Assembly Xsec

Hi people
I'm creating a Xsec in a Assembly file.
Do u know if it's possible to keep entire (not cut) some parts excluding
them from Xsec?
Thanks

Pier

 

Yes, select properties on the hatch, cycle trough each part and you can
remove (dont remember the exact name)the hatch for the selected part.

Hugo

 

Yes I know
But in this case you have the part cut in 3D and without hatching.
I' d like to have the part NOT CUT !
I 'd like to see the assembly in 3D environment with some parts cut and
with some other parts not.
Bye
Pier

 

Yes it is. You should aquaint yourself with the ZONE method of selecting and
defining components for cross sectioning. Especially useful is zone creation by a
quilt definition of the boundary of the zone. This quilt can be a series of
copied, merged surfaces defining the exact parts you wish to have excluded. This
is available when first creating the xsec by selecting Zone as the creation method
(NOT Planar or Offset). As with most things in Pro/e, it helps if you create this
zone ahead of time, with the tools that are optimally available. With
"Inside/Outside" for component selection, you can use a quilt as the definition of
what components belong in the cross section and which do not. The "recycle" arrows
flip the direction (and provide yet another example of the heterogeous, amorphous,
elastic definition that PTC/Pro/e has of GUI interface ~ and in Pro/e's case, it's
about 6 dinstinct interfaces, 90% of which are still Menu Manager style of
floating, separate windows. I just wish they'd get the idea of dedicated screen
regions and doing everything in a common working area) Create your zone quilt that
includes/excludes components outside of this xsec creation functionality. As with
cross sectioning, in general, the setup is best done in Pro/MODEL, not Pro/DETAIL.

 

Thank you David.
I tried unsuccessfully. The surface is closed, is made on part level.
there is not any error messagge. With double click on section name
nothing happens !
Anyway I understand your suggestion !
I'm sure you agree me if I say that it's a very complicated method to
get a partial section. I'm not interested on "elastic definition " or
"flexibility" in ProE environment. I think it should be very simple to
select from the assembly tree the parts not included in the section
(other CAD program can do it) and that's all !
I found another way based on Simplyfied Reps but it's complicated too.
Thanks
Bye
Pier

 

Okay, forget zone selection; you're right: too difficult, clumsy and ineffective.
Now, instead of doing what huggre suggested in the drawing, do it in the part.
Pick 'View>View Manager>Xsec', select the view name then RMB 'Redefine>Hatching'.
Cycle through the section with Next xsec until you come to the components you want
to exclude and click on Excl Comp. Do this with each component you want to exclude
from the section. When you show the section in your 3D view, those excluded
components should not be sectioned ~ neither cut nor hatched.

 

I don't believe you fellas are talking about the same things here.

3D environment = an asssembly model window?

3D view = where the view is not normal to the section plane?

 

Sorry, make that "where the drawing view is not normal to ...".

 

I admit the possibility of what you say; still, what I think both Pier and I both
want is this:
a view, with excluded components, should show up as not only not hatched in an ISO
view, but also not cutaway, not sectioned, when you do Excl Comp. I say it's
possible, if one does it in the model; no matter how it looks in the
assembly/model hatched section view, it will look correctly sesctioned in the
drawing view (odd, I know, that it'd look wrong in the model but right in the
drawing, but that's my contention.)

 

I say it's possible, if one does it in the model ...

It (excluding in a drawing view) can be done while working in the drawing, too.
Update sheet when done to redraw the missing edges. (Perhaps I misunderstand
the inference; e.g. you Must exclude while in model mode.)

I do know one thing; Pier and I would both like to see a method of exclusion by
rule of some sort. It's not real high on my list of dream features but Select_1
vs. Select_1_or_more leaves a big hole in the fuctionality. I guess the
practice of not axially sectioning common hardware (fasteners, etc.) items
doesn't hold much sway with Pro/E's larger accounts unless I'm missing
something.

I'd like to hear more about Pier's simp rep solution.

If it is truly the "3D environment" that Pier's concerned with; is an assembly
cut feature worth looking into?

 

Hi friends.
I conferm that my ieda is to have an "uncut" model in an assembly
environment. Let's suppose not to have drawing at all.
The "Excl Comp" in a ViewManager-Xsec operation regards only the hatching.
For me it's important to keep entirely solid one or more parts in an
assembly environment.
I think about two solution.

1 - Extrude-Cut feature in an assembly mode.
Intersect option to exclude one or more components.
Simple but it's a feature anyway ( it's necessary to remember to
suppress it,it should be the last feature in an assembly tree, it's not
simple to manage in a drawing,ecc...).
It's good for a quick image.

2 - "Simply rep" for the parts I want to section.
Component environment - Simply Rep - Work region - Draw the area to cut
as an extrude-cut.
Assembly environment - Simply Rep - Substitute - By rep - select the
simply rep of the part I want to sec .
Good solution because it's not a really cut operation and it's simpler
to manage it for 2d view , ecc...
It's not good if you have a complex assembly with a lot of components.

I'm working with WF2.
Any info about WF3 ??

Bye
Pier