Display/Delete Relations in Solidworks

Display/Delete Relations in Solidworks is your primary tool when dealing with sketch relations. It is particularly useful for sorting relations by the various categories shown in Figure 1.1. The capability to show sketch relations in the graphics window is nice, but sorting them in a list according to their state, with the capability to delete all in any particular state, is very useful.

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Figure 1.1. The Display/Delete Relations Property Manager

Sketch relations in the Display/Delete Relations dialog box can be divided into the following categories:

All in this sketch. Shows all the relations in the active sketch.

Dangling. Shows only the dangling relations. Dangling relations appear in a brownish-green or olive color, and represent relations that have lost one of the entities that drives the relation. You can repair dangling relations by selecting the entity with the dangling relation, and then dragging the red dot onto the entity to which it should have the relation.

Overdefining/Not Solved. Overdefined relations are any set of conflicting or redundant instructions that are given to a sketch entity, and appear in red. For example, if a line is collinear with an edge and vertical, but the edge itself is not vertical, then both the collin- ear and vertical relations appear in red.

The Not Solved condition often accompanies Overdefined. Not Solved typically refers to a dimension or relation that cannot be applied because of the conflict. The lower-right corner of the screen and the status bar show flags warning that the sketch is overdefined, as shown in Figure 1.2.

When an overdefined situation exists, all the relations and dimensions in a sketch often become overdefined. This can look like a daunting task to repair, especially when the entire problem is caused by a single relation. Do not automatically delete everything. Instead, try deleting or suppressing the last dimension or relation that was added, or a single relation that looks suspect. It is also a good idea to delete red relations before deleting yellow ones. Yellow simply means conflict, while red means a condition that cannot be applied. You can suppress a dimension by setting it to Driven in the right mouse button (RMB) menu, and you can suppress relations in the Display/Delete Relations Property Manager.

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  • External. External relations connect with an entity outside the active sketch. This includes the part Origin, or any model edges. The term external relations can also signify any relations outside of the part.
  • Defined in Context. Any relation between features in one part in an assembly and another part is considered an in-context relation.
  • Locked (Broken). External relations (outside the part) may be locked or broken to increase speed and to lock out parametric changes. There is no advantage of breaking relations rather than locking them. Both are ignored, but locked relations can be unlocked; broken relations can only be deleted. l Selected Entities. Sketch relations are shown only for the selected sketch entities.

Caution

Some of the relations listed in the Display/Delete Relations dialog box may be colored to signify the state of the relation. Unfortunately, colored relations are typically placed at the top of the list to attract attention, but when you select them, they are always gray, and so the advantage of color-coding is always defeated for the first relation in the list. The only way around this is to select a relation other than the first one in the list. If there is only one relation in the list, you cannot see the state color. 

A setting in Tool ➪ Options controls the display of errors. You can choose Tools ➪ Options ➪ FeatureManager to find an option called Display Warnings, where you can choose Always, Never, and All but Top Level. When a sketch contains sketch relations with errors, they display as warn- ing signs on the sketch, and will propagate to the top level of a part or assembly if you have selected the Always option.

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