

 

I guess cable design is more schematic than plastic part design. I
haven't tried skeletons: I suspect they're used more in your type of
situation.

Anybody else out there?

 

Skeletons are capturing the intent of other shared layout data
(assemblies, parts, routing paths/no-go areas/connectors/pass through/
grnd points../) within the group so,, sketetons would work great for
cable/routing if you are working collectively or within a group?

... (is it me or are we all going backwards in time,.. and why am I in
this hand basket?)

 

I think that for mold design you really want to look into something
like TDO (Tool design Option) This reinforces the master-model
concept and works initially with surfaces. TDO can streamline the
process quite a but, but needs the .mfg file in session to force
updates (I think)

I use Pro-E for forge tooling design with a master cavity model that
has a co-ord system included for tooling placement. The outer skin
geometry is surfaces that are 'published'. The tooling then uses
external-copy-geom to include the published geometry from the cavity
in the die model as surfaces. The advantage of using published
geometry is that you can add or subtract surface patches without
bombing downstream features that depend on the published geometry as a
whole.

Using surfaces vs. solids avoids the problems associated with matching
accuracies between solids, especially of you go on to create die EDM
electrodes from the die models.

Now, none of this works unless you have the right config,pro options
turned on to propagate changes and update models.

I don't use Interlink/PDMlink, so I can't comment on how that affects
the mix.

I could give you an example if you like,
Chris Gosnell

 

fwiw...

For basic geometry that is to be shared globally across many
components, we'll use skeletons contained in a top level assembly.
Geometry such as point, plane, axis, and maybe some general surface
stuff, like envelopes surfaces. These are shared using ExtCopyGeom.
At the component level, we create a "master" one piece model, place
this in it's own assembly. This master model will use ExtCopyGeom on
the toplevel skeleton. Then stuff individual sub-components needed
for this component model into the same component assembly. These sub-
components use ExtCopyGeom from the master model (only geom needed to
create) . Some other sub-assemblies may be needed, etc. etc. The
point being, there are no isolated components. When you open the top
level assembly, ~all components are opened and all updates are
propagated through entirely. Drawings use Simplified Reps a lot due
to so many of the same components stuffed into the assemblies.

We use a lot of weldments in our operation. Weldments require a
unique method for modeling and after several years we have, what I
believe, nailed down successful methods. The above has worked pretty
flawless for us. Duplication can get a little problematic though.
Have to really think ahead before hand on what components may be re-
used.

imo, ~don't use Merge... this can be a real pain in the future. We
avoid them like the plague.
we use some inheritance--works good with castings.
use CopyGeom sparingly--only in short assemblies where sub-components
can be "hard-wired" and will not be used without the parent assembly.


-mark

 

<snip>

Thanks for your description of some sophisticated, top down design methods.
But, to echo Graham's concern, how do these methods preserve relationships
to the parts they are based on?

This was the one, judging by the name and reputation, that I thought had the
best chance of preserving a relation to the parent part. But, I haven't used
it and I'm not sure why its use seems to be so confined to molds and
castings. Any insights as to why it isn't more widely used!?!

David Janes

 

~hey David

By having all the models and sub-assemblies tied to top down, when you
open any level assembly, regen will propagate any changes down to
children. Preferably you should always open the top most assembly,
even if you simply close the window. This insures you haven't missed
a branch when it regens.

I think inheritance definitely has it's place, but I would say it's a
heavy weight usage component. It carries all the features and
definition of it's owner, where most of the time (at least what I've
done) you may only need a couple of surfaces to help define the new
component. In some weldments and finish machining instances
inheritance is absolutely beautiful! In other instances it would be
virtually impossible (may read: ridiculous) to use.

 

I've posted this to:
http://www.ptc.com/forums/

as well. It seems to be more active than this group.

 

Chris, I design molded parts, not the tools. Our products are often
fairly organic, so the exterior shape is made with one or more
boundary blends or swept blends around a part line. I use a master
file to keep overall shape related between the final molded parts and
also things like screw bosses, windows, keypad openings etc etc.