Best Practices for Sketch Project Link
@tookemtoni - do you mean "body to sketch"? Or, does "sketch to body" refer to "Project Curve to Surface"?
There are differences in stability of projections into a sketch. In rough order from most stable to least stable, it is something like this:
- projecting an Origin geometry into a sketch. Those projections will only fail if the component that owns the origin is deleted (and in the case of the root component origin, will never get deleted)
- work geometry derived entirely from origin geometry. Again, will never fail unless you delete that work geometry yourself.
- sketch geometry to a sketch. Again, with some exceptions, sketch geometry is never deleted unless you delete it yourself, so the projection is stable
- body to a sketch. Choosing the type as body for Intersect (the intersection of the body with the sketch plane), or regular project (silhouette of the body). That will not lose its reference unless the body itself goes away. However, the results of the projection can change if the body changes or moves, so you may get a different set of curves as a result
- face to a sketch. Within a body, faces are the most stable entities. Can obviously fail if the sketch geometry that produces that face is deleted, etc.
- edge to a sketch. An edge is basically tracking two adjacent faces, so you have double the chance of a failure if either face fails
- vertex to a sketch. This is tracked as 3 faces (in most cases), so has 3 possible points of failure.
The key to preventing most sketch projection failures is to be careful with your edits. If you are editing a sketch, try not to delete geometry, as that geometry is the basis for all downstream entity tracking. Don't delete anything (work geometry, features, etc) if you can avoid it. Edit features, parameters, dimensions, etc instead of delete and re-create.
The attached is from a class I did at Autodesk University with @Phil.E in 2020 that goes into some of this in more detail, if you are bored over the weekend...
Jeff Strater
Engineering Director
Jeff,
Perfect thank you for the list !!! It's pinned up next to my computer.
Debugging your Fusion Design: Let's get rid of those red and yellow features is an uncut gem. (Why isn't this on Youtube? I would have discovered all this information sooner.)
Dear Fusion 360 Community,
If you haven't read it or watched it, please do. It will save you a lot of time and frustration because there is a best way to make your model parametric so you don't cause an error. 👍
Here are some excerpts that I found very useful even after 100 hours with Fusion:
In Section 3
What Causes Fusion Design Errors?
".....When editing a sketch, try as much as possible to preserve the geometries in
that sketch. Don’t delete and re-create sketch geometry. Preserving the original sketch
object preserves the feature that uses it."
In Section 5.1.1
Minimize Unnecessary Dependencies
“....Turn off the sketch preferences which “automatically” create references”
“...Sketch dimensions and constraints are even worse, because there is no
preference that actually disables auto-projection – it happens unconditionally.
So, be careful when creating/placing sketch dimensions and constraints – don’t
accidentally select an edge to dimension to if it is not absolutely necessary to
dimension to that edge. Sadly, you may need to turn off body visibility, or make
the body un-selectable temporarily to prevent this”
“...Be mindful when creating any feature of only picking geometry when that
relationship is actually required to achieve your design intent. Often, that
reference is not necessary, and your design intent can be more stably achieved
using methods like referencing a user parameter.”
In section 5.1.4
Using Parameters Instead of Dependencies
“...One advantage of a parametric design CAD application is: It contains parameters…
And, in many cases, you can use parameters to avoid having to reference geometry....”
In Section 6.1
Design Iterations
“...Always throw away the first version, and re-do it”
In Section
6.2.1 Name everything
“...Unfortunately, Fusion has no way to put comments on features in the Timeline. So, the
only way to put information on these items is to put it into the feature name. I find this
very helpful for myself, when I come back to a design that I worked on a long time ago, I
can easily find which sketch matches to which feature, and what the feature is for. This
can result in very long feature names, but to me this is worth it.
I can highly recommend the add-in DirectName to help with this
