Orienting a twisted part in Drawings 2

[dedevo]

I have a complex part that I broke up in to several pieces, did a "Save Bodies" and made it in to an assembly for detailing properly in my drawings.

However, when doing "Save Bodies" the part shows up with a common origin to the assembly, and it is all disoriented.

I have attached one of these parts as an example.

I want to be able to get views that are "Normal To" a face, but I also want the lines to be vertical/horizontal.
Is there a way to rotate the part slightly (in the drawing view) without modifying the part itself? (ie. no "Move Part")

Devon Murray, EIT [Mechanical]
Solidworks 2011 SP 2.0

 

[MadMango]

Pick a face that you want be Front, then in the View Orientation add a new custom view. You might have to select another face to get things square. Insert these new custom views into your drawings.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[CorBlimeyLimey]

http://help.solidworks.com/2011/Eng...gacyhelp/sldworks/drawings/aligning_views.htm

 

[CorBlimeyLimey]

For the part you posted, you would need to align one edge, then create a second view at 90°, and realign another edge.

MadMango's suggestion would be simpler and (semi)permanent.

 

[ArtL]

dedevo You have "plane1" click on that plane and click on "normal to" with plane1 highlighted. the part then is square to
the computer screen. use alt or control plus the arrow keys to move part around square to screen as you want.

 

[SnowCrash]

Another way is place a coordinate system at the corner, properly aligned with the part, export using the new coordinate system and import back in; it should be right.

--
Hardie "Crashj" Johnson
SW 2011 SP 2.0
HP Pavillion Elite HPE
W7 Pro, Nvidia Quaddro FX580

 

[dedevo]

Nearly every tutorial I found about this didn't quite do what I wanted it to do.

I found one burried on another page:
In the part/assm, select the face you want to be normal
Ctrl+Click the face you want to be the new Top
Then do "Normal To"

After that, setting the views was just another step.

I needed the parts properly oriented so my ISOs would turn out. I guess the title was misleading; I needed to orient more than just the drawing.

Devon Murray, EIT [Mechanical]
Solidworks 2011 SP 2.0

 

[CorBlimeyLimey]

Once the main drawing view was created (per my post), the ISO's projected from it would be correct.

There is no right or wrong way ... use whatever works best for you.

 

[rbpmc]

Any advise on this subject when working with cylindrical parts?