I can’t decide if I am doing something wrong, or if this is another SW bug. (2022 SP5.)
I am trying to create a detail view, and I want the profile to be a square instead of a circle. I am attempting to follow the instructions in this old video:
Please see the GIF below. I can create the detail view without issue. I can “edit sketch”, delete the circle and replace it with a square, but after doing that, the detail view still shows a circular profile. When I click on the sketch and try and select the “Profile” radio button, it is greyed out and I cannot select it.
I know I’ve found a way to fight through this in the past, but I cannot remember the magic steps.
I didn’t look at the YouTube video, but you’re trying to do it the hard way.
Sketch your shape first, then with that selected insert the Section View. At first the outline may still be a circle, but if that happens selecting “Profile” instead of “Circle” at the top of the property manager will fix it.
The workaround I found was to leave the circle, but trim it. Then I could select “profile”. (But I still couldn’t delete the circle and replace it with a square.)
Edit the profile circle, delete the sketch circle…sketch another shape then exit sketch. Then you have to change the Style to something other than “Standard” or “Broken Circle”, like “with leader” which then allows you to select the profile option.
They definitely need to cleanup the UI and process, its been unchanged for like 15 years.
If I recall right, early on you HAD to sketch the profile first before the Detail View button would allow you to select it, like most functions. Then they started adding the post selection stuff…which feels awkward in some cases like this.
You got to do it how Glenn said above, sketch the profile first, then select the lines and hit the detail view icon button to create the view. If you do it the way you showed in the GIF you automatically get the circle. I think you can go back and edit the circle to another shape after dropping the view on the sheet, but I never do it that way.
SPerman Ok, I see the bug when I watched your steps more closely. When you changed the Style to “With leader” and then edited the circle sketch to a rectangle, it won’t keep the change and reverts to a circle, with profile still greyed out. If you change the style to “Per Standard”, then edit the sketch to a rectangle, then change the style back to “with leader”, you can select Profile.
I guess my “old school” SolidWorks baggage never took me down this workflow…I always pre-sketch the rectangle then select the Detail View command.
I forgot to mention it earlier, but the reply above from jcapriotti reminded me. I don’t know which version you’re using, but beginning with SW2023 you can set the Style in the document properties (and of course in your Drawing Templates).
I’ve been wanting that for a long time. It might seem like a small thing, but I was getting very tired of changing the Style every stinking time I created a Detail View.
