Using Display/Delete Relations

Display/Delete Relations is the primary tool for dealing with sketch relations. It is particularly useful for sorting relations by the various categories shown in Figure 6.1. The capability to show sketch relations in the graphics window is nice; sorting them in a list according to their state makes this feature even more useful. To show the sketch relation symbols on the screen beside the sketch entities, use the View ➢ Sketch Relations menu selection.

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

• All In This Sketch: This shows all the relations in the active sketch.
• Dangling: This 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 instructions that are given to a sketch entity; they appear in red or yellow. If a line has conflicting relations, but it can still meet the requirements, it turns yellow. If the sketch relations cannot be solved, it turns red.
  • When an overdefined situation exists as shown in Figure 6.2, 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 any single relation that looks suspect. 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 PropertyManager.

    

• 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 to breaking relations rather than locking them. Both are ignored, but locked relations can be unlocked; broken relations can only be deleted.
• Selected Entities: Sketch relations are shown only for the selected sketch entities.

In-context design, also called top-down, as well as locked and broken relations are covered in detail in Chapter 20, “Modeling in Context.”

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

Using Replace Entity

The Replace Entity tool enables you to swap out a particular sketch entity with all of the associated references further down the tree reconnected. When you extrude a rectangle into a solid, for example, all of the faces and edges that are created are given specific names so that the software can internally keep track of what references what. If you were to change one of the lines of the rectangle to an arc by making the line a construction line and drawing a new arc, then rebuilding the solid, any faces or edges that were built from the original line would now be different; and if any features like a fillet referenced the original edge, they would fail. Using Replace Entity makes sure that everything updates properly. It is easy to do, but in order for it to work, you have to actually use it. Here is a step-by-step procedure to help you see how the tool works:

1. Open a new part.
2. Sketch a rectangle on any standard plane, making sure one corner references the origin.
3. Extrude the rectangle to some depth.
4. Apply a Fillet feature to an edge parallel to one of the sketch lines, as shown in Figure 6.3.

   

5. Expand the Boss-Extrude1 feature in the FeatureManager so you can see the Sketch1 underneath it.
6. Right-click Sketch1 and select Edit Sketch.
7. Sketch a three-point arc across the line that is parallel to the filleted edge, as shown in Figure 6.4. Notice the new arc is displayed as a thinner line than the lines of the rectangle.

   

8. Manually convert the line under the arc to construction.
9. Use the Confirmation Corner to close the sketch. Notice that the Fillet feature fails.
10. Right-click Sketch1 and select Edit Sketch.
11. Convert the construction line back to a regular line.
12. In the menu, select Tools ➢ Sketch Tools ➢ Replace Entity.
13. Make sure the line is in the top box and the arc is in the bottom box, with the settings as shown in Figure 6.5.

    

14. Exit the Replace Entity command and exit the sketch. Notice that the Fillet feature now rebuilds properly.

Using SketchXpert

The SketchXpert, shown in Figure 6.6, can help you to diagnose and repair complex sketch-relation problems. The Diagnose button at the top creates several possible solutions that you can toggle through using the forward and backward arrow buttons in the Results panel. The Manual Repair button displays all the relations with errors in a window where you can delete them manually.

By selecting the option at the very bottom of the dialog box—always open this dialog when a sketch error occurs—you can make the SketchXpert appear whenever a sketch error occurs. To display the SketchXpert manually instead of automatically, you can access it by right-clicking in any sketch or clicking in the Over Defined warning on the right end of the status bar.

Dimensioning from Centerlines

In Figure 6.7, I have dimensioned from a centerline. Notice that the cursor changes and displays an R, which indicates that the next dimension will be radial and will be made with respect to the centerline. This means that if I select the center of one of the holes, it will be dimensioned from the centerline.When placing the dimension that originally went to the centerline, if I had placed it on the other side of the centerline, SolidWorks would have given me a diameter dimension on the cursor displayed with a D (for diameter). Selecting the circle itself cancels the function because that implies a diameter, not a distance from something.

