IN THIS CHAPTER
Distinguishing sketch entities
Creating relationships in sketches
Examining sketch settings
Using sketch blocks in parts, assemblies, and drawings
Using reference geometry
Learning to use sketch relations tutorial
Using blocks and belts tutorial
Referencing geometry tutorial
The workflow for most SolidWorks features goes like this:
So the first step to leaning how to create models in SolidWorks is to learn how to sketch. If you are coming from another parametric 3D modeler, many of your skills will be transferable to SolidWorks. If you are coming from a 2D application, sketching is just like drawing except that you do it in smaller chunks and on planes in 3D space. If you have never used CAD before, think of the sketch-feature relationship as creating a simplified 2D drawing that represents a portion of the part that you can make with some sort of process such as extruding the shape in the 2D drawing, or revolving it.
So far, in this book, you have looked mainly at concepts, settings, and setup, which is necessary but mundane business. In this chapter, you begin to learn how to control parametric relationships in sketches. Then in later chapters, you begin to build models, simple at first, but gaining in complexity and always demonstrating new techniques and features that build your modeling vocabulary. Beyond this, you use the parts to create drawings.
This chapter deals entirely with sketches in parts. However, you will be able to apply many of the topics I cover here to assemblies. Some related topics, such as layout sketches, have functionality that is exclusive to assemblies, and these topics are covered in the assemblies' book, SolidWorks 2011 Assemblies Bible (Wiley, 2011).
When you open a sketch, several tools become available, specifically all the sketch entities and tools. Conversely, you cannot do several things until you open a sketch. For example, you cannot apply a Fillet feature while a sketch is open. Open sketches and selection filters are two very common sources of frustration for new users. Several indicators exist to let you know when you are in Sketch mode:
While most users find the sketch grid annoying or distracting, when teaching, I've always used the grid to remind students when they are in Sketch mode. If you forget or would like a visual cue, the sketch grid is a useful option.
Sketches must be either open or closed, and you can only have one sketch open at a time. SolidWorks uses many indicators to show the state of a sketch, including the Confirmation Corner and the Task Bar.
Several methods exist to open new sketches in SolidWorks:
You can open existing sketches several ways:
The first step in creating most SolidWorks parts is a sketch. This will usually be a 2D sketch, although you can also use 3D sketches. A 2D sketch is simply a collection of 2D lines, arcs, and other elements that lie together on a plane; it usually also contains relations and/or dimensions between the entities so that the sketch can automatically adjust to changes because each sketch entity understands its function.
SolidWorks sketch entities include many types, some of which you will use all the time, and some of which you may not use, even if you spend years working with the software. Next, I identify each entity type. This enables you to see it at least once and know that it is available if you need it at some point.
In the following section, I first identify the default buttons on the Sketch toolbar, followed by the rest of the entities that you can access by choosing Tools Customize Commands Sketch.
The Sketch tool opens and closes sketches. You may notice that the name of the button changes depending on if the sketch is open or closed. If you preselect a plane or planar face and then click the Sketch button, SolidWorks opens a new sketch on the plane or face. If you preselect a sketch before clicking the Sketch button, SolidWorks opens this sketch. If you preselect an edge or curve feature before clicking the Sketch button, SolidWorks automatically makes a plane perpendicular to the nearest end of the curve from the location you picked. If you do not use preselection, and only click the Sketch tool with nothing selected, SolidWorks prompts you to select a plane or planar face on which you want to put a new sketch, or an existing sketch to edit.
The 3D Sketch tool opens and closes 3D sketches with no preselection required. 3D sketch is covered in more detail in Chapter 31.
The Smart Dimension tool can create all types of dimensions used in SolidWorks, such as horizontal, vertical, aligned, radial, diameter, angle, and arc length. You can create dimensions several ways, as shown in Figure 3.1:
Selecting the line is the easiest and fastest method. Selecting parallel lines on the ends is not recommended because if you delete either of the selected lines, the dimension is also deleted; however, sometimes this method is necessary.
You can use the first and second techniques for the angled line shown in Figure 3.1 to create any of the three dimensions shown. To accomplish this task, drag the cursor while placing the dimension until the witness lines snap to the orientation you want.
Tip
To lock the orientation of a dimension while moving the cursor to place the actual dimension value, click the RMB. To unlock it, click the RMB again. The RMB cursor appears as a lock when the functionality is unavailable and an unlock icon when it is.
The third technique locks you into the horizontal orientation because of the orientation of the selected lines.
