Boundary blend solid?

Hello

I have just discovered the boundary surface blend, really easy to use.
Pick two or more edges then a surface is produced. The only problem I
have is I need to create a solid from it. I have tried "Solidify",
"Thicken" but to no avail.

Anyone know how to convert them?, or should of I created a solid blend
originally?

Thanks

Geoff

 

You have to merge the surfaces first. Pick a couple surfaces and the Merge icon
should activate. Keep merging until you have a single quilt. Leave that last quilt
selected and try the 'Edit>Solidy' icon again. Or the 'Thicken' icon, if it's not
a closed, watertight volume.

 

.... The only problem I have is I need

If your Boundary Blend surface / quilt intersects solid faces in such a way that
intersect / trim / join operations would result in a volume definition it can be
Solidify'd. Just select the newly created surface / quilt and see if the Solidify
toolbutton becomes active.

 

Yes it does become active, but when I complete the feature the suface
disapears?, I checked the info button which tells me it is a cut
feature.

I cant see where to change that to a protrusion.

I'll give a little infomation about the part I'm trying to do. I have
two solid rectangles one smaller than the other. The smaller one is
offset above the bigger one. I clicked a edge off the bigger one & an
edge off the smaller one. Then I clicked the boudary blend button which
produced the surface.

Thanks

 

.... I clicked a edge off the bigger one & an

Clicked "an" edge
---- or ---
chained enough edges to bound a "region" for each section, which is what I think you
want to do?

If that's not it we can try to talk thru it or you can post models on forums like
mcadcentral.com.

 

Clicked "an" edge

Ok, I see what you've got. The single, open surface will not intersect / trim / join
to create a volume definition so the only option available is a Cut (and it errors
since nothing gets cut).

So, what you want to do (a mini lesson in "chaining") is:

_ Select an edge.
_ Hold the cursor over the edge until it pre-highlights again.
_ Press / hold Shift. Notice the screen tip says; One-by-one.
_ RMB to toggle thru chaining possibilities until it says; Surface loop, and the
correct solid face is highlighted.
_ Click to select the loop.
_ Release Shift and press Ctrl. (You've completed the first section, Ctrl starts a
new chain for the next section.)
_ Select an edge of the second block and repeat the process.

You'll probably need to adjust the Start Point for one of the sections. Grab and
drag or ...
_ Click the Curves flyout tab on the Dash Panel.
_ Click Details under First Direction.
_ Options tab, Start Point.

The default Control Points won't be to your liking (why on such a simple shape is
beyond me).
_ Dash Panel, Control Points tab, Fit: Piece to Piece (is the easiest way and
suitable for this application).

That should get you what you want (unless you want to constrain the boundaries
tangent to the sides). Once done, the feature will still be in the Selection Set and
the Solidify toolbutton active. Hide the BBlend quilt when done.

 

Thanks Jeff

I'll have a go and get back to you.

 

Hi

I still cant get this to work, I have used the surface chain to create
a quilt then I try to Solidify or Thicken but both produce a cut.

I have also created the surfaces one by one then merged them using the
Merge with the"Join" option. This again produces a cut with Thicken or
Solidify?

Any ideas

Geoff

 

Any ideas

Not without seeing the part. Why don't you post it to mcadforums.com and someone
will take a gander at it (state the version of Pro/E used). Two minutes to look and
fix vs. two hours written communication and guessing.

 

I have to agree with Jeff. This medium is too restrictive for difficult problems
of visualization and communication. For example, I replied directly to you, Geoff,
with an IGES that I thought answered your description of the problem, with some
explanation of how to go about making it (got bounced back as undeliverable; I
thought it was probably the attachment); so forwarded the same to this NG, with
the attachment, and, of course, it never appeared in the distribution (maybe my
news server filtered it out!?! although it'd be a first), then I tried sending
directly, just some comments on the problem (no attachments) to your
and got bounced again, so I'm guessing it's your "reply
to:" address that's bogus. (Three strikes, I should be out.)

Anyway, before we go skipping off to MCADland, could I get an answer to just one,
simple question? The surfaces you've created by whatever means ~ a blend between
two offset, rectangular solids ~ is this a six sided quilt (four outside sides
plus a top and bottom surface), forming a completely enclosed volume; all merged
into a single quilt? If you answer 'yes', go ahead and post, with pictures,
outside this group, cuz I don't get it and can't help you. If, however, you didn't
make a six-sided, completely enclosed quilt, don't go anywhere. Just copy the
bottom surface of your top rectangle (select, ^C, ^V) and the top surface of your
bottom rectangular solid (^same) and merge those with the sides. While still
selected, do 'Edit>Solidify'. Ooops, order of operation error: do this first then
use these edges for chaining, as Jeff suggested, to create the boundary blend
surfaces. In fact, one more enhancement: do two opposite sides, then enclose the
ends, using the edges of the new surfaces as second direction guides.

Anyway, this is some of the stuff that was in the posts that didn't make it
through.

David Janes

 

... is this a six sided quilt ...

Actually, one solid face on each block is part of the volume boundary so you just
need four surfaces in the quilt to get the Solidfy to work.

I'm curious about the attachments and your not being able to post one. Gonna try a
small part (WF2, smaller than some of the freakin' spammer's posts) as a reply to
this post to see if it works.

 

Nope, won't work; though I know pdfs and jpgs will attach. Guess the spammers are
one up on us. 8~)

 

Right I've just posted the files here

http://www.mcadcentral.com/proe/forum/forum_posts.asp?TID=28020&PN=1&TPN=1

Its a pity this newsgroup doesn't support file uploads

 

It does limit the possibilities. I'd thought to ask if you were trying to create the
geometry in assy environment, but who knows how long it would have been before
someone got around to it. 8~)