If you want to get out of the Radial or Diameter Dimension mode, press Esc on the keyboard to revert to normal dimensioning. This feature works like automatic baseline dimensioning.

Sketching with Numeric Input

To use the numeric input, first enable it with Tools ➢ Options ➢ Sketch ➢ Enable On Screen Numeric Input On Entity Creation.

With the Create Dimension Only When Value Is Entered setting turned on, when you sketch a rectangle, for example, SolidWorks automatically dimensions the length and height of the rectangle. The catch here is that you must use click+click sketching. Click-and-drag cannot be used with this technique. After you click the first corner of the rectangle, SolidWorks will put up a numeric entry field; and if you enter a number, it will automatically put dimensions on the rectangle and prompt you to edit one of them. You can then key in another dimension for the other side of the rectangle.

Moving, Rotating, Copying, and Scaling Entities

• Move Entities Tool The Move Entities tool enables you to move selected sketch entities by either selecting From and To points or by entering XY coordinates for the move. When the Keep Relations Option is unselected, the Move tool automatically detaches sketch segments whose endpoints are merged, as shown in Figure 6.8. If Keep Relations is selected, SolidWorks moves the entities and tries to maintain the sketch relations and merged points. All the tools have a pushpin icon in the interface. You can use the tool multiple times in succession when the pushpin icon is pushed in; tools with the pushpin are deactivated after one use if the pushpin icon is not pushed in.

  

• Rotate Entities Tool The Rotate Entities tool rotates selected entities in a sketch in the same way that Move Entities works. You can drag the angle or enter it manually. The green checkmark icon is on the RMB, as shown in the cursor display in Figure 6.9.

  

• Keep Relations Option The Keep Relations option does not actually keep any relations—it deletes the Horizontal and Vertical relations in the sketch, as shown on the left in Figure 6.8—but it does keep the merged endpoints, as shown on the right in Figure 6.8. This can be useful, especially considering how many sketch relations it would take to make a sketch move like this naturally.
• Copy Entities Tool The Copy Entities tool works exactly like the Move Entities tool, except that it copies instead of moving. The Copy Entities tool enables you to copy selected sketch entities by either selecting From and To points or by entering XY coordinates to place the copy. SolidWorks copies the entities and tries to maintain the sketch relations and merged points.
• Scale Entities Tool Scale Entities is one of those functions probably best left alone. This is because the results are erratic and unpredictable, particularly if there are dimensions on the sketch. This tool works on a selection of entities, particularly on an isolated selection that is not connected to other entities in the sketch. The PropertyManager for the Scale Entities tool is shown in Figure 6.10.

Modifying a Sketch

The Modify Sketch tool has been available in SolidWorks for a long time, but it has been superseded by some of the newer tools, such as Move Entities. However, it still has some unique functionality that is not covered by any other sketch tool. Modify Sketch works on the entire sketch rather than on selections within the sketch. It works best if there are no external relations between sketch entities and anything outside the sketch. It can also work on a sketch without the sketch being active. While most feature and tool interfaces have been moved to the PropertyManager, Modify Sketch still uses a dialog box (shown in Figure 6.11) that floats in the graphics window.

The Modify Sketch dialog box enables you to perform the following functions:

• Scale About: The Scaling function in the Modify Sketch tool enables you to scale about either the part origin or the movable origin. The movable origin is shown with a black origin symbol with knobs on the ends of the axes and at the intersection. The movable origin can be moved and even snapped to entities that are internal or external to the sketch.
• Translate: The Translate function of the Modify Sketch tool enables you to click and drag to move the entire sketch or to select a point and move it to a specific set of coordinates that you enter. If the sketch is dragged onto an external entity and picks up an automatic relation, then a message may appear saying that you can now use Modify Sketch only for rotating the sketch because there is an external relation.
• Rotate: The Rotate function of the Modify Sketch tool enables you to position the movable origin to act as the center of rotation. You can rotate either by entering a rotation angle or by dragging with the right mouse button to rotate, as indicated by the cursor.

