SOLIDWORKS 2022 for Designers, 20th Edition

Chapter 2

Drawing Sketches for Solid Models

Learning Objectives

After completing this chapter, you will be able to:

• Understand the sketching environment

• Start a new document

• Set the document options

• Learn the sketcher terms

• Use various sketching tools

• Use the drawing display tools

• Delete sketched entities

THE SKETCHING ENVIRONMENT

Most of the products designed by using SolidWorks are a combination of sketched, placed, and derived features. The placed and derived features are created without drawing a sketch, but the sketched features require a sketch to be drawn first. Generally, the base feature of any design is a sketched feature and is created using the sketch. Therefore, while creating any design, the first and foremost requirement is to draw a sketch for the base feature. Once you have drawn the sketch, you can convert it into the base feature and then add the other sketched, placed, and derived features to complete the design. In this chapter, you will learn to create the sketch for the base feature using various sketching tools.

In general terms, a sketch is defined as the basic contour for a feature. For example, consider the solid model of a spanner shown in Figure 2-1.

Figure 2-1 Solid model of a spanner

This spanner consists of a base feature, cut feature, mirror feature (cut on the back face), fillets, and an extruded text feature. The base feature of this spanner is shown in Figure 2-2. It is created using a single sketch drawn on the Front Plane, refer to Figure 2-3. This sketch is drawn in the sketching environment using various sketching tools. Therefore, to draw the sketch of the base feature, you first need to invoke the sketching environment where you will draw the sketch.

 Figure 2-2 Base feature of the spanner

 Figure 2-3 Sketch for the base features of the spanner

Note

Once you are familiar with various options of SolidWorks, you can also use a derived feature or a derived part as the base feature.

The sketching environment of SolidWorks can be invoked anytime in the Part or Assembly mode. You just have to specify that you need to draw the sketch of a feature and then select the plane on which you need to draw the sketch.

STARTING A NEW SESSION OF SOLIDWORKS 2022

Double-click on the SolidWorks 2022 icon; the SolidWorks 2022 window will be displayed. If you are starting the SolidWorks application for the first time after installing it, the SolidWorks License Agreement dialog box will be displayed. Choose Accept from this dialog box; the SolidWorks interface window along with the Welcome - SOLIDWORKS dialog box will be displayed, as shown in Figure 2-4. Click anywhere in SOLIDWORKS 2022 window to collapse the Welcome - SOLIDWORKS dialog box.

 Figure 2-4 The SOLIDWORKS window

TASK PANES

In SolidWorks, the task panes are displayed on the right of the window. These task panes contain various options that are used to start a new file, open an existing file, browse the related links of SOLIDWORKS, and so on. Various task panes in SOLIDWORKS are shown in Figure 2-5 and are discussed next.

 Figure 2-5  Various Task Panes in SOLIDWORKS

SOLIDWORKS Resources Task Pane

SOLIDWORKS Resources task pane contains various rollouts that have options for accessing resources. It can be invoked by clicking on the  icon. The rollouts and options available in this task pane are discussed next.

Welcome to SolidWorks

This option is used to open the Welcome - SOLIDWORKS dialog box, refer to Figure 2-6. This dialog box provides a convenient way to open new and saved documents. It also provides access to various folders, SOLIDWORKS resources, and various technical news alerts related to SOLIDWORKS. It appears by default whenever you open a new session of SOLIDWORKS. However, if you select the Do not show on startup check box available at the bottom-left corner then from the next time it will not appear by default. There are four tabs available in this dialog box which are discussed next.

Figure 2-6 The Welcome - SOLIDWORKS dialog box

Home Tab

    The Home tab is chosen by default and the options under this tab are used to open new and existing documents. This tab also provides access to recent documents and folders. Various resources like updates in the current version, user groups for discussion, technical support can be accessed using this tab.

Recent Tab

   The Recent tab lists large number of recent documents and folders as compared to Home tab. You can also browse your saved files by using the Browse button available at the right in this tab.

Learn Tab

    The Learn tab provides various resources to learn more about SOLIDWORKS through PDF files and tutorials for practical approach.

Alerts Tab

    The Alert tab lists various news and alerts regarding SOLIDWORKS.

SolidWorks Tools Rollout

The options in this rollout are used for customizing the tab, diagnosing and troubleshooting SolidWorks, performing system maintenance, checking performance test, saving and restoring the customization settings of SolidWorks, and so on.

Online Resources Rollout

The options in this rollout are used to invoke the discussion forum of SolidWorks, partner solutions, and manufacturing network.

Subscription Services Rollout

The options in this rollout are used to get direct access to the Dassault Systemes partner products website. This partner products website will help you to interact with the design partners and designers for various technical supports and tips.