Note
In some situations, you may run into lines that appear to be parallel but are not exactly so. This will result in an angle dimension instead of a linear dimension. Here, you can select one of the lines and one endpoint. SolidWorks requires parallelism be precise, and situations where lines aren't exactly parallel happen if the angular measurement is off in the second or third decimal place, measuring in degrees. Imported 2D drawings and reverse-engineered 3D models can be particularly susceptible to this type of error.
Caution
When you select lines to establish a dimension instead of endpoints, both of the lines gain an implied parallel relation that prevents them from moving as you might predict. In the example shown in Figure 3.1, neither of the end lines can be angled unless you remove the dimension.
Another issue with adding dimensions to lines is that if you delete either line, the dimension is also deleted. This is not true for the first and second techniques, where as long as the endpoints remain, the dimension remains.
You can change Smart Dimension values several ways. The most direct way is to simply key in a value such as 4.052. The software assumes document units unless you key in something specific. You could also key in an expression, even with mixed units, such as 8.5 mm/2+.125 or 25.4+.625 in. You can also key in negative dimensions, which function the same as the Change Sense button in the Modify box.
Another way to put a value into the Modify box is to click the down arrow to the right of the value field, and select either to use an equation to calculate a value or a Link Value. A Link Value is like a variable name to which you can assign a value. You can link multiple dimension values to that Link Value. In sheet metal parts, the default Link Value of Thickness is used; if you change the thickness in one feature, it changes for all the sheet metal features.
To the right of the drop-down arrow is a pair of up and down “spin” arrows that enable you to change the value in the Modify box by a set increment amount. You set the increment in Tools Options System Options Spin Box Increments. You can also store multiple increment values within the Increment Value icon on the Modify box.
The final way to change the value in the Modify box is by using the wheel underneath the value field. The wheel uses the default increment value. Pressing Ctrl while using the wheel multiplies the increment by ten, and pressing Alt while using the wheel divides the increment by ten.
Here is a look at the Dimension Properties interface.
Note
Along with the Radial and Diameter dimensions, you may also want to dimension between arcs or circles, from tangent or nearest points. To do this, press the Shift key and select the Smart Dimension tool to select the arcs near the tangent points. Alternatively, to change a dimension from a center-to-center dimension to a max-to-max dimension, you can drag dimension attachment points to tangent points or use the dimension properties.
The Line creates straight lines using one of two methods:
Note
The click+click and click and drag methods have been treated equivalently by SolidWorks until recent releases. Some new functions like Enable on-screen numeric input seem to function better with click+click than click and drag.
Alternate methods for drawing lines include horizontal, vertical, angle, and infinite lines. The interface for these options appears in the PropertyManager, as shown in Figure 3.4.
Note
The Add Dimensions option exists in several sketch entity PropertyManagers and adds Smart Dimensions to newly sketched entities. The option only appears in the sketch entity PropertyManager if the setting at Tools Options Sketch Enable on-screen numeric input on entity creation is selected.
The on-screen numeric input is not the same as the Input Dimension Value function, and, in fact, it overrides that option. You cannot input dimension values when using the Add Dimensions in conjunction with click and drag sketching. It appears to be intended for click+click sketching only, so that you can enter values between clicks.
The Corner Rectangle creates a rectangle by clicking one corner and dragging to the diagonal corner. This action creates four lines with Horizontal and Vertical sketch relations, as appropriate. The Corner Rectangle is also available as a flyout icon with a Corner Rectangle, Center Rectangle, 3 Point Corner Rectangle (rectangle at an angle), and 3 Point Center Rectangle, as well as a Parallelogram. Figure 3.5 shows the flyout and flyout icons, and the PropertyManager for the Rectangle, which also enables you to switch types of rectangle easily.
Notice the Add dimensions check box in the PropertyManager. Selecting this box while creating a rectangle causes the software to add dimensions aligned with the sides of the rectangle. This option is also available for lines, arcs, and circles.
Note that if you use this option in conjunction with the Enable on-screen numeric input on entity creation setting, found at Tools Options Sketch, it makes creating sketch entities to the correct size immediately much easier.
The Circle creates a circle using one of two methods, which are available from either the flyout icon or the Circle PropertyManager:
The Centerpoint Arc creates an arc by clicking the center, dragging the radius, and then clicking and dragging the included angle of the arc. The first two steps are exactly like the Center-Radius circle.
Tangent Arc tool creates an arc tangent to an existing sketch entity. Depending on how you move the cursor away from the end of the existing sketch entity, the arc can be tangent, reverse tangent, or perpendicular, as shown in Figure 3.7.
Another way to create a tangent arc (called auto-transitioning) is to start drawing a line from the end of another sketch entity, and while holding the left mouse button, press the A key; or return the cursor to the starting point and drag it out again. This second method can be difficult to master, but it saves time compared to any of the techniques for switching sketch tools.