When you place the cursor over the knobs on the movable origin, the cursor symbols change to indicate the functionality of the RMB. These cursors are shown in action in Figure 6.12. The cursors enable rotation, mirroring about X, Y, or both simultaneously.

Copying and Pasting Sketch Entities

Probably the simplest way to copy sketch entities in a sketch is to select the entities and use Ctrl+C, Ctrl+V, or one of the many other methods available for this purpose (such as the RMB button menu, the Edit menu, or Ctrl+dragging). Copying with box dragging, lasso, Ctrl+A, or contour selection are all useful methods.

In addition to copying selected entities within an active sketch, you can also select a sketch from the FeatureManager and then copy and paste it to a selected plane or planar face (if you are not in a sketch to begin with). This creates a new sketch feature in the FeatureManager that is not related to the original, although it does maintain internal dimensions and relations. (External relations are not copied with the sketch.) This is particularly useful when setting up certain types of lofts that use several profiles that can be created from a single copied profile. Copying and pasting is a fast and effective method of putting sketches on planes.

A copied sketch is similar to a derived sketch (addressed later in this chapter), except that with a copied sketch, there is no link or internal relations; and with the derived sketch, the new and old sketches remain identical through changes to the original sketch.

Dragging Entities

If a selected set of sketch entities has no external relations, you can select it as a group and move it without distorting or resizing the sketch. For the best results with this technique, avoid dragging endpoints; drag an actual line.

Creating a Derived Sketch

A derived sketch is a parametrically linked copy. The original parent and derived sketches do not need to have any geometrical relation to one another, but when the parent sketch is changed, the dependent derived copy is updated to stay in sync.

To create a derived sketch, you can select a plane or planar face, Ctrl+select the sketch you want to copy, and then choose Insert ➢ Derived Sketch.

Once you create a derived sketch, you cannot change its shape or size; it works like a block of a fixed shape driven by the parent. However, you can change the position and orientation of the derived sketch. Figure 6.13 shows a derived sketch and its parent. Modify Sketch is a great tool to use for manipulating derived sketches that are not related to things outside the sketch, especially for mirroring or rotating.

Using Three Views

When you're building a model from images, it is often helpful to have three or more images from orthogonal views, similar to re-creating a part from a 2D drawing. If you have a left view and a right view, it may be a good idea to put them on planes that are slightly separated so the images are not exactly on top of one another, which makes them both hard to see. Putting them on slightly offset planes means that one will be clearly visible from one direction and the other visible from the other direction.

Each sketch picture must be in a separate sketch. Figure 6.15 demonstrates the use of multiple sketch pictures to trace the outline of a vehicle, with the partially complete model shown with the images.

Additionally, you can put multiple sketch pictures inside a single sketch. Both images will show up in the FeatureManager, and both can be displayed at the same time, although you may have difficulty if you want to put them on top of one another.

Compensating for Perspective

When taking digital photographs to be used as sketch pictures in SolidWorks, you have to consider how perspective affects the image. Perspective can make it difficult to size items in the foreground or background. If you are taking the pictures that will be used as sketch pictures, you can minimize the effects of perspective by standing farther away from the object and using zoom on the camera if possible.

Estimating Sharp Edges

When you are sketching an object, you usually draw theoretically sharp corners of the model. Real parts usually have rounded corners, so you may have to use your imagination to project where the 3D surfaces would intersect at an edge minus the fillets.

Reverse-modeling a part from images is not an exact science. It is better than not being able to put pictures into the sketch, but there is nothing about it that can be considered precise. Often, putting a ruler or size gauge in the image somewhere is useful.

