Sweeping curves instead of profiles 1

[MechGrad]

Hi

I was wondering whether there is a method of creating a solid model by sweeping curves:

I created a curve that represents a cross-section of my geometry using imported x,y,z coordinates, and now I would like to sweep that cross-section through 90 degrees.

However, it appears that the sweep command needs a profile, and to the best of my knowledge a curve isn't considered as a profile.

Is there a way to do this? Or is there a way around this?

If you could help me on this, it would be great.

Thanks!

-S

 

[SBaugh]

When doing a sweep, a profile must be a closed sketch and the path...is well a path unclosed.

So I think you need to close the profile then if your path is setup right it should work.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[TheTick]

Make a 2D or 3D sketch, and use "Convert Entities" to copy your curve into a the sketch. Use the sketch in your sweep profile.

On justice and on friendship, there is no price, but there are established credit limits.

 

[meintsi]

What about using the suface-sweep command and then create your solid from your swept surface?

The swept profile does not need to be closed using surfaces.



Remember...
"If you don't use your head,
your going to have to use your feet."

 

[MechGrad]

Hi

Thanks for your replies on this issue. Although I converted the entities, it didn't really seem to work well. So I found a way around it using the loft command as follows:

1. Create the beginning and end cross-sections using spline curves based on the xyz coordinates.

2. Now, using a rotation matrix in excel (or some other spreadsheet program), create guide curves for the loft command by picking a particular point on your cross-section and rotating this point through your desired number of degrees

3. Repeat this process of guide curve creation for several points on your cross section. This way, you can mimick a sweep command. For my case, I chose points that would be at 0, 90, 180 and 270 degrees in the cross-section plane and I rotated these points through 90 degrees.

4. Now import all of these free curves into Solidworks and use the loft tool. It may take awhile for the program to build the solid model, but eventually it will work.

Hope that helps anyone else with the same problem.

-S

 

[TheTick]

Is your sweep path circular? If so, did a revolve feature not work?

On justice and on friendship, there is no price, but there are established credit limits.

 

[MechGrad]

Yeah, my sweep path was circular, however I couldn't use the revolve command. The error message stated that it needed a closed profile (which it was).

Anyway, the loft command worked splendidly

-S

 

[SBaugh]

One thing to use when you get an error like that "Closed profile (which it was)." Is to use the Tools\Sketch tools\Check Sketch for feature Then you can choose the type of feature and it will show you the problem with the sketch if there is one.

IHTH,


Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help