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Aligned Cross Section.

joenjoe

New member
We know how to create a cross section view using a single "flat" plane through the part. However, we need to create an alignedcross section view whose cutting planeis bent at a differentangle at the center of the part. The resulting cross section view should appear to project both halves of the part to the same plane. I am not sure how to better explain this. Please see the image below showing the parent view. The red line represents the desired cutting plane. Any suggestions would be greatly appreciated.
 
Please forgive me. We are new to PRO-E and have had very little training.


Oldman, thanks but no, I actually need the alignedsection to be shown in a single view. This is common drafting practice for us to be able to show the different features (bolt holes in this case) which don't necessarily share the same centerline.


Charleskim, can you futher explain the process. (We are using Wildfire 3.0) I begin the View Manager, select New, name the view, and select Offset. From there, the choices are "One Side" or "Both Sides" and "Single". I am lost after that.


I have already created a plane corresponding to the angled portion. The vertical portion corresponds to the default FRONT plane. I even created a sketch on the right plane for the line (shown in red in my earlier attached graphic). I'm not sure if or when this sketch will be used.


Thanks for any further assistance you may be able to offer.
 
Basically with 'Offset'.
You are going to sketch the section line (like the red-line you have on picture above).


From 'Offset' selection, with 'Both Sides' & "Single'.


Then you select the plane to sketch on and orientation (Just like any other sketch).
Then you sketch the section line.


Hope this explains. BTW, I'm on WF2.
 
hi, firstly, make a projection of view shown, select the projected view, goto the properties select section, select 2d section ,click on plus sign(green colour),create new, select offset, done,name it (other then existing names ), select sketch plane(clickon view), select direction(u can flip also), use line from dash board to cut the part( like sketcher) , to display arrows go back from where u select section , u see arrow display option click in box below arrow displayand select the view in which u want arrow display. hopethis can solve ur problem


regards


singh
 
and in the end to face ahead propably your next question - this kinda view can be shown as unfolded in drawing mode only if you make it as general view, with X-section option as unfolded, as I remeber right. Right?
 
Thank you all for the help. You all saved us a lot of grief. We were finally successful in creating our aligned section view. I think our original problemwas trying to establish the cross-section in the part model mode and then trying to select that in the drawing mode. It seems as though it works much better starting in the drawing mode.
 
We actually have one question remaining on this subject. After successfully creating a projected view with an aligned section (please see attached graphic), I am not sure how to avoid having asolid centerline/symmetry line through the part as shown. If we were able to solve this problem, I know then how to show axes in this view to get the desired results. Any further suggestions?
 
Yes! That worked. Thanks, dr_gallup and everyone else. We are documenting these procedures as best we can so we can learn and remember as we go.
 

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