Using Auto Trace

Auto Trace is an add-in that you can select by choosing the Tools ➢ Add-ins menu. Auto Trace is intended to trace between areas of contrast in sketch pictures, creating sketch entities. Activating the Auto Trace add-in activates a set of arrows at the top of the Sketch Picture PropertyManager. There is nothing to identify the functionality with the Auto Trace name.

Auto Trace works best with solid blocks of black and white in the sketch pictures. To achieve this, you may need to use image-processing software and reduce your picture to a two-color (black and white) bitmap, TIF, or PNG image. Even if this preprocessing gives perfect results, don't expect much from Auto Trace.

Using Stick Fonts

SolidWorks makes available the OLFSimpleSansOC Regular font for those times when you need a stick font in your sketch to drive CNC machinery.

Working in Color Display Mode

The Color Display Mode button is found on the Line Format toolbar. In drawings, you can use the Color Display Mode button to switch sketch entities on the drawing between displaying the assigned line or layer color and displaying the sketch status color. It has exactly the same effect in part and assembly sketches.

When you select the button, the sketch state colors are used. When the button is not selected, any custom colors that you have applied to the sketch entities appear. If the button is not selected and you have not applied colors to the entities, the default sketch state colors are used.

You can use sketch colors for emphasis, to make selected sketch entities stand out, or to make sketches with various functions immediately distinguishable. Color Display mode has an effect only on an active sketch. Once a sketch is closed, it returns to the gray default color for inactive sketch entities.

Assigning Line Color

Line color enables you to assign color to entities in an active sketch. The Color Display Mode tool determines whether the assigned color or the default sketch status colors are used. Chapter 28, “Using Layers, Line Fonts, and Color,” has more information on this functionality, especially related to drawings.

Using the Edit Sketch or Curve Color Tool

The Edit Sketch Or Curve Color tool can be found on the View toolbar. You can use the Edit Sketch Or Curve Color tool to assign color to an inactive sketch or to a sketch block to replace the default gray color. The color that you assign to sketches in this way displays only when the sketch is inactive. The sketches also follow the toggle state of the Color Display Mode button. For example, if the Color Display Mode button is selected, then inactive sketches display as gray. When the Color Display Mode button is not selected, then inactive sketches display in any color that you have assigned by using the Edit Color tool.

When you use this tool to color a sketch block, the block displays the color inside the active sketch. You cannot use the Line Color tool mentioned earlier to assign color to a block.

Assigning Line Thickness and Line Style

The Line Thickness and Line Style tools function independently from the Color Display Mode button, but they are still used only when the sketch is active. As soon as a sketch that contains entities with edited thickness and style is closed, the display goes back to the normal line weight and font.

To assign a thickness or a style, you can select the sketch entities to be changed, click the button, and then select the thickness or style. Although a single sketch entity may have only a single thickness or style, you can use multiple thicknesses or styles within a single sketch. Figure 6.17 shows a sketch with the thickness and style edited.

Line thickness and line styles are covered in more detail in the discussion of drawings in Chapter 30, “Creating Assembly Drawings.”

Working with RapidSketch

RapidSketch is meant to help you easily change sketch planes. As you move a sketch cursor over flat faces of a model, the faces highlight to indicate that you can start a new sketch there. Each new sketch appears in the FeatureManager.

The workflow with this tool is that you start in one sketch with RapidSketch activated. Activate a sketch tool, move the cursor over a plane or face, and a dark plane will appear to indicate you can start sketching on that plane. To move to another plane, the sketch tool must still be active, but not be in-progress on an entity (nothing attached to the cursor). This option makes SolidWorks sketching work more like Solid Edge, where it's easier to change to a new sketch.

Adding Sensors

You can add sensors in the SolidWorks FeatureManager for parts and assemblies by right-clicking the Sensors folder and selecting Add Sensor. You can find the Sensors folder at the top of the FeatureManager. If you cannot find the Sensors folder, make it visible by choosing Tools ➢ Options ➢ FeatureManager, and make sure the Sensor folder is set to Show.

