DesignSpark Mechanical Online Help

Sketching Constraints

You can choose constraint-based sketching to reduce the degrees of freedom (place constraints) on the drawing objects in 2D drawings and designs. Adding constraints restricts the type and range of movement of the objects, and links objects such that certain editing tasks on one drawing object will cause linked objects to be modified. Use tools in the Constraints group in the Sketch tab to add constraints to sketches.

Certain sketching tools included rudimentary tangency and coincident constraints (enabled with the Maintain Connectivity option), but these may be overridden during drawing editing. The tools in the Constraints group offer additional types of constraints which can be applied to any of the standard drawing objects (line, circle, arc, and so on) and are more robust.

To enable constraint-based sketching, select Enable constraint based sketching in the Advanced options in the DS Mechanical Options.

You can Save and Open models containing sketch Constraints. Designs that include Constraints will open in Sketch mode. Leaving Sketch mode will trigger the deletion of all constraint data. You need to save a copy of the sketch with constraints intact before solidifying if you intend to resume the design with constraints.

NoteAnnotation placed on a design, drawing sheet, or 3D markup. Notes contain text or symbols that you insert and can be connected to geometry by a note leader.:Sketch constraints are active only in 2D sketch mode. If you switch to 3D mode, existing constraint data is deleted. If you expect to edit constraints as part of your design workflow, you must save a copy of the sketch with constraints before switching to 3D mode.

The following Constraints can be added to your sketch:

• DimensionAnnotation on a drawing showing measurement of an edge or face. Use the Dimension tool to add measurements to your design, drawing sheet, or 3D markup.
• Coincident
• Midpoint
• Concentric
• Fixed
• Horizontal
• Vertical
• Parallel
• Perpendicular
• TangentLineA straight line, arc, or spline drawn in Sketch mode or on a layout plane. Lines have length but no area. When you pull a sketch into 3D with the PullTool used to distort or deform geometry. Use the Pull tool to offset, extrude, revolve, sweep, draft, and blend faces; or to round, chamfer, or extrude edges. When converting a sketch to 3D, pulling a line creates a surface and pulling a surface creates a solid. tool, lines become edges. that touches a curve (arc or circle) at only one point, without crossing over, and is perpendicular to the radius at the point of tangency. You can sketch a line tangent to a curve or you can sketch an arc tangent to a line or curve.
• Equal Radius
• Equal Distance

Notes:

• Most of these constraints require two selected drawing objects. The first selection is the target and will generally be moved to satisfy the constraint. The second is the anchor object and will generally remain in position. The cursor symbol changes to indicate the type of constraint and whether you are selecting target or anchor.

  For example:

  First selection for Parallel:

  Second selection for Parallel:

• Fixed, Horizontal and Vertical constraints require only one selected drawing object.
• The Fixed constraint tool acts as a toggle – click an object to apply, click a second time to remove.
• The Equal Distance constraint uses on-screen tool guides to determine the anchor and target. See the example below.
• Concentric and Equal Radius constraints propagate when modifying the curves.
• Equal Radius constraints are added automatically when you create multiple rounded corners using the Ctrl key and the Create Rounded CornerSee FilletRounded corner at the intersection of two lines or edges; concave intersection between two surfaces. Fillet refers to an interior corner; exterior corner is known as a round. You can draw a fillet using the Create Rounded Corner tool or by selecting the Fillet (Constant radius round) option from the PullTool used to distort or deform geometry. Use the Pull tool to offset, extrude, revolve, sweep, draft, and blend faces; or to round, chamfer, or extrude edges. When converting a sketch to 3D, pulling a line creates a surface and pulling a surface creates a solid. options. See RoundRounded corner at the intersection of two lines or edges. Round refers to an exterior corner; an interior corner is known as a fillet. Rounds and fillets are both called rounds. See Fillet, Constant-radius round, Variable-radius round.. (interior corner) or RoundRounded corner at the intersection of two lines or edges. Round refers to an exterior corner; an interior corner is known as a fillet. Rounds and fillets are both called rounds. See Fillet, Constant-radius round, Variable-radius round. (exterior corner) tool in the Modify group. All the rounds created this way maintain an Equal Radius constraint so that changing the size of one will change all of them.

