In earlier versions of SOLIDWORKS there has been some inconsistency in handling the availability of geometry referenced by assembly level features and mates; we have made improvements in 2019 to make them work more seamlessly. Let’s take a look through this simple example.

Before SW2019: Features affected by assembly feature

1. We start with an assembly with a simple part and an assembly hole

2. Add a reference plane “PLANE1 on FACE1” on top of the face “FACE1”

3. Add an assembly cut to cut off the “FACE1”

4. Suppress/unsuppress  “PLANE1 on FACE1” to force it to update; a rebuild error will appear for the plane. It is kind of reasonable since the referenced face              “FACE1” is not available, though you may ask why a later feature should affect a previous feature.

5. But if we suppress “Hole1” first, then Suppress/unsuppress “PLANE1 on FACE1”, the error is gone. “Hole1” looks totally irrelevant, but why it could affect the      outcome?

6. Now add another reference plane “PLANE on FACE2” on top of the face “FACE2” and add another assembly cut to cut off  “FACE2”

7. Suppress/unsuppress the newly added “PLANE on FACE2”, this plane will show an error too. The assembly cut “Cut-Extrude2” is created after the  “PLANE on FACE2”, why should a later feature affect a feature created earlier?

Before SW2019: Mates affected by assembly feature

1. We start with an assembly with two simple components. Add a distance mate between two faces of the components

2. Now add an assembly cut to cut off the face “FACE1”. There is no error for mate “Distance1”

3. Add another distance mate referencing the newly created “FACE2”

4. And add another assembly cut to cut off “FACE2”, we can see error in the mate. Why the first mate has no error but the second one has?

In SOLIDWORKS 2019 beta 2, for all the above workflows, there will be no errors

Behind the scenes

In SW 2018 and earlier, SW has a mechanism to determine where to look for the geometry, at component level or at the assembly level. The unrelated feature “Hole1”, is part of the mechanism and unfortunately in this case it leads to inconsistent behavior. When geometry is cut off at the assembly level but still exists at the component level, you may see features/mates behave without any error; however if the geometry is created from an assembly cut and does not exist at component level, after it is cut off by another assembly feature (after the second assembly cut), SW is not able to get the geometry anywhere and will post an error for the feature.

In SW 2019, a new mechanism is used to access the geometry even it is cut off by a later assembly cut. When updating a feature or a mate in an assembly, all assembly features created after the feature/mate are temporarily rolled back internally, so that the geometry being referenced at the time the feature/mate is created is always available.