Magneta outline of feature in drawing mode

Reference this picture
http://www.flickr.com/photo_zoom.gne?id=99803630&size=o

This part is an assembly that I created another part "on the fly"
using the original part as a reference.

As you can see in the section view, the filled part is the "overlay".
It extends over the surface shown in the left hand view. When I
created the final feature, which was a rotated protrusion, Pro shows
it as a magenta outline in the drawing (might show up as purple in the
JPEG), why? Also notice how it is not "hidden" by the outside surfaces
in either view.

Geom Check is greyed out, so I'm *ass*uming there is nothing wrong
with the geometry. I've opened just the overlaid part and no Geom
Check there either. Here's that drawing...same thing:
http://www.flickr.com/photo_zoom.gne?id=99806060&size=o

Any suggestions would be highly appreciated.
Doug
Wildfire 2.0 Build M160
Windows XP SP2
ATI Fire GL T2-128

 

Reference this picture

Not gonna "sign up" to take a gander but sounds like you've created a surface
feature vs a "protrusion".

 

Clicked the rotatated protrusion button....maybe I'll do "solidify"
just for grins.

Sorry for the need for signup....new to this whole flickr thang. This
URL will show the image.

http://static.flickr.com/28/99803630_a166956a90_o.jpg

Here's the other image URL

http://static.flickr.com/39/99806060_6bd9620e14_o.jpg

Doug

 

What were you doing with this "rotated protrusion" and where: if you'd created it
in assembly mode to make a cut, it defaults to surface. Most of these are highly
technical questions related to HOW you are making these 'copied' parts ~ what
method you've employed (Copy gemometry from other model or Shrinkwrap from other
model) come to mind as ways to 'reference' another part. But to avoid guessing the
right (or just as often, the wrong) answer, we need to know the how you are doing
this and it often doesn't hurt to know WHY ~ what's your goal, what're you trying
to accomplish. Then we can tell you some good methods for getting where you're
going. And they may not be the ones you originally selected. We do not want to be
put in the position of going to great pains to tell you precisely how to do
something dumb.

And the magenta goes away when you use the surface to create a solid through
'Edit>Solidify' or 'Edit>Thicken'. Select the quilt first, then the menu item.

 

Reference this:
http://static.flickr.com/33/100147855_d51b49b2e2_o.jpg

The dark surfaces is the nitrile overlay

So it seems I made a quilt. As to why I did what I did. The large part
is a machined casting which gets overlaid with nitrile. I chose
"create component in assembly mode" I chose "part" and "create
features". At that point I created a revolved protrusion over the thin
"lip" (feature on left of aforementioned picture). Then I created a
extruded protrution on the bottom surface and finally the revolved
protrusion on the right hand surface. That is the one that became the
quilt.

The reason I created the overlay using the assembly part as reference
is for expediency. I've used the same technique to create welded
overlay for seats and valve discs. I've never ran into the problem
with quilting until now. Funny it's only the last feature that
quilted, none of the other surfaces show that.

I tried to solidify and Pro complains that it has a problem resolving
the interesction of the revolved feature and the extruded feature.
Thicken works but I get this "hole" in the hatching in the cross
section view unless I choose .001 and then there is no cross hatching.

Thanks for the suggestions.
Doug

 

So..if you inadvertently press the "surfaces" button in the
dashboard...you make a surface...imagine.....Sorry for the waste of
bandwidth

<doug slinks off redfaced>

Doug

 

... if you inadvertently press ...

No prob. Sometimes just talkin' about it helps. I know. `;^)

 

I think I might know what's going on, between your descriptions and the picture,
Doug. It sounds like you revolved an open cross section (i.e., the geometry didn't
form a closed figure, something like revolving a U | without putting a top on it).
So, while you could have made it a thin protusion right off the bat, it defaults
to a surface. To create the solid you want, make sure the original cross section
is closed, even if it buts up against another solid. So, if it is against another
solid, you can use its edge as one side of your cross section sketch with 'Use
Edge'. Alternatively, create you open, revolved surface, then, make surface copies
of your solid and merge the copied surfaces with your open surface to form an
enclosed quilt.

The only other thing that corresponds to the symptoms you've described is the
rovolved U with separate surface geometry for the top, but which is not merged,
does not form a single, merged quilt. So, while it is encloses a watertight
volume, is can not be solidified because it is not a single quilt but adjacent
patches. Merge the U with its top and then solidify.