Sweep profile along path issues 2

[Dingo0z]

Hi,
I'm trying to sweep a closed profile along an open path. I've tried drawing the profile in one sketch & then the path in another. This didn't work for me. I also tried drawing both the profile and path together in a 3d sketch. This did not work either. The command I have been using is "Swept boss base". I have attached the file I'm working with. If there is anyone who thinks they can help, I would greatly appreciate your efforts. This is something we are going to build. (hopefully)

Thank you for your time,
-Dan

Solid works 2009

 

[ArtL]

Mr.Dingo You have to resolve all sketches, and lines, or down the road you will have problems of things moving when you don't want them to.

 

[ArtL]

Mr D Sworks 2011 ver

 

[Dingo0z]

Thankyou, thats exactly what I was trying to do. I was able to open the .IGS file, but not the 20011, because I'm using 2009. Can you save it as a 2009 version so I can better follow what you did? When you say "resolve" is that the same as fully defining the sketch so it's locked into place? Is that what was preventing it from working?

Also, is it fairly simple to get a pattern of the long flat edge thats at a approximate 45 degree angle within that radius portion of the crown? We are making this out of sheet metal. We can bend the straight sections on a brake press, but the radius portion will require cutting out & then welding all of the crown members together one piece at a time. When you look at the crown from the front, you'll see what I mean... there is only that wide angled piece within the radius that is difficult to make a pattern for without this program.
Thank you again for your help.
I'm gobbling up any bit of knowledge you are willing to share. This is really useful stuff!

 

[CorBlimeyLimey]

The end of the path was not meeting the Front Plane. The start point of the path must lie on the same plane as the profile. The path & profile do not have to intersect, but it is good practice to use the Pierce relation to ensure they do.

 

[Dingo0z]

At the risk of sounding like what I am (a new user). How do I make the path start point lie on the same plane as the profile? it looks like they are intersecting? I tried selecting the end point of sketch 2 that appears to intersect with sketch 1 and add a pierce relation but it rejected it saying "no intersection found for pierce point". I'm obviously missing something because on the surface it appears that these two sketches are lined up and share a point.
Can you help me understand?
Thank you for your assistance. It is valued and appreciated.
-Dan

 

[CorBlimeyLimey]

Activate Edit Sketch for the path.
Ctrl select the end point and the Right Plane, and set a coincident relation between the two. If you use the Measure tool you will see they are 0.00239962in apart.

With that done, the Sweep will work.

 

[CorBlimeyLimey]

BTW, it is good practice to base either (or both) the path or the profile sketch, on or around the Origin of the part.

 

[Dingo0z]

Thanks for helping me out of the box. I never would have thought of adding a relation between geometry and a plane. I thought it was just used for objects. You've opened a door for me.
Now to figure out how to get a pattern for that piece of crown I mentioned towards the top.

Thanks again for your help.
-Dan