You are not limited to using sensors only when working with sketches; you can use them outside of sketches in parts and assemblies to warn you when various types of parameters meet various types of criteria.

Figure 6.18 shows the Sensor PropertyManager. You can create sensors for measurements, simulation data, or mass properties. I included sensors in this chapter due to the measurement options, which enable you to select a dimension and set a range of values or criteria for which you want to be notified. The dimension can be a driving (black) sketch dimension, a driven (gray) dimension on a sketch, or even a driven dimension placed directly on solid geometry.

Figure 6.18 shows what happens when a sensor finds a condition that you asked it to notify you about.

In addition to turning sensor alarms on or off, you can suppress sensors when they are no longer needed or to improve performance.

Sensors are a great way to keep an eye on particular values, such as wall thickness or clearance between parts. You can use a sensor to monitor any value you want to monitor but don't drive directly.

Using Metadata for Sketches

Metadata in SolidWorks is nongeometrical text information attached to geometrical data. Metadata is particularly helpful as keywords in searches, in Product Data Management (PDM) applications, or as custom properties in drawing and tables. If you don't use metadata within your CAD documents, it can be easy to forget that it is there at all.

You can use the following items as metadata in SolidWorks files:

• Sketch and feature names
• Sketch and feature comments (access comments via the RMB menu)
• Custom properties
• Design Binder documents
• Tags for features (located in the lower-right corner of the status bar)

Metadata searches can be particularly useful in large assemblies or parts with long lists of features that you need to find or search through. You can conduct searches for metadata through the FeatureManager Filter at the top of the FeatureManager. The Advanced Search function in assemblies can also search metadata sources. SolidWorks Explorer is a good first-level data management solution that can search, display, and edit metadata and previews. Windows Explorer can also search properties and tags.

Creating Construction Geometry

In SolidWorks, the only construction geometry that can be created directly is the construction line. All other sketch entities can be converted to construction geometry by selecting the Construction Geometry option within the sketch entity's PropertyManager or by using the Construction Geometry toggle toolbar button.

SolidWorks terminology is inconsistent, because it sometimes refers to construction lines as centerlines. The two are really the same thing. Centerlines are used for revolved sketches and mirroring, but there is no difference between a centerline and a construction line in SolidWorks.

Construction geometry is useful for many different types of situations. I use it frequently for reference sketch data. You can make sketch relations to construction geometry, to create symmetry, and you can use it for layout sketches or many other purposes.

Navigating in Space

To start a 3D sketch, activate the 3D Sketch icon on the flyout under the 2D sketch icon; or, in the menus, go to Insert ➢ 3D Sketch. When drawing a line in a 3D sketch, the cursor and origin initially look like those shown in Figure 6.18. The large red origin is called the space handle, with the red legs indicating the active sketching plane. Any sketch entities that you draw lie on this plane. The cursor also indicates the plane to which the active sketching plane is parallel. In the XY graphic shown in Figure 6.19, the sketch is not required to be on the XY plane, just on an imaginary plane parallel to it.

Pressing the Tab key causes the active sketching plane to toggle between XY, YZ, and ZX. The active sketching plane indication does not create any sketch relations; it just lets you know the orientation of the sketch entities that are being placed. If you want to create a skew line that is not parallel to any standard plane, you can do this by sketching to available endpoints, vertices, origins, and so on. If there are no entities to snap to, you will need to accept the planar placement, turn off the sketch tool, rotate the view, and move one end of the sketch entity.

The biggest challenge with 3D sketches is visualization. It can be tough to see if a line is coming out of the screen or is just a short line in another plane. An excellent tool to help you visualize what is happening in a 3D sketch is the Four Viewport view. This divides the screen into four quadrants, displaying the front, top, and right views in addition to the trimetric or isometric view. You can sketch or edit in any of the viewports, and the sketch will update live in all the viewports simultaneously. This arrangement is shown in Figure 6.20. You can easily access the divided viewport screen by using buttons on the Standard Views toolbar. You can also manually split the screen by using the splitter bars at the lower-left and upper-right ends of the scroll bar areas around the graphics window. These window elements are also described in Chapter 2, “Navigating the SolidWorks Interface.”

