Caixa de dialogo

From FreeCAD Documentation
This page is a translated version of the page Sketcher Dialog and the translation is 3% complete.

Introduction

While a sketch is being edited, or, in other words, while a sketch is in edit mode, the Sketcher Dialog is displayed on the Task tab of the Combo view.

To put a sketch in edit mode see Sketcher EditSketch. To finish edit mode see Sketcher LeaveSketch.

The Sketcher Dialog has the following sections:

Tool parameters

introduced in version 1.0

Some tools add a parameters section at the top of the dialog. Available options and/or modes depend on the tool.

The parameters section of the Sketcher CreateLine tool

Solver messages

This section informs about the state of the sketch.

The possible messages are:

  • Empty sketch
  • Fully constrained
  • Under constrained: n DoF(s)
  • Redundant constraints: (#, #, #)
  • Over-constrained: (#, #, #)
  • Solver failed to converge

If a sketch is under-constrained the number of degrees of freedom (or DoFs) is indicated. Clicking the underlined text will select the under-constrained sketch elements. See Sketcher SelectElementsWithDoFs.

If a sketch has redundant constraints or is over-constrained the indices of the involved constraints are indicated. Clicking the underlined text will select them. See Sketcher SelectRedundantConstraints and Sketcher SelectConflictingConstraints.

The last three messages are displayed in red for a reason: they are warnings that should not be ignored. They indicate issues that must be addressed as they interfere with the solver.

The last three messages are not mutually exclusive. If more than one applies only the most important message, occurring lowest in the list, is displayed.

Available options:

Option Description
This button opens a menu:
  • Auto update: If checked, the whole document is recomputed after every sketch action. Not advisable for complex documents.

Advanced solver control

This section will only appear if you check the Show section 'Advanced solver control' option in the sketcher preferences.

Note that most of the options in this section are of no practical use. They can however help with testing and understanding the solvers.

Available options:

Option Description
Default solver The solver that is used for solving the geometry. LevenbergMarquardt and DogLeg are trust region optimization algorithms. The BFGS solver uses the Broyden–Fletcher–Goldfarb–Shanno algorithm.
DogLeg Gauss step This setting is only available for the solver DogLeg. It is the step type used in the DogLeg algorithm.
Maximum iterations If the solver needs more iterations to find a convergence to a solution, it will stop and output that it failed.
Sketch size multiplier If checked, the maximum iterations will be multiplied by the number of parameters. The idea is that bigger sketches would need more iterations to converge.
Convergence The threshold for the squared error. This error is used to determine whether a solution converges or not.
Eps/Eps1/Tau These settings are only available for the solver LevenbergMarquardt. You should only change something here if you fully understand how the LevenbergMarquardt solver works.
Tolg/Tolx/Tolf These settings are only available for the solver DogLeg. You should only change something here if you fully understand how the DogLeg solver works.
QR Algorithm During diagnosing the rank of the matrix is calculated which enables to further analyze the constraint system to determine if there are redundant/conflicting constraints. The rank revealing decomposition used in FreeCAD is QR. There are two algorithms: Eigen Dense QR is a dense matrix QR with full pivoting, which is the legacy proven algorithm that works very well but it is rather slow as the system grows. The Eigen Sparse QR algorithm is an optimization for sparse matrices (having lots of zeros), which is usually much faster, since FreeCAD's systems do have a lot of zeros.
Pivot threshold When doing a QR, values under the pivot threshold are treated as zero.
Redundant Solver The solver that is used during diagnosing to determine whether a group is redundant or conflicting.
Red. Max Iterations The same as Maximum iterations, but for the redundant solving.
Red. Sketch size multiplier The same as Sketch size multiplier, but for the redundant solving.
Red. Convergence The same as Convergence, but for the redundant solving.
R.Eps/R.Eps1/R.Tau The same as Eps/Eps1/Tau, but for the redundant solving.
R.Tolg/R.Tolx/R.Tolf The same as Tolg/Tolx/Tolf, but for the redundant solving.
Console Debug mode Setting to specify the verbosity of the console output.
Solve This button explicitly starts the solver.
Restore Defaults This button restores the default solver settings.

Constraints

This section lists the constraints in the sketch. Unchecking a constraint in the list will hide it in the sketch. Constraints can be selected in the list as well as in the sketch.

Constraints can also be (un)hidden with Sketcher SwitchVirtualSpace.