  

By comparison, in normal sketching, the rounds are equal radius during creation only. After creation, they do not maintain an association and can have their sizes changed independently.

Adding DimensionAnnotation on a drawing showing measurement of an edge or face. Use the Dimension tool to add measurements to your design, drawing sheet, or 3D markup. constraints

1. Activate the DimensionAnnotation on a drawing showing measurement of an edge or face. Use the Dimension tool to add measurements to your design, drawing sheet, or 3D markup. constraint in the Constraints group.
2. Select an individual sketch object, or two objects as required for certain types of dimensions. MoveA tool used to translate or rotate geometry. the cursor away from the object to position the dimension. The normal behavior for applying and locating dimensions is observed. However, when applied as a constraint, if you attempt to edit one object, other objects may be modified to maintain the dimension constraint.

   Notes:

   • DimensionAnnotation on a drawing showing measurement of an edge or face. Use the Dimension tool to add measurements to your design, drawing sheet, or 3D markup. constraints may be used to modify the size of the selected object. After creating the dimension constraint, double click to select the dimension and then modify the value.
   • DimensionsValues or expressions you enter for precise control during the creation or modification of a design. You can dimension every element, from lines in sketches to faces of solids. See Ordinate dimensions, Progressive dimensions, Ruler dimension. may be positioned vertically, horizontally, or aligned with the object.
   • Angle dimensions are supported – select the first object and then hover over the second object until the angle dimension appears. MoveA tool used to translate or rotate geometry. the cursor to position the dimension.
   • ArcCurved line of constant radius; part of a circle. See Sweep arc, Three point arc, Tangent arc. length dimensions are supported – hold the Ctrl key while selecting the arc to create an arc length dimension. MoveA tool used to translate or rotate geometry. the cursor to position the dimension.

Adding an Equal Distance constraint

The Equal Distance constraint uses on-screen tool guides to determine the anchor and target distances, and to create the constraint. This is because more than one selection is often necessary to create the constraint.

1. Activate the Equal Distance constraint in the Constraints group.
2. With the TargetThe object you want to cut, when using the Combine tool to split a solid or surface. tool guide active, select your moveable drawing object or pair of geometries to define the first dimension.

   

   A dimension line with the target symbol is added to the design page.

3. Select the Anchor tool guide (or hold the alt key), and then select your stationary drawing object or pair of geometries.

   

   A dimension line with the anchor symbol is added to the design page.

4. Click the Complete tool guide to create the constraint.

   The target object will be modified as required.

NoteAnnotation placed on a design, drawing sheet, or 3D markup. Notes contain text or symbols that you insert and can be connected to geometry by a note leader.: A dimension between two lines will force the lines to be parallel.

ObjectAnything recognizable by the tools. 3D objects include vertices, edges, faces, surfaces, solids, layouts, planes, axes, and origins. 2D objects include points and lines. States

When using constraint-based sketching, you can make sketch objects under-defined, fully-defined, or over-defined.

• Under-defined objects have some degree of freedom and are highlighted cyan in the design window.
• Fully defined objects have no degrees of freedom and are highlighted dark blue in the design window.
• Over-defined objects are highlighted red in the design window. This also applies to dimensionally over-constrained lines. One or more constraints must be removed before you can proceed with your design.

Creating Multiple Sketches With Constraints

You can create multiple sketches with constraints on the same sketching plane. The active Sketch node is shown in bold in the tree and the active sketch is highlighted in the design window.

To activate a different sketch, select the Sketch node in the Structure treeDisplay in the Structure panel that shows you each of the objects in your design. You can expand or collapse the nodes of the tree to view the objects. You can rename objects, create, modify, replace, and delete objects, as well as work with components. and select Activate Sketch.

