|Localização do menu|
|Sketcher → Validate sketch|
|Introduzido na versão|
The Validate sketch utility can be used to analyze and repair a sketch that is no longer editable or has invalid constraints, or to add missing coincident constraints to a sketch created from imported geometry such as DXF files. It can also be useful to locate a missing coincidence in a native sketch that generates a "can't validate broken face" error when trying to apply a PartDesign feature.
The Sketcher validation task panel
- This tool cannot be used on a sketch that is in edit mode. If required exit edit mode by doing one of the following:
- Select the sketch to be validated from the Tree view or by clicking on one of its edges in the 3D view.
- To open the validate sketch utility do one of the following:
- Select the Sketch → Validate sketch... option from the menu.
- Press the PartDesign Workbench). button (not available in the
- See Options below for the available operations.
- Press the button when done.
Finds out missing coincidences for overlapping vertices, and adds them. Press thebutton; a pop up dialog will appear to report how many missing coincidences were found; they will be shown in the 3D view as yellow crosses. Press to close the dialog, then press the button to add the missing coincidences.
If necessary, define a larger tolerance value in the drop-down field.
Pressto highlight vertexes that are outside this tolerance.
This tolerance is also used by the/ process.
Leave the "Ignore construction geometry" checkbox checked to disregard construction geometry in the analysis.
Checks for malformed constraints.
For example, if there is a Circle-Line-Tangent constraint, but it references two lines, it is considered invalid.
(This sometimes happens due to the Topological naming problem, i.e. the external geometry changes type).
It also does other checks, such as for empty links.
Degenerated geometry can result from solver actions in a sketch.
For instance, if a line is forced to shorten to become almost a point.
Other examples: a zero length line or zero radius circle/arc.
Reversed external geometry
Reversed external geometry can happen because the handling of reversed geometry was changed around revision 0.15.
This process might be helpful if sketches with external-geometry fail to solve because of these changes.
Constraint orientation locking
Tangent and perpendicular constraints are implemented (via-point).
Internally they work by constraining the angle between tangent vectors. With tangent constraint for example, the angle can be 0 or 180 degrees (co-directed or opposed vectors). The actual angle is remembered in the constraint data ("constraint orientation is locked"), it guards against flipping. But the angle can be erased ("constraint orientation unlock") or updated; these tools do exactly that.
The locking mechanism typically works well and this tool should not be needed. It should only used after making a backup of the open document.