I need to create a detailed view but i need it to be some other shape than a circle.
As Kenneth B. suggested, but draw the sketch first.
I always use ASME/ANSI standard views.
Under Style select "Profile"
Solidworks will not allow me to chose this option. It stays on circle no matter what i do. Profile stays grey.
Change Style to one of these ...
You have to draw the profile first.
See attached video.
Edit: and then I saw that Chris said the same thing.....well....the video is here anyway.
Make sure you have the Style set to either:
Using Per Standard or Broken Circle will not allow you to select the Profile option.
Solidworks will not allow me to chose this option. It stays on circle no matter Style: i chose. Profile stays grey.
Randall Dickerson wrote: Solidworks will not allow me to chose this option. It stays on circle no matter Style: i chose. Profile stays grey.
Randall Dickerson wrote:
De-select the option shown below at Tools > Options > System Options > Drawings.
You can edit an existing detail view originally created as a circle to another enclosed shape. May help if you have information on your existing detail you do not want to re-create.
Edit the sketch of the circular detail.
Delete the circle currently defining the detail area.
Draw your new detail geometry. Make sure it is an enclosed region/contour.
Before exiting the sketch, Make sure your newly created sketch entities are selected. Using a window selection works best.
Exit sketch and you should be able to change your style to With Leader, No Leader, or Connected and the Profile selection will be available.
Prior to setting the detail to be Profile, it will show as an over-sized circle. This should update after you select Profile.
Retrieving data ...