The 3 Point Arc creates an arc by first establishing endpoints, and then establishing the included arc, as shown in Figure 3.8. Again, this tool also works using the click+click or click and drag methods.
The Sketch Fillet creates a sketch fillet in one of two ways. Either you can select the endpoint where the sketch entities intersect or you can select the entities themselves, selecting the portion of the entity that you want to keep. Figure 3.9 illustrates both techniques.
The Sketch Chamfer tool is on the same flyout as the Sketch Fillet by default. Sketch Chamfer does not have a list selection box the way that fillet does, and does not use a preview like the fillet.
Sketch Fillets
While the Sketch Fillet tool is easy to use and may align with your way of working in a 2D program, it is not considered best practice to use sketch fillets extensively. Some reasons for this include:
Fillet features are the preferred method for creating rounds and fillets. The same can be said for chamfers. Still, sometimes you need to use tangent arcs in sketches. You will have to decide which way works best for you.
The Centerline follows the same methods as regular lines and is called a construction line in some cases. Other construction entities, such as construction circles, are not available directly, but you can create them by selecting the For Construction option in the PropertyManager for any entity.
Spline draws a freeform curve. Splines may form either a single closed loop or an open loop. In either case, the spline is not allowed to cross itself. You can draw a spline by clicking each location where you want to add a control point. Figure 3.10 identifies the elements of a spline. The detail image shows the structure of a spline handle.
Splines are used mainly for freeform complex shapes in 2D and 3D sketches, although you can also use them for anything in which you would use other sketch elements. If you need more information on splines and complex shape modeling, refer to the SolidWorks Surfacing and Complex Shape Modeling Bible (Wiley, 2008).
The Point creates a sketch point. Aside from limited cases of lofting to a point or using a point as a constraint sketch in a Fill feature, sketch points are usually used for reference or for the location of the centerpoint of Hole Wizard features.
You can also use the sketch point as a virtual sharp. If two sketch entities do not actually intersect because of a fillet or chamfer, selecting the two entities and clicking the Point tool creates a point at the location where they would intersect if they were extended. This is useful for dimensioning to the sharp. Virtual sharp display is controlled by a Document Property setting.
The 3D Sketch Plane creates a plane in a 3D Sketch. I discuss 3D Sketches in more detail in Chapter 6. By sketching on planes within a 3D sketch, you get most of the benefits and usage of 2D sketches, and you do not have to deal with history between sketches. Before committing too much work to this course, you should look into some of the shortcomings of 3D Planes. The planes are treated just like any other entity in the 3D sketch, which means you can assign sketch relations to them, but it also means that they can move around within the sketch like sketch entities.
The Add Relation displays a PropertyManager window that enables you to apply sketch relations. This interface appears to be obsolete because it is easier to simply select sketch items and apply relations via the context toolbar or in the PropertyManager window that appears automatically when you select them; however, there are some subtle workflow-related reasons for using this tool.
Two advantages exist to using the Add Relations dialog box over simply selecting sketch entities and adding relations. When the Add Relation PropertyManager is active, you do not need to use the Ctrl key to select multiple entities. You also do not need to clear a selection before making a new selection for the next relation. These two reasons sound minor, but if you have a large number of sketch relations to apply, the workflow goes much more smoothly using this tool than the default method.
The Display/Delete Relations enables you to look through the relations in a sketch and sort them according to several categories. From this window, you can delete or suppress relations and replace entities in relations.
The Quick Snaps flyout enables you to quickly filter types of entities that sketch elements will snap to when you move or create them. To access the tools, click the drop-down arrow to the right of the toolbar button.
The Mirror Entities mirrors selected sketch entities about a single selected centerline and applies a Symmetric sketch relation. In addition, a Dynamic Mirror function is described later in this chapter.
Note
PropertyManagers for sketch tools such as Mirror, Convert Entities, Sketch Fillet, and Intersection Curve now include a selection box for the entities to be used in the operation. The Offset PropertyManager is one that is conspicuously missing this functionality.
The workflow for the sketch tools with the selection boxes generally feels interrupted, in comparison to the workflow in SolidWorks versions before the selection boxes existed. To overcome this problem, you can deselect the push pin, and on the next execution of the tool, preselect the entities that would go into the selection box and then click the toolbar icon.
The Convert Entities converts edges, curves, and sketch elements from other sketches into entities in the current sketch. When edges are not parallel to the sketch plane, the Convert Entities feature projects them into the sketch plane. Some elements may be impossible to convert, such as a helix, which would produce a projection that overlaps itself. Sketch entities created using Convert Entities get an On-Edge sketch relation.
