Actually, I'll respond here because this may be valuable information for others.
To be honest, I did not watch the video closely when I replied. My mistake...
The problem here is related to the way that Stitch works in Fusion. When you specify a tolerance in Stitch, Fusion does not move the edges of the surfaces at all. Instead, it creates what we internally call "tolerant edges". Normally, an edge is an infinitely thin curve. However, a tolerant edge can be visualized as more of a tube, with the diameter of the tube being the necessary tolerance to join it to other edges, and the centerline of the tube as the source edge curve. The tolerance you put into Stitch is the maximum size of that tube that you will allow.
So, the stitch succeeds, but contains these tolerant edges. The BRep surface itself is generally OK to work with, but you may encounter downstream problems with the model (if it's a solid, booleans can fail, to-face terminations can fail, etc).
But, in the case of the Sketch Project Intersect command, we have a problem. We are projecting the intersection of the sketch plane with the body, which in most cases, is the intersection with the faces, and those are in their original positions.
Here's an exaggerated view of what is happening. Here are some faces that have gaps between them:
And here is my interpretation of what happens when you stitch those faces with a large tolerance. The red tubes are the tolerant edges. But, the faces have not changed at all:
If we have a sketch plane in the middle:
This is what the intersection will look like:
In your case, you will see that the distance between the sketch points is within the tolerance (0.001) that you specified:
Hope this helps clear up what is going on. The real problem is in the source data for this model. It's pretty inexact, is my guess.
Jeff
Jeff Strater
Engineering Director
