Simple sweep with guide curve

[westrock]

I'm just learning Solidworks and am stumped by a very simple problem. I am attempting to sweep a triangle using a guide curve. Perhaps I have missed a step; here's what I have done.

- On the front plane created a straight path.
- Above the path on the same plane created a simple guide curve.
- Dimensioned the path and guide curve fully; the start and end points of each are vertical with proper relations.
- On the side plane created a triangle with equal sides and a dimensioned bottom.
- Created a "pierce" relation between the bottom center of the triangle and the path.
- Created a "pierce" relation between the top of the triangle and the guide curve.

When attempting the sweep, the profile (triangle) will select no problem but when attempting to select the path nothing happens. If I remove the guide curve the trangle sweeps along the path no problem. If I remove the original guide path then the triangle will sweep along the guide curve no problem. There do not appear to be any intersections or obstructions withing the possible sweep. What am I missing.

 

[Theophilus]

For whatever reason (?) you cannot have two usable curves in the same sketch. What I do in this case is convert the entities of one of your curves to construction lines, exit the sketch, start a new one, and convert the construction lines into your new sketch. The end result is that you now have two separate curves in two separate sketches--which is--grievously--what you'll need to complete your sweep. The rest of what you mentioned sounds fine as best I can tell.



Jeff Mowry

http://www.industrialdesignhaus.com

A people who value security over freedom will soon find they have neither.

 

[westrock]

Seperate sketches for path, and guide curve; that was the key that I was missing. That simple fact is not in any of the literature that I have looked at. Much appreciated Jeff, thank-you.

Cheers....George Vancouver Island

 

[Eltron]

Also, the Pierce command isn't necessary for sweeps to perform properly.

Dan

http://www.eltronresearch.com

 

[mjcole]

If you are using 2008 the Selection Manager which can be activated by right click menu will allow you to do this with 1 sketch for path and guide and a second for the cross section or profile.

The select Group icon with 3 cursors shown will allow you to pick portions of a sketch instead of the entire sketch which causes the feature to fail.

Michael

 

[mjcole]

Selection Manager option

 

[westrock]

Thank-you Michael,
I am using 2004 so that option is not available. Although 2008 may be required as I am using art images from Adobe Illustrator which can be imported directly by 2008. I am attempting to convert Northwest native low relief carving images into Solidworks geometrics. Needless to say the complexity of surfaces, curves, and planes is intense so I have a steep learning curve ahead.