The Offset Entities works like the Convert Entities feature, except that it offsets the sketch to one side or the other of the projection of the original edge, sketch, or curve. Figure 3.11 shows the interface for this command.
The options available in the Offset Entities interface are as follows:
Caution
The Offset Entities command may fail if the offset distance is greater than the smallest radius of curvature, and you are attempting to offset to the inside of the arc.
In addition to the bidirectional offset with capped ends, SolidWorks also has slot sketch entities for straight and curved slots, which are covered later in this chapter. Composite slots (made of a combination of straight and curved sections) still require the offset method.
The Trim is actually several functions rolled into one, and it is an extremely powerful tool for editing sketches. Trim Entities allows several methods for trimming, as well as extending and deleting sketch entities. Figure 3.13 shows the PropertyManager interface for this function.
You can also use power trim to extend sketch entities along their paths by dragging the endpoints. Regular dragging can also change the position or orientation of the rest of the entity, but by using the Power trim feature you affect only the length.
In all cases, the selected section of the entity is removed. The Trim to closest option can also extend when you drag one entity to another; if an intersection is possible, the first entity is extended to the second entity. Figure 3.17 illustrates how the Trim to closest option functions.
The Construction Geometry toggles between regular sketch entities and construction entities. Construction sketch entities are not used to create solid or surface faces directly; they are only used for reference — for example, revolve centerlines, extrude and pattern directions, and so forth. Be careful with the icon for this function, because it looks almost identical to the No Solve Move icon, especially as printed here in gray scale.
Note
The icons for Hide/Show Edges, No Solve Move, and Construction Geometry look substantially similar, and in this black and white book they may be indistinguishable.
The Stretch sketch tool is intended for use in sketches where there are enough dimensions to make a particular change difficult by changing dimensions only. It is similar in purpose and use to the AutoCAD Stretch function because it was loosely modeled after the AutoCAD functionality. Stretch enables you to specify a change that will change several dimensions simultaneously. Figure 3.18 shows the initial, intermediate, and final states of the sketch being stretched.
Tip
The main ideas to remember with the Stretch tool are that it is used to stretch dimensioned lines, and that you need to select the lines that will lengthen or shorten as well as the lines that will move. Because of this, selecting entities for Stretch is best done with the right-to-left window selection, which also selects any items that the selection box crosses. (Left-to-right window selection only selects items that are completely within the selection box.)
Caution
Figure 3.18 shows the X/Y option being used, but if you use the From/To option, be aware that it may unexpectedly delete some sketch relations.
The Move, Rotate, Copy, and Scale sketch tools operate on selections within a sketch. You can use these tools with pre- or post-selection methods. These tools delete existing sketch relations when necessary to accomplish the task. For example, if you want to move a rectangle connected to the origin, the Move tool will delete the Coincident relation between the sketch endpoint and the origin. If you want to rotate a rectangle, the Rotate tool will delete all the horizontal and vertical relations on the entities being rotated. This operation may result in a completely underdefined sketch. SolidWorks does not warn you that sketch relations are being deleted.
If you use the Scale tool on a fully defined sketch, SolidWorks will scale the position of the selected entities, deleting sketch relations if necessary to do so, but no dimensions will be scaled or deleted.
Caution
Be careful when using these sketch tools. They can delete sketch relations without warning.
These sketch tools were originally put in the software to avoid some of the complexities and limitations of the Modify Sketch tool, which can also move, copy, rotate, and scale sketches. Figure 3.19 shows the simple interface for the Move Entities command. Select the entities to move in the upper box and the method to move them below.
Select is usually used to turn off the previous command and return the cursor to its default state.
Grid/Snap is used to open the Grid/Snap section of Tools Options Document Properties.
Parallelogram is used to draw a parallelogram (adjacent sides are not perpendicular, and opposite sides are parallel). Click one corner of the parallelogram, then click the second and third corners. Works like the 3 Point Rectangle except that adjacent sides are not perpendicular.
Polygon creates a regular n-sided polygon in the same way as a circle. Click the center and drag the radius. You need to set the number of sides in the PropertyManager before clicking in the graphics window.
Ellipse is created by clicking the center, dragging one axis, and then dragging the other axis.
Partial Ellipse is created by clicking the center, dragging one axis, dragging the other axis, and then clicking and dragging the included angle of the partial ellipse. The Partial Ellipse feature works like the Centerpoint Arc command.
Parabola is created by clicking the location for the Focus, and then dragging the position of the Apex. You then click and drag the included angle of the parabola, as shown in Figure 3.20. This is a rarely used sketch entity and is often difficult to control with sketch relations or dimensions.
Spline on Surface is used in 3D sketches to draw a freeform spline on any 3D surface. The Spline on Surface feature can cross face boundaries as long as the faces are at least tangent (ideally curvature continuous) across the edge. Spline on Surface can be used to trim surfaces or create split lines.