NoteAnnotation placed on a design, drawing sheet, or 3D markup. Notes contain text or symbols that you insert and can be connected to geometry by a note leader.: Constraints may be applied within sketches on the sketching plane.

Creating a New Sketching PlaneConstruction geometry consisting of a flat surface. Planes can be used for a 2D sketch, section view of a model, a neutral plane in a draft feature.

1. Click Select New Sketch PlaneConstruction geometry consisting of a flat surface. Planes can be used for a 2D sketch, section view of a model, a neutral plane in a draft feature. in the mini-toolbar, or right-click and select the Select New Sketch PlaneConstruction geometry consisting of a flat surface. Planes can be used for a 2D sketch, section view of a model, a neutral plane in a draft feature. option from the context menu.
2. Hover over any existing geometry to display existing planes.
3. Click to select the highlighted plane and display the sketch grid.

Existing sketches are solidified, and a new Sketch node is added to the Sketching PlaneConstruction geometry consisting of a flat surface. Planes can be used for a 2D sketch, section view of a model, a neutral plane in a draft feature. in the tree. The previous sketch remains active temporarily until you start sketching in the new Sketch.

NoteAnnotation placed on a design, drawing sheet, or 3D markup. Notes contain text or symbols that you insert and can be connected to geometry by a note leader.: Coplanar Sketch Constraints can reside on different containing planes.

Viewing Constraints

Select Show Constraint Tips in the Constraints group to view the constraints applied.

Hover over the constraint tip to see the type of constraint. The geometries involved will be highlighted dark blue.

If multiple constraints are applied, click the drop-down to see all the constraints applied.

Deleting Constraints

You can delete constraints using the Delete Constrainttool in the Constraints group or using the option from the mini-toolbar.

Using the Delete Constraint tool:

Select Delete Constraint in the Constraints group. The Delete Constraint tool is available when Show Constraint Tips is enabled.

Select the constraint to be deleted. In case of multiple constraints, click the drop-down and then select the constraint to be deleted.

Using the option from the mini-toolbar:

1. Right-click a drawing object.

In addition to the context menu, a mini toolbar appears at the cursor location.

2. Click the drop-down next to the Delete icon to see the list of active constraints on the selected drawing object. For example,

   

   NoteAnnotation placed on a design, drawing sheet, or 3D markup. Notes contain text or symbols that you insert and can be connected to geometry by a note leader.: If the drawing object is a point, the mini toolbar and drop-down will be simpler, containing only the point’s constraints. If multiple drawing objects are selected, the drop-down panel will contain the constraints common to all the selected objects.

   Alternatively, click the red X to delete a constraint. The list of active constraints is shown.

3. To check which geometries are involved in a constraint, hover over the constraint’s symbol in the drop-down panel. Geometries involved will highlight in red. For constraints involving a point, the point’s parent curve will highlight dashed as well, to help distinguish it from other overlapping points. If applicable, related constraints will highlight in yellow. Related constraints will be affected by changes to the highlighted constraint. Circles constrained to have equal radii could be an example of related constraints.
4. To delete a constraint, click the constraint’s symbol in the drop-down panel. The symbol will gray out. If the sketch was in an over constrained state, the sketch may adjust if a solution is now achievable.

Using MirrorAssociative relationship between two faces or planes mirrored about a centerline plane or planar face. The second object is a copy of the original; if the geometry of the original is changed, the mirrored copy is also updated. Use the Mirror tool to designate a face or plane as a mirror, or to create a mirror plane between two faces. With Sketch Constraints

1. With Constraint-based sketching active, sketch a line in the desired mirror position.
2. Use the right-click context menu, select Set as MirrorAssociative relationship between two faces or planes mirrored about a centerline plane or planar face. The second object is a copy of the original; if the geometry of the original is changed, the mirrored copy is also updated. Use the Mirror tool to designate a face or plane as a mirror, or to create a mirror plane between two faces. LineA straight line, arc, or spline drawn in Sketch mode or on a layout plane. Lines have length but no area. When you pull a sketch into 3D with the PullTool used to distort or deform geometry. Use the Pull tool to offset, extrude, revolve, sweep, draft, and blend faces; or to round, chamfer, or extrude edges. When converting a sketch to 3D, pulling a line creates a surface and pulling a surface creates a solid. tool, lines become edges. to set up the mirror.

