The FeatureManager design tree on the left side of the SOLIDWORKS window provides an outline view of the active part, assembly, or drawing.
The FeatureManager design tree uses the following conventions:
- A
symbol to the left of an
item’s icon indicates that it contains associated items, such as sketches. Click
to expand the item. To collapse all expanded items at the same time,
click Shift+C, or right-click the
document name at the top of the tree and click Collapse Items.
- The Rebuild icon
precedes features, parts, and assemblies if a
change requires a rebuild of the model.
- The Lock icon
displays after the part name if the parts are frozen by the freeze bar.
- While a drawing view updates, the drawing icon changes to:
.
- In an assembly, each instance of the component is followed by a
number in angle brackets <n> that
increments with each occurrence.
- Sketches are preceded by:
|
(+)
|
Over defined
|
|
(–)
|
Under defined
|
|
(?)
|
Sketch cannot be solved
|
|
No prefix
|
Fully defined
|
- Errors and warnings display next to the part, feature, and sketch icons. The
What's Wrong? dialog box and tooltips describe the
errors and warnings:
|
|
Error in the model
|
|
|
Error with the feature
|
|
|
Warning underneath the node
|
|
|
Warning with the feature
|
- Positions of assembly components are indicated by:
|
(+)
|
Over defined
|
|
(–)
|
Under defined
|
|
(?)
|
Not solved
|
|
(f)
|
Fixed (locked in place)
|
- Assembly mates are preceded by:
|
(+)
|
Involved in over defining the position of components in the assembly
|
|
(?)
|
Not solved
|
- For the state of external references, the following symbols display after the
name of the part or feature:
|
–>
|
External reference
|
|
-> ?
|
Out-of-context external reference
|
|
-> *
|
Locked external reference
|
|
-> x
|
Broken external reference
|
To hide the x symbol, click and clear Show "x" in feature tree
for broken external references.