Sketch Text creates editable text in sketches using TrueType fonts installed in your Fonts folder. Some fonts produce sketches that are unusable for solid features, due to violating sketch rules with overlapping or zero thickness. You need to be careful which fonts you select, but I have had success with a wide variety of fonts I have found on the Internet. Sketch Text may be dissolved into lines and arcs so that you can edit them manually. Dissolve is available on the RMB menu. Figure 3.21 points out the key elements of the Sketch Text interface.
Note
Note that the Link To Property icon enables you to link sketch text to a custom property, or a configuration specific custom property. Using configurations and properties to drive sketch text can be a valuable function.
Intersection Curve, in 2D sketches, creates sketch entities where the sketch plane intersects selected faces. In 3D sketches, the Intersection Curve sketch tool creates sketch entities where any types of selected faces intersect. This can be an extremely useful tool in many situations.
Face Curves applies the underlying U-V isoparameter mesh to a selected face. It is most commonly used as an evaluation tool for complex surfaces, but you can also use it to create curves to rebuild faces. Accepting the results by clicking OK creates a separate 3D sketch for each spline. Figure 3.22 shows the original surface and the results of using face curves on a complex lofted surface.
Extend extends a sketch entity up to its next intersection with another sketch entity. This is not to be confused with the Extend for surface entities.
Split Entities splits a sketch entity into two segments. You can also delete it later to rejoin the entity back into a single segment. Closed loop entities require at least two split points.
Dynamic Mirror can be used when you pre-select a centerline and Dynamic Mirror is turned on. Any new sketch entity that you draw is automatically mirrored to the other side of the centerline. The ends of the mirror line have hatch marks on them to remind you that you have mirroring turned on.
Linear Pattern creates a one- or two-directional pattern of sketch entities. You can define spacing and angles. Figure 3.23 shows the interface and the results of this function.
Circular Sketch Pattern creates a circular pattern of sketch entities.
You should use sketch patterns as little as possible. For many of the same reasons that fillet features are preferred over sketch fillets, pattern features are preferred over sketch patterns. Sketch patterns are not as editable or as flexible as feature patterns. They solve slowly, especially when you pattern many entities. Best practice is to avoid sketch patterns unless there is no alternative.
Make Path is intended to help create machine-design motion in sketches, in particular, cam type motion. Although it is helpful, you do not need to make a block of the cam first. You can then right-click the block and select Make Path. A tangent relation to a path enables a follower to roll around the entire perimeter.
Modify Sketch is one of my favorite sketch tools, but it has been falling out of favor in more recent versions of SolidWorks because of the improvements to tools such as Move Sketch. It is also one of few remaining dialog box interfaces in the software. The Modify Sketch tool is flexible and powerful, and enables you to move, rotate, and scale the sketch, as well as mirror about a horizontal or vertical axis or about both axes simultaneously. Figure 3.24 shows the interface, which consists of a dialog box, a special Origin-like symbol, and a context-sensitive cursor.
Both the left and right mouse buttons have special functions, which change when the cursor is moved over the three knots on the special Modify Sketch Origin. The RMB enables you to mirror or rotate the sketch, and the left mouse button (LMB) enables you to move the Origin or move the sketch.
This function has some limitations when you use it with sketches that have external relations. Certain functions may be disabled or a warning message may appear, saying that you need to remove external relations to get a particular function to work correctly.
No Solve Move enables the moving of sketch entities without solving any relations in the sketch. If you select this option and you move an entity with relations that would otherwise not allow it to move (such as a collinear relation), you are prompted with a choice to delete the existing relation and continue or copy the entity without the relation. As mentioned earlier, be careful with the icon for this function because it looks almost identical to the Construction Geometry icon, especially as printed here in gray scale.
Sketch Picture is a picture that is placed in the sketch, lies on the sketch plane, and is listed in the FeatureManager indented under the sketch. The Sketch Picture may be suppressed independently from the rest of the sketch, and when the sketch is hidden the picture is not visible. You can easily move, resize, and rotate Sketch Pictures, as well as apply a transparent background color to them. Sketch Pictures are usually used for tracing over or as a planar decal without the need for PhotoWorks. Figure 3.25 shows the controls for manipulating the Sketch Picture feature.
Equation Driven Curve is a sketch spline driven by either an explicit or parametric equation, as shown in Figure 3.26. An explicit equation is in the form y = f(x), while a parametric equation uses multiple equations driven by a common parameter value of the form, such as
x = cos(t)
y = sin(t)
0>t>pi
where t is a number in radians.
