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

Reply to
Kuntal Jain
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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

Reply to
David Janes

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

Reply to
Kuntal Jain

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

Reply to
dakeb

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

Reply to
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.

Reply to
Gra-gra

(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.

Reply to
Gra-gra

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