Ballfreak10 wrote: ↑Sun Jul 04, 2021 11:26 am
So I was able to get the Sweep operation to complete until I added one small horizontal line at the bottom-left of the path sketch (In the file attached here)...and now I'm back to getting the same error!
Again, this is due to the self intersecting profile....
When working with sweeping non-tangential convex path, you need to be aware of how your profile is being sweep.
See the image below, the horizontal profile is intersecting with the convex curve profile
There are a few workaround and that depends on your design intent
Option 1: Creating a horizontal line that is tangent to the convex curve
The convex curve will change (either shrink vertically or grow horizontally)
Notice that how the profile on horizontal line no longer intersect the profile from the curve because the line is tangent to the curve
Option 2: Split the sweep into 2 feature (You will need either 2 sketch or using selection manager)
For the first sweep, sweep until the curve end point (red sketch)
For the second sweep, sweep using the face and the horizontal line (green sketch)
Depending on the design intent, you might need an additional extrude to get the horizontal end face
However, this option will cause the sweep on the horizontal line to have different profile than the original sweep profile (note the 0.25 and 0.24 dimension).
This is because in the second sweep, the face is forced to follow the horizontal line, hence the sweep profile is projected, causing the dimension to change
Option 3: Use Keep Normal Constant for your Profile orientation option
This will force the profile normal to be kept constant
But that note that this will produce a really "bad" geometry at the curve area
Each option will produce different result.
I believe Option 1 is the correct way for this case if you want to have a consistent sweep profile
!