The result is a proportional spline in a sketch, not a curve feature as the name suggests. The capability exists to drag the spline itself, or its endpoints, in 2D or 3D and SolidWorks calculates the new transformation. To reposition a sketch, use sketch relations and dimensions.
If you start an Equation Driven Curve in a 2D sketch, you get the form for a 2D curve equation. If you start in a 3D sketch, you get the form for a 3D curve. Once these splines are created, you cannot remove the relation to the equation and manually edit the spline; they are tied to the equation until you delete the entire spline.
One way to get around this limitation would be to create an equation-driven curve in one sketch, and then open another sketch and use convert entities to copy the spline, delete the On Edge relation, and use Simplify Spline to add control points to it. This is a technique commonly used with other types of curves; it does not enable you to update the overall size or shape of the spline through the equation, but you can manually adjust sections of a curve originally created from equations. Examples of where this might be useful would be a lead in or lead out on a cut thread, a special attachment loop in the middle of a spring, or a flare around the edge of a lens or reflector dish for mounting.
Straight Slotand Curved Slot draw slots of a given width and length with full rounds on the ends. All the slot sketch entities can be seen in the PropertyManager shown in Figure 3.27. If you need to draw a composite slot or a slot with multiple entities, you will need to use the bi-directional sketch offset with capped ends mentioned earlier.
The Dimensions/Relations toolbar has a few tools that you have already seen, but as the name suggests, it also contains tools that will either help you to create or investigate dimensions and sketch relations. Figure 3.28 shows the default toolbar, but in the following pages, you look at all the available tools you can see at Tools Customize Commands Dimensions/Relations.
If a line is not selected as the zero reference entity, the Ordinate Dimension feature defaults to a Horizontal Ordinate.
You can remove Ordinate Dimensions from the common alignment by right-clicking the dimension and selecting Break Alignment. Ordinate Dimensions will jog automatically if SolidWorks senses that the dimensions are getting too close to one another. You can also jog them manually. After you create the Ordinate Dimension set, you can add to it by accessing the Add to Ordinate command through the RMB menu. All the options for Ordinate Dimensions are shown in Figure 3.30.
Not all the listed options are available in the model sketch environment; some are available only in drawings.
Horizontal and Vertical Ordinate Dimensions have the same function as the regular Ordinate Dimensions, except that they only drive horizontal and vertical dimensions, respectively.
Chamfer Dimension is another type of dimension that is only driven and only applied in drawing documents. It works by first selecting the chamfered edge and then selecting the angle reference edge. It produces dimensions like the one shown in Figure 3.31.
Automatic Relations toggles to enable or disable the automatic creation of sketch relations while sketching. This toggle is also available through Tools Sketch Settings Automatic Relations. Automatic relations help you to create intelligent sketches with less manual intervention. Although using them takes a little practice, it is well worth the effort.
Caution
As with any automatic function, there are times when automatic relations will do things that you do not expect or want. While you are sketching, it is recommended that you watch the cursor and the relations that it automatically applies.
While sketching, symbols appear on the cursor to show that a relation will automatically be created. These symbols have a yellow background and will apply horizontal, vertical, coincident, tangent, parallel, and perpendicular relations. Figure 3.32 shows two situations where automatic relations are applied — a horizontal and a tangent relation.
Although SolidWorks users (even experienced ones) often confuse Inferencing and Automatic Relations, these functions are not the same. Inferencing refers to the blue dotted lines that display in Sketch mode when the cursor aligns with endpoints, centerpoints, or the Origin. Inferencing does not create sketch relations, with one exception. If both ends of a line pick up the same inference to the same point, SolidWorks will add that inference as an automatic relation.
When the cursor displays a small sketch relation symbol with a yellow background, this means that an automatic relation is going to be applied. If the relation symbol has a white background, the relation is inferenced but not applied as an actual sketch relation. The symbols with the blue (the color may also be green in SolidWorks 2008 or later) background are relations that have been applied to existing sketch entities. The symbols look the same, regardless of background color. Be aware that differences in versions and differences in color schemes can cause these colors to be different on your system.
Table 3.1 shows the symbols for the various inferences, automatic relation cursors, and applied sketch relations. The difference between the three types is simply the background colors: white, yellow, and blue, respectively.
The Fully Define Sketch interface uses sketch relations and dimensions to fully define the active sketch. It enables you to select which types of sketch relations and dimensions will be used to do this. Figure 3.33 shows the Fully Define Sketch interface. Be careful of this icon because it looks almost identical to the Sketch icon.
If you are familiar with older versions, the Fully Define Sketch function was formerly called Auto Dimension and has absorbed the functionality of Scan Equal and Add Relations. This function is very useful when used with imported sketch data. If you do not like the automatic dimensioning scheme, you can at least take advantage of the automatic sketch relations.
