Is there a way to display cross breaks in a isometric or orthogonal view? I can display cross breaks in flat pattern, but not in any view that represent of finished part.
You can display the sketch that is used in the cross brake.
Right click on the drawing view, and select properties. In the display tab, in the parts list, right click on the part, and click "List Sketches". With the sketches now displayed in the list, select the cross brake sketch, and select the "Show" checkbox on the righthand side of the listbox.
unfortionatly, that sketch is also used for three other things. This is the first time I was aware that combining model sketches was a bad thing for drafting.
If you've got everything combined into one sketch and do not want to create another, cut and paste back and forth, break the cross brake feature, etc... you can create a Tear-Off sketch and select just those elements you want to see in the new sketch.
A tear-off sketch will maintain associativity with the original sketch, so that if you change the cross brake location for example, it will move with your changes. I sometimes use this also to get sketch elements in my master sketch onto one side or the other of the actual sheet metal model material thickness, so it displays correctly in iso views on my drawing. (Using parallel plane option in the Tear-off sketch.
I'm not sure if this is what you are looking for but...
I change my cross-break sketch into an "etch" under the sheet metal Dimple tab. And then this can be turned on or off, independantly for each file (psm & asm) by right clicking, selecting show/hide components, and then selecting curves. For dft, the option is in Properties, at the bottom of the menu of the Display tab, there is a box "Use configuration or model view...", this will allow you to turn them on or off.
And now that they have the "Create Blank" feature, you can still flatten it