Does anyone have Solid Edge experience drafting/dimensioning bent tubes with copes on different compound angles on each end?
Currently I'm starting with a "top view," and using angled cutting planes to maneuver the projections into the coping planes while maintaining association between my projections, but it is rather ugly, and seems to be a "brute force" method. Is there a more elegant way of accompishing this? Ideally a method of projecting a new view at something other than 90 degrees along the fold line (it would be labeled so the two projections would still be associated). Unfortunately there does not seem to be much information available online, regarding proper practices for drafting copes on bent tubes in general, let alone specific to Solid Edge. Any suggestions would be greatly appreciated!
EDIT: I should mention, I'm on ST8. And I did find the "rotation angle" option under view properties/general, but as I'm dealing with compound angles it doesn't really help, since the rotations are not carried through to child projections.
EDIT Again: Sorry if my original post was unclear. I am using the xpress route tubing module, creating the geometry was easy enough (3D sketch then xpress route for the tubes, create rotated planes about each end for the cuts). I'm struggling to properly show the required views on a print.
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I believe this is one of the things the harness design option of the software gives you. In general, the ability to design and draft in terms of a tube bender. Length, bend, rotation, length bend etc. At least that's what I remember from a call to GTAC long ago. If you don't get a good response from one of the true pro's here like Imics or many others, I would call GTAC about it.
I'm assuming you are talking about difficulty of creaing views/dimensions of 'cuts' on compound angles.
I think its going to be a combination of section views (which can be put on a defined angle) and auxilliary view (which rely on existing edges of the model to define the angle). I haven't tried this but if you draw a line in view can you then use that line to define an aux view. You might also need to place a view using 'look at face' command in the orientation set-up.
Edit: Just tried it - you can draw a line in view and then use that to define the aux view direction.
Thanks for the responses everyone.
Are you using ST8? Under my view tab I don't have any sketcing options. Under the sketching tab I can create a line, but am unable to select it with the auxiliary view; aux only lets me select the tube centerlines.
I used the "look at face" command to determine my starting plane, but if I do that for multiple views I lose my view association. Section views have so far been the only way I can find to do it, but it's ugly - minimum of five different section views to get what I need. The tube has a single bend in it, but the coping cuts on each end are on different compound angles.
Do you remember how you called out the cuts on the tube prints? That's where I'm stuck.
No - using ST7
RMB on the view then Draw in View.
In there you can sketch lines, then when you exit draw in view you can use them for aux view orientation.
Once you have the view created you can go back into draw in view and hide the line(s) by moving it (and any dimensions you might have created) to the layer "Auto Hide".
Edit: can you post a picture of what you have at the tube end.