Available options:

Option Description
Filter If the Filter checkbox is checked the Filter dropdown list controls which constraints are listed:
  • All: All constraints.
  • Geometric: Geometric constraints.
  • Datums: Driving dimensional constraints. Does not work properly: all dimensional constraints are filtered.
  • Named: Named constraints. Does not work.
  • Reference: Driven dimensional constraints. Does not work.
  • Selected constraints: Constraints selected in the sketch.
  • Associated constraints: Constraints associated with elements selected in the sketch.
This button toggles the visibility of the listed constraints in the sketch.
This button opens a menu:
  • Auto constraints: If checked, some geometric constraints are applied automatically to new elements.
  • Auto remove redundants: If checked, new constraints that are redundant are automatically removed.
  • Show only filtered Constraints: If checked, only the listed constraints are shown in the sketch.
  • Extended information (in widget): If checked, extended information is added in this form:
[(GeoID1,PosID1),(GeoID2,PosID2),(GeoID3,PosID3)]
GeoID is a zero-based index for non-external geometry. The X axis has GeoID -1, the Y axis has GeoID -2. GeoID -3, -4 etc. are used for external geometry.
PosID can have the following values:
0 = edge, 1 = start point, 2 = end point, 3 = center point.
For example a dimension from the origin to the center of a circle that is the 2nd non-external element in the sketch will have this extended information:
[(-1,1),(1,3)]
  • Hide internal alignment (in widget): If checked, constraints associated with internal alignments are hidden in the list. The Show/Hide internal geometry tool can also hide these constraints, but will also hide the internal alignments in the sketch.
Context menu Right-clicking the background of the list, or right-clicking constraints selected in the list opens a context menu. The menu has the following options:
  • Change value: Changes the value of a dimensional constraint. Only works for a single constraint. You can also double click the constraint in the list, or double click its value in the 3D view.
  • Toggle to/from reference: See Sketcher ToggleDrivingConstraint.
  • Deactivate or Activate: See Sketcher ToggleActiveConstraint.
  • Show constraints: Same as checking the constraint checkbox. But, unlike the checkbox, also works for more than one constraint.
  • Hide constraints: Same as unchecking the constraint checkbox. Idem.
  • Select Elements: See Sketcher SelectElementsAssociatedWithConstraints.
  • Rename: Renames the constraint.
  • Center sketch: Centers the 3D view around the selected constraints.
  • Delete: Deletes the selected constrains. The Del key can also be used.
  • Swap constraint names: Swaps the names of selected constraints. Only works if two constraints with user given names are selected.

Elements

This section lists the elements in the sketch. Unchecking an element in the list will hide it in the sketch. Elements can be selected in the list as well as in the sketch.

Available options:

Option Description
Filter If the Filter checkbox is checked the Filter dropdown list controls which elements are listed:
  • Normal: Normal geometry: geometry that does not fall in the next three categories.
  • Construction: Construction geometry.
  • Internal: Internal geometry.
  • External: External geometry.
  • All types: All geometry types. Specific types can be selected in the rest of the list:
    • Point
    • Line
    • Circle
    • Ellipse
    • Arc of circle
    • Arc of ellipse
    • Arc of hyperbola
    • Arc of parabola
    • B-Spline
This button opens a menu:
  • Extended information: If checked, extended element information is provided.
For non-external geometry the information in the list then changes from:
<N>-<TYPE>
to:
<TYPE>(Edge<N>#ID<GeoID>#<VLX>)[-Construction]
<TYPE>: Element type.
<N>: A 1-based index that indicates the creation order of the element.
<GeoID>: See under Constraints.
<VLX>: Element layer. See below.
Each element in the list has 1 to 4 buttons organized in 4 columns. These select a specific part of the element. Only applicable buttons are shown.
  • Button in column 1: Selects the edge of the element.
  • Button in column 2: Selects the start point of the element.
  • Button in column 3: Selects the end point of the element.
  • Button in column 4: Selects the center point of the element.

Clicking the text has the same effect as clicking the first available button of the element.


In the image the edge of a line and the center of an arc have been selected.
The line does not have a button in column 4 as it does not have a center.

Context menu Right-clicking the background of the list, or right-clicking elements selected in the list opens a context menu. The menu contains the Geometric constraint tools, the Dimensional constraint tools and the following additional options:
  • Toggle construction geometry: See Sketcher ToggleConstruction.
  • Select Constraints: See Sketcher SelectConstraints.
  • Select Origin: See Sketcher SelectOrigin.
  • Select Horizontal Axis: See Sketcher SelectHorizontalAxis.
  • Select Vertical Axis: See Sketcher SelectVerticalAxis.
  • Layer: 3 layers are available:
    • Layer 0: Indicated as VL0 in extended information. This is the default layer. Elements on this layer are displayed with a solid line type.
    • Layer 1: Indicated as VL1 in extended information. Elements on this layer are displayed with a dashed line type.
    • Hidden: Indicated as VL2 in extended information. Elements on this layer are hidden in the sketch.
The rendering order of layers 0 and 1 is such that when picking coincident points in the 3D view elements on layer 0 are selected in favor of those on layer 1.
  • Delete: Deletes the selected elements. The Del key can also be used.