Best Practice
The Fully Define Sketch function does not necessarily use the best dimensioning practice for manufacturing drawings or for Design Intent. This tool is best used in situations when baseline and ordinate dimensions are appropriate.
In addition to sketch tools, another important aspect of controlling sketches is sketch settings. Sketch settings are found in two different locations. The first location is at Tools Options Sketch. In this chapter, I cover the settings found at the second location, Tools Sketch Settings. These settings mainly affect sketch relations.
If you import a large drawing from the DXF or DWG format, these drawings import as sketch entities into either a SolidWorks sketch or a drawing. SolidWorks may automatically turn off the Automatic Solve setting for performance (speed) reasons on files of this type.
It is recommended that you leave Detach Segment on Drag off. Turn it on only when you need it, and then immediately turn it off again. This setting can be hazardous for everyday use, because it enables you to simply drag sketch elements that may be otherwise fully defined.
Note
Combining Override Dims on Drag with Instant3D can be very handy for concept work, enabling you to drag sketches, model faces, and edges easily.
Sketch blocks are collections of sketch entities that can be treated as a single entity and can be reused within a single document or shared between documents. You can use sketch blocks in parts, assemblies, and drawings. To create a sketch block, select a group of sketch entities and click the Make Block button on the Blocks toolbar, or select Tools Blocks Make. Pre-selection is not necessary; you can also select the entities after you invoke the command.
Blocks may be internal to a particular document, or they may be saved as an external file. The externally saved block may be linked to each document where it is used, so that if the block is changed, it updates in the documents where it is used.
You can use blocks in conjunction with the Make Path function mentioned earlier in this chapter to create functional layouts for mechanisms. You can also use blocks in an assembly to build parts in-context. Refer to the SolidWork 2011 Assemblies Bible (Wiley, 2011) for a more in-depth examination of the assemblies aspects of blocks in SolidWorks.
The following is a description of the various tools that are available on the Blocks toolbar:
Reference geometry in SolidWorks is used to help establish locations for geometry that you can't physically touch, such as planes, axes, coordinate systems, and points. You often use reference geometry to establish a characteristic of the finished solid model before the model is created or to include an item that you may want to mate another part to in an assembly later. Mate References are also classified as Reference Geometry.
The importance of working with reference geometry becomes obvious in situations where you need to create geometry that doesn't line up with the standard planes. You might use planes to represent faces and axes to represent the centers of holes. Axes are often used to establish a direction, such as in plastic parts where, because of draft, you never truly have any vertical edges; an axis is frequently used to establish the direction of pull for the mold.
Coordinate systems come in handy, especially when translating a part from one system to another for the purpose of machining or some type of analysis. SolidWorks users usually model in such a way that the modeling work is made simpler by the choice of how the part origin is positioned relative to features of the part, but rapid prototyping, machining, mold building, and sheet metal manufacturing applications may have different requirements. As a part modeler, you cannot account for the needs of all downstream applications with your initial choice of origin placement, but you can always create a reference coordinate system for those downstream applications to use.
Planes are the most commonly used type of reference geometry because they are used for sketching, cutting, as extrude end conditions, and more. The Plane feature PropertyManager and its functionality have changed significantly in recent versions. With the new interface, shown in Figure 3.35, you start by selecting model items (faces, edges, points, vertices, or other sketch or reference geometry) that you want to use to create the plane. The new plane uses constraints like sketch relations from the selected references. For example, in Figure 3.35, the new plane is tangent to the selected First Reference cylindrical face and at an angle to the selected Second Reference of a plane.
The good news about this method is that there are far more options for creating planes than in the previous method, but the bad news is that the options are not all spelled out anywhere. You have to make a selection before it shows you the available constraints. The older interface presented the available options right up front, but there were fewer to choose from. Hopefully this interface matures in the future. Meanwhile, you may need to experiment to see what works best for the type of modeling you do.
For longtime users, when you start using the new Plane functionality, it may be best to try to ignore the new interface and simply make the same types of selections that you made in the past. The new Plane functionality will work perfectly that way. If you are a new user, just think of how you would like to specify the new plane, given the available geometry, and give it a try. The available options are not documented, so working with this interface requires some blind trust on the part of the user. The tool is quite powerful, but you will need to spend time experimenting with it. Even then, you will be unsure whether you are missing important options.
You can use axes to create pivot points in a part where you do not have any hole-type geometry for mating with other parts, or as a direction of pull for plastic parts or molds. Axes are frequently used to establish direction. Figure 3.36 shows that the first three features in a plastic part are axes established from the standard planes.