When unconstrained entities in a 3D sketch are moved, they move in the plane of the screen. This can lead to unexpected results when viewing something at an angle, moving it, and then rotating the view, which shows that it has shot off into deep interplanetary space. This is another reason to use the Four Viewport view, which enables you to see what is going on from all points of view at once.

Exploring Sketch Relations in 3D Sketches

Sketch relations in 3D sketches are not exactly the same as in 2D sketches. Relations are not projected into a plane in a 3D sketch the way they are in 2D. For example, an entity in a 2D sketch can be made coincident to an entity that is out of plane. This is because, to make the relation, the out-of-plane entity is projected into the sketch plane, and the relation is made to the projection. In a 3D sketch, coincident means coincident, with no projection.

Several relations are available in 3D sketches that are not found in 2D sketches, such as AlongX, AlongY, AlongZ, and OnSurface.

As a general caution, keep in mind that solving sketches in 3D is more difficult than it is in 2D. You will see more situations where sketch relations fail or they flip in the wrong direction. Angle dimensions in particular are notorious in 3D sketches for flipping direction if they change and go across the 180-degree mark. When possible, it is advisable to work with fully defined sketches and to be careful (and conservative) with sketch relations.

Using Planes in Space

It is possible to create planes directly in 3D sketches. These planes work like regular planes initially. Having planes in the sketch also enables planar sketch entities such as arcs and circles in 3D sketches. Sketches can be created on these planes, and the sketch will move with the plane, but the plane will also move with the sketch. Planes within 3D sketches can be confusing if you expect them to work like 2D sketches and planes.

Figure 6.21 shows the PropertyManager interface for creating 3D planes.

The confusing part is this: Say you create a vertical line on a plane in a 3D sketch. You can then angle the line, and the plane will rotate with it. There is no way to rotate the plane on its own unless you have some sketch geometry on the plane and cause that to rotate.

To open a sketch on a plane in a 3D sketch, double-click on the sketch or use the 3D Sketch on Plane tool. The plane is activated when it displays a grid. You can double-click an empty space to return to regular 3D Sketch mode. The main thing you give up with abandoning 3D sketch planes is the simplification of certain sketch entities such as arcs and relations.

The advantage of using planes within a 3D sketch is that you abandon the parent/child concept that you would otherwise embrace if you used a series of 2D sketches and 2D planes. In my opinion, 3D sketches are an incredibly useful tool; however, the 3D planes concept is not very well developed. I'm not ready to say it's dangerous, but it certainly is not fully thought out.

Using Planar Path Segments

Some path segments that are allowed in 3D sketches can be used only if they are sketched on a plane. These entities include circles and arcs and can include splines, although splines are not required to be on a plane. I've already mentioned that to sketch on a 3D plane (a plane created within the 3D sketch), you can simply double-click the plane.

To sketch on a standard plane or reference geometry plane, you can double-click the plane or Ctrl+click the border of the plane with the Sketch Entity icon active. The space handle moves, indicating that newly created sketch entities will lie in the selected plane.

Defining Dimensions

Dimensions in 2D sketches can represent the distance between two points, or they can represent the horizontal or vertical distance between objects. In 3D sketches, dimensions between points are always the straight-line distance. If you want to get a dimension that is horizontal or vertical, you should create the dimension between a plane and a point (the dimension is always measured normal to the plane) or between a line and a point (the dimension is always measured perpendicular to the line). For this reason, reference sketch geometry is often used freely in 3D sketches, in part to support dimensioning.

Using 3D Sketch Summary

Three-dimensional sketches are extremely powerful for many different applications. The problem is that they are also limited in some of their capabilities, and they do not work exactly like 2D sketches. You will benefit from knowing how to use 3D sketches at some point, even if it isn't every day.