3. With multiple MirrorAssociative relationship between two faces or planes mirrored about a centerline plane or planar face. The second object is a copy of the original; if the geometry of the original is changed, the mirrored copy is also updated. Use the Mirror tool to designate a face or plane as a mirror, or to create a mirror plane between two faces. Lines, entities are mirrored about each mirror line whether they are perpendicular or not.

4. To stop creating mirror constraints, uncheck Set as MirrorAssociative relationship between two faces or planes mirrored about a centerline plane or planar face. The second object is a copy of the original; if the geometry of the original is changed, the mirrored copy is also updated. Use the Mirror tool to designate a face or plane as a mirror, or to create a mirror plane between two faces. LineA straight line, arc, or spline drawn in Sketch mode or on a layout plane. Lines have length but no area. When you pull a sketch into 3D with the PullTool used to distort or deform geometry. Use the Pull tool to offset, extrude, revolve, sweep, draft, and blend faces; or to round, chamfer, or extrude edges. When converting a sketch to 3D, pulling a line creates a surface and pulling a surface creates a solid. tool, lines become edges..

Notes:

• Splines are not supported with a MirrorAssociative relationship between two faces or planes mirrored about a centerline plane or planar face. The second object is a copy of the original; if the geometry of the original is changed, the mirrored copy is also updated. Use the Mirror tool to designate a face or plane as a mirror, or to create a mirror plane between two faces. LineA straight line, arc, or spline drawn in Sketch mode or on a layout plane. Lines have length but no area. When you pull a sketch into 3D with the PullTool used to distort or deform geometry. Use the Pull tool to offset, extrude, revolve, sweep, draft, and blend faces; or to round, chamfer, or extrude edges. When converting a sketch to 3D, pulling a line creates a surface and pulling a surface creates a solid. tool, lines become edges., but the other Sketch tools are.
• A Fixed constraint is automatically applied to the mirror line to ensure more predictable dragging. It is possible to delete this constraint but dragging behavior may deteriorate.
• Equal Radius constraints are made automatically when creating multiple Rounded Corners with a MirrorAssociative relationship between two faces or planes mirrored about a centerline plane or planar face. The second object is a copy of the original; if the geometry of the original is changed, the mirrored copy is also updated. Use the Mirror tool to designate a face or plane as a mirror, or to create a mirror plane between two faces. LineA straight line, arc, or spline drawn in Sketch mode or on a layout plane. Lines have length but no area. When you pull a sketch into 3D with the PullTool used to distort or deform geometry. Use the Pull tool to offset, extrude, revolve, sweep, draft, and blend faces; or to round, chamfer, or extrude edges. When converting a sketch to 3D, pulling a line creates a surface and pulling a surface creates a solid. tool, lines become edges..

• To delete MirrorAssociative relationship between two faces or planes mirrored about a centerline plane or planar face. The second object is a copy of the original; if the geometry of the original is changed, the mirrored copy is also updated. Use the Mirror tool to designate a face or plane as a mirror, or to create a mirror plane between two faces. (Symmetry) constraints individually, click on an entity to open the mini toolbar. Individual constraints can be removed using the Delete dropdown menu.

NoteAnnotation placed on a design, drawing sheet, or 3D markup. Notes contain text or symbols that you insert and can be connected to geometry by a note leader.: 1D Patterns and 2D Patterns are not supported for Constraint-based sketching.

Referencing Existing Geometry

It is possible to create constraints and dimensions to cross sections and edges that lie in the sketch plane. Such cross sections and edges are treated as reference curves and will not be changed. Creating a Sketch Constraint or dimension requires at least one non-reference curve to allow for the constraint to be satisfiable.