Fusion
I don't see a link here. But, I can answer a few questions:
- "When I edit a sketch it doesn't center on the screen. Sometimes it isn’t even visible. What can be the cause of this phenomenon?" That is because the view always includes the sketch origin (the "cause"). We are reviewing possible solutions to this.
- "Why is the component sketch repositioned on that of the assembly when it is edited? Wouldn't it be possible to ban this phenomenon? On inventor or solidworks this does not happen." This is because when you edit a sketch, Fusion needs to roll back to the point in time when it was created. If you have moved the component afterwards, that movement will also be rolled back. It does not happen in Inventor or Solidworks, because you only edit sketches in a part environment in those tools, so there are no components to move. No, it is not possible to prevent this behavior.
- "For a few months now, there has been no normalization of the selected plane when creating a new sketch". Not sure what you mean by "normalization" here, but if you are talking about the "auto look at" behavior (rotating the view when editing a sketch), this is suppressed if you have 3D sketch on:
Jeff Strater
Engineering Director
@mac_ito wrote:It's a shame, but I don't understand why this is not possible when the phenomenon is not present when editing sketches of external parts ?.
That is because Edit in Place actually is editing a different document than what happens when you edit a local component. Notice that the timeline is different during Edit in Place. Edit in Place is similar to Open (where you edit the external design in a separate tab), but just takes place in the same tab. The external design in your video does not contain a move. If it did, the same thing would happen - Fusion always needs to roll back to the sketch to edit it.
Jeff Strater
Engineering Director
Yes, I see no way that this can change, as it is built into the very foundation of the way the Fusion timeline works. Any edit of a feature, T-Spline, or sketch has to roll back to the point in history where it was created. This is to prevent circular references from being created (for example, projecting an edge of an Extrude that consumes the sketch being edited, creating a cycle between the sketch and its own Extrude).
However, there are other ways to "edit" a sketch - if you make the sketch visible, you can drag geometry in the sketch, you can delete geometry, and, if you make dimensions visible, you can edit those dimensions, all without editing the sketch itself. You can also edit parameters of the sketch via the Parameter table. All of those activities can be done without rollback (because they cannot create those references). What you cannot do is create new sketch content. You must be editing the sketch to create geometry, new dimensions, or new constraints (because those operations can create references)
Jeff Strater
Engineering Director