Design Library Task Pane

The Design Library task pane is invoked by choosing the Design Library tab from the window. This task pane is used to browse the default Design Library and the toolbox components, and also to access the 3D ContentCentral web site. Note that to access the 3D ContentCentral website, your computer needs to be connected to the Internet. To access the toolbox components, you need to install Toolbox add-in in your computer.

File Explorer Task Pane

The File Explorer task pane is invoked by choosing the File Explorer tab from the window. This task pane is used to explore the files and folders that are saved in the hard disk of your computer.

View Palette Task Pane

The View Palette task pane is invoked by choosing the View Palette tab from the window. This task pane is used to drag and drop the drawing views into a drawing sheet. This is available only when you are in the drafting environment.

Appearances, Scenes, and Decals Task Pane

The Appearances, Scenes, and Decals task pane is used to change the appearance of model or display area. On choosing the Appearances, Scenes, and Decals tab from the window, you will notice three nodes, Appearances(color), Scenes, and Decals in the Appearances, Scenes, and Decals task pane. The Appearances(color) node is used to change the appearance of model, the Scenes node is used to change the background of the graphics area, and the Decals node is used to apply decals to a model. To assign appearance to the model, expand the desired category node from the Appearances node. Next, select a sub-category; different appearances of the selected sub-category will be displayed at the bottom area of the window. Now, drag and drop the required appearance on the model in the graphics area by selecting and holding the left-mouse button; the Appearance Target palette will be displayed. Select the required button from this palette to apply the selected appearance. You can change the properties of the appearance added by using the corresponding appearance PropertyManager. You will learn about this PropertyManager in later chapters.

To change the background of the graphics area, expand the Scenes node from the Appearances, Scenes, and Decals task pane and select a category; the preview of different backgrounds available for the selected category will be displayed. Drag and drop the background in the graphics area; the background of the graphics area will be changed. You can also click the down-arrow next to the Apply Scene button in the View (Heads-Up) toolbar and select an option from this toolbar to change the background of the drawing area.

Similarly, to apply an image as a decal, expand the Decals node and select the logos subnode; the default logos will be displayed. Drag and drop the image on the model; the Decals PropertyManager will be displayed. Set the properties in this PropertyManager and choose the OK button.

Custom Properties Task Pane

The Custom Properties task pane is displayed on choosing the Custom Properties tab from the window. This task pane is used to view the properties of the files. If you do not have a property template for the files, then you can create it by choosing the Create now button from the Custom Properties task pane. On choosing this button, the Property Tab Builder 2022 window will be displayed. Set the properties in this window and save it. After saving the properties, you can view them in the Custom Properties task pane. To do so, choose Tools > Options from the SOLIDWORKS menus; the System Options - General dialog box will be displayed. Choose the File Locations option from this dialog box. The options related to the File Locations option will be displayed on the right of the dialog box. Select the Custom Property Files option from the Show folders for drop-down list. Next, browse the property template in the Folders area by choosing the Add button. Choose the OK button from the dialog box to exit. Now, you can view these properties in the Custom Properties task pane.

Tip

To expand the task pane at any stage of the design cycle, choose any one of the tabs provided on the task pane. Choose the Auto Show button to pin the task pane. To collapse the task pane, click anywhere in the drawing area when the Auto Show button is not chosen.

Note

In assemblies, you can assign properties to multiple parts at the same time.

STARTING A NEW DOCUMENT IN SOLIDWORKS 2022

To start a new document in SolidWorks 2022, select the Welcome to SOLIDWORKS option from the SolidWorks Resources task pane; the Welcome - SOLIDWORKS dialog box will be displayed, as shown in Figure 2-6. You can also invoke this dialog box by choosing the Welcome to SOLIDWORKS button from the Menu Bar. The options to start a new document using this dialog box are discussed next.

Part

The Part button is available in the New area of the Home tab in the Welcome - SOLIDWORKS dialog box. On choosing this button from the dialog box; the Part document will be invoked. In this mode, you can create solid models, surface models, or sheet metal components.

Assembly

Choose the Assembly button from the Welcome - SOLIDWORKS dialog box to start a new assembly document. In the assembly document, you can assemble the components created in the part documents. You can also create components or new layout in the assembly document.

Drawing

Choose the Drawing button from the Welcome - SOLIDWORKS dialog box to start a new drawing document. In a drawing document, you can generate or create the drawing views of the parts created in the part documents or the assemblies created in the assembly documents.

You can also start a new document using the New SolidWorks Document dialog box. To invoke this dialog box choose the New button from the Menu Bar, the New SolidWorks Document dialog box will be displayed, as shown in Figure 2-7. Choose the desired button and then the OK button to start a new document.

