Sectionioning in assy

Dear All,
I have made an assembly which is comprising of many components
including sub assemblies. Now when I cut the whole assy using any of
the default assembly planes then, in drawing of that main assembly
when I am showing the sectional view, the component which are lying
behind are also shown in the section as thick geometry lines.... I
have made the display mode of that view's display mode as No hidden,
No disp Tan & Hide skeleton mode. The version I am working on
Proe2000i & Proe2001. The problem is there in both.
Now My question is how can I avoid the thick lines of those components
which are lying beyond the section?
Thanks
kjain

 

: Dear All,
: I have made an assembly which is comprising of many components
: including sub assemblies. Now when I cut the whole assy using any of
: the default assembly planes then, in drawing of that main assembly
: when I am showing the sectional view, the component which are lying
: behind are also shown in the section as thick geometry lines.... I
: have made the display mode of that view's display mode as No hidden,
: No disp Tan & Hide skeleton mode.

Flip the cut plane arrows. I think you're looking at the section through the
assembly instead of looking at the assembly through the section.

David Janes

 

Dear David,
No the flipping action is not the cause. It is something else.
thanks
kjain

 

Are you sure the components are hidden, and that your section cut has not
revealed them?

 

: Dear David,
: No the flipping action is not the cause. It is something else.

In the same 'View Modify' menu manager window with the 'View Disp' menu is one
called 'X-Section'. If you look at the options under this menu item, you'll see
one called 'Flip'. I would try this as this is what I meant by flipping the cut
plane arrows. Anyway, this determines whether the cutting action cuts away the
front or back of the model. If you cut away the back, you will see the cross
section but still be viewing the solid structure of the assembly in front of the
section. When you flip it again, you should see the section geometry but not
what's behind when view display is set to no hidden.

BTW, Pro/e makes it possible, as a supposed convenience, to create and, to some
extent, modify cross sections in drawing mode. I took the detailing course and
learned there what a PITA this is. I haven't done a cross section in drawing mode
since. I make all my cross sections in part/assembly mode where you have a model
to manipulate, where it is much easier to select datums, where it is easier to
create datums and sections and even to modify cross hatching (angle, spacing,
etc.) By the time you get to Wildfire, you have 'Tools>Model sectioning' which
lets you create zones, envelopes and sections, lets you manage and edit them and
even create patterned sections, all in the same interface. So, my advice to one
and all is to get used, if you don't already do this, to creating/managing
sections in part/assembly mode. When the sections exist, you'll be given the list
of existing named sections in drawing mode to select from. All you need to make
sure of is that the view is placed so that the section is parallel to the screen.
If you have a problem with how it is cutting, go back to the model and flip the
direction of the cutting action. Any problems will be easier to see and manage in
the model.

David Janes

 

I can think of a few things you can do. You can modify the view type,
click on the view, accept the existing settings (e.g. Projection-Full
View-Section-Unexploded) then in the next menu change Total Xsec to
Area Xsec and click Done. That kind of section only shows what's been
cut.

If that's not want then instead of doing the above you want you can go
to Display Mode>Member Disp>Blank-Picked View and blank the components
from the view which you don't want to see. Or... instead of Blank you
can click on Style and make them PhantomTrnsp (although that may not
be what you want) Or...... under Style you can change the component to
a different user defined colour, which might be one linked to
particular pen width that you have set.

 

(Sorry, previous reply was a bit garbled. I'm a busy boy.)

I can think of a few things you can do. You can modify the view type,
click on the view, accept the existing settings (e.g. Projection-Full
View-Section-Unexploded) then in the next menu change Total Xsec to
Area Xsec and click Done. That kind of section only shows what's been
cut, not what's behind the cutting plane.

If that's not what you want then instead of doing the above you can go
to Display Mode>Member Disp>Blank-Picked View and blank the components
which you don't want to see.

Or... instead of Blank you can click on Style and make them
PhantomTrnsp (although that may not be what you want)

Or...... under Style you can change the component to a different user
defined colour, which might be one linked to particular pen width that
you have set.