Sweep - won't cross a path

[susan458]

Hopefully the attached drawing will best explain - basically I am trying to sweep along the outside path, but can't get it to follow the path where it crosses itself.  I'm sure ther is an easy answer to this but just can't see it

[jeff_strater]

there is not an easy answer - sweep does not allow self-intersections.  I was able to do it in 6 different sweeps:

[susan458]

Even with your helpful timeline I am still not able to create any sweeps after the first, I just keep getting an error message, see attached image.

 

[KristianLaholm · Accepted solution]

I don't have an answer to your sweep problem, this is my suggestion on a completely different workflow.

If the design intent is creating a 2mm wide and deep cut with a round bottom I would use Extrude Thin and Fillet creating the cut.

I started over and did not use a primitive (box) as a starting point, everything based on sketches.
There is symmetri in the design and the start of the workflow is only 1/4 of the final body, makes it easier to select geometry and I'm lazy.

[susan458]

Thankyou, I had never seen "Thin" extrude before (and I use extrude all the time).    What a wealth of possibilities this tool will bring to my designs,   and I also liked your clever use of mirrors to save time. So thankyou again.

I am still curious how Jeff in the first reply managed to sweep the entire path from the one profile - I would love to know how that was done.

[jeff_strater]

the key is to not select the sketch profile, but to select the solid face from the end of the previous sweep.  Looking at the third one:

and then select the next section of the path (chaining off):

[g-andresen]

Hi,

The problem is caused by the sketch.
If you correct the double line and the connection to the circle segments, both pipe and sweep will work.

Screencast

günther