Consider using axes set up in this way as standard features in your template files. They can be effective in assemblies for moving parts in orthogonal directions and in parts for pattern or draft directions.
Note
The interface for the Axis feature has not been changed to match the Plane interface. Notice that the methods for creating an axis are spelled out clearly in the interface. I expect to eventually see a change to Axis to make it match the Plane interface.
Coordinate Systems in SolidWorks are primarily used for import and export, but can also be used for mating, mass properties, and other purposes. Coordinate Systems are usually located by a point to determine location or a set of edges to determine direction. Figure 3.37 shows the PropertyManager for assigning a coordinate system, along with the Export Options dialog box, which you can access from the Save As dialog box when the Files of Type drop-down is set to an export format.
To use the coordinate system when saving as a translated file type such as IGES or Parasolid, click the Options button, as shown in Figure 3.37; at the bottom of the Export Options dialog box, a selection box for Output coordinate system appears.
To use the coordinate system with mass properties, choose Tools Mass Properties from the menu, and then select the Output coordinate system, as shown in Figure 3.38.
The Point reference geometry feature is infrequently used; however, in some situations there is nothing else that does the job quite as well. This is not the same as a sketch point and does not require a sketch to be open; it is just a reference point that you can place in space. Figure 3.39 shows the PropertyManager for the Point reference geometry feature.
My favorite Point placement method is the Along Curve Distance option (the bottom one in Figure 3.39). It enables you to create several regularly spaced points along a curve.
Although, it is useful to read through the definitions and functions of all the sketch entities, tools, and relations, using your mouse to create is what this is all about. This tutorial makes sure that you get to know all the major functions in SolidWorks sketches. Almost every part that you build will start with a sketch, so this is a skill worth mastering. Follow these steps to learn about sketch relations:
On the DVD
The BibleInchTemplate.prtdot template used in this tutorial is in the Chapter 3 folder on the DVD.
Sometimes I am amazed at the things that can be done in SolidWorks, even with fairly simple tools. This is one of those times. If you design machines, this tutorial will have some extra meaning for you. If you do not design machines, Blocks and Belts are still valuable tools to have in your toolbox ready to use in various situations. Follow these steps to learn about using Blocks and Belts.
This tutorial steps you through creating reference geometry on an existing part in preparation for locating 3D features.
On the DVD
The Chapter 3 Reference Geometry.SLDPRT file (or drawing) used in this tutorial is in the Chapter 3 folder on the DVD.
When you are done, click the X at the right end of the FeatureManager filter to clear the result. Pressing Esc does the same thing.
The selection of the Cylindrical/Conical Face option should be automatically activated by your selection of the cylindrical face of the hole. Accept the result with the green check mark when the selections and settings are complete.
Note
If the view is already normal to the selected plane, and you double-click Normal To, the view switches to 180 degrees opposite. For this exercise, it doesn't matter which way you view the part, but from the top is better than from the bottom because the view is clearer.
You can tell if any relations have been applied if you go to the View menu and activate Sketch Relations. Make sure the centerpoint has a coincident relation and that none of the corners has any relations.
Note
The temporary axis is not on the same plane as the sketch plane, so if the view is not normal to the sketch plane, picking up an automatic relation between the centerpoint of the rectangle and the temporary axis will be difficult.
Best Practise
It is best practice to dimension or create sketch relations to items that have the fewest other relations. You should try to use the part origin and standard planes when possible. Dimensioning to reference geometry is better than dimensioning to model edges, although this is not always possible. Experienced users will immediately recognize the need for removing layers of references to prevent restrictive parent-child relations and broken or dangling relations. For beginning users, after you have some experience with making changes to models where relations have been applied carelessly, being more selective with sketch and dimension references will look more attractive to you.
You may have to adjust the direction of the extrude using the icon with the arrows just below the Direction1 heading in the Boss-Extrude PropertyManager.
Sketching in SolidWorks is something that you will do almost every time you open the software. A lot of automated functions are available that can enable you to do much of the work for you. You also have a lot of control to make changes manually. Remember that the best way to create most sketches is to use automatic relations when you can, sketch the approximate shape that you want to make, and then either drag it to pick up automatic relations, add dimensions, or add relations manually. Remember that you can use the left-click context toolbar to speed up adding relations manually.
The options for creating intelligent relationships that establish your Design Intent, as well as SolidWorks's capabilities in laying out mechanisms, is only limited by your imagination. The more familiar you become with the tools in your toolbox, the more of a craftsman you can become with this software.
Reference geometry is an essential part of creating and controlling relationships in any parametric model. Reference geometry is usually more stable than solid geometry, so sketch relations and dimensions should use reference geometry as references when possible.