Figure 2-7 The New SOLIDWORKS Document dialog box

UNDERSTANDING THE SKETCHING ENVIRONMENT

Whenever you start a new part document, by default, you are in the part modeling environment. But you need to start the design by first creating the sketch of the base feature in the sketching environment. To invoke the sketching environment, choose the Sketch tab from the CommandManager. Next, choose the Sketch button from the Sketch CommandManager tab. For your convenience, you can add the Sketch button to the Menu Bar and invoke the sketching environment using this button. To do so, right-click on any toolbar and choose the Customize option from the shortcut menu; the Customize dialog box will be displayed. Choose the Commands tab and select the Sketch option from the Toolbars list box; all tools in the sketch categories will be displayed in the Buttons area. Press and hold the left mouse button on the Sketch button and then drag it to the Menu Bar. Click the OK button to exit the Customize dialog box. Figure 2-8 shows the Sketch button added to the Menu Bar.

Figure 2-8 SOLIDWORKS 2022 screen displaying the Sketch button in the Menu Bar

When you choose the Sketch button from the Menu Bar or invoke any tool from the Sketch CommandManager tab, the Edit Sketch PropertyManager is displayed on the left in the drawing area and you are prompted to select the plane on which the sketch will be created. Also, the three default planes (Front Plane, Right Plane, and Top Plane) are temporarily displayed on the screen, as shown in Figure 2-9.

Figure 2-9 The three default planes displayed on the screen

You can select a plane to draw the sketch of the base feature depending on the requirement of the design. As soon as you select a plane, the CommandManager will display various sketching tools to draw the sketch.

The default screen appearance of a SolidWorks part document in the sketching environment is shown in Figure 2-10.

Figure 2-10  Default screen display of a part document in the sketching environment

SETTING THE DOCUMENT OPTIONS

When you install SolidWorks on your computer, you will be prompted to specify the dimensioning standards and units for measuring distances. The settings specified at that time will become the default settings and will be applied on any new SolidWorks document opened thereafter. However, if you want to modify these settings for a particular document, you can do so easily by using the Document Properties dialog box. To invoke this dialog box, choose the Options button from the Menu Bar; the System Options - General dialog box will be displayed, as shown in Figure 2-11. Alternatively, choose Tools > Options from the SolidWorks menus to invoke the System Options - General dialog box. In this dialog box, choose the Document Properties tab; the name of this dialog box will change to the Document Properties - Drafting Standard dialog box. The procedure to set the options for the current document using this dialog box is discussed next.

Figure 2-11  The System Options - General dialog box

Modifying the Drafting Standards

To modify the Drafting standards, invoke the System Options - General dialog box and then choose the Document Properties tab. You will notice that the Drafting Standard option is selected by default in the area available on the left of the dialog box to display the drafting options.

The default drafting standard that was selected while installing SOLIDWORKS will be displayed in the drop-down list in the Overall drafting standard area. You can select the required drafting standard from this drop-down list. The standards available in this drop-down list are ANSI, ISO, DIN, JIS, BSI, GOST, and GB. You can select any one of these drafting standards for the current document.

Modifying the Linear and Angular Units

To modify the linear and angular units, invoke the System Options - General dialog box and then choose the Document Properties tab. In this tab, choose the Units option from the area available on the left in the dialog box to display the options related to the linear and angular units, refer to Figure 2-12. The default option that was selected for measuring the linear distances while installing SolidWorks will be available in the Length field under the Unit column. You can set the units for the current document from the options in the Unit system area. To specify the units other than the standard unit system in this area, select the Custom radio button; the options in the tabulation will be enabled. Select the cell corresponding to the Length and Unit parameter; a drop-down list will be displayed. Set the units from the drop-down list.

The units that can be selected for Length are angstroms, nanometers, microns, millimeters, centimeters, meters, microinches, mils, inches, feet, and feet & inches. To change the units for angular dimensions, select the cell corresponding to Angle and Unit; a drop-down list will be displayed. The angular units that can be selected from this drop-down list are degrees, deg/min, deg/min/sec, and radians. Set the number of decimal places in the corresponding field under the Decimals column.

Figure 2-12  Setting the dimensioning Standards

In SOLIDWORKS, you can also change the unit system for the current document by using the Unit system button that is located on the right in the status bar. To change the unit system using this option, click on the Unit system button; a flyout will be displayed with a tick mark next to the unit system of the activated document, refer to Figure 2-13. Now, you can select the required unit system for the activated document from this flyout. You can also invoke the Document Properties - Units dialog box by choosing the Edit Document Units option from this flyout.

Figure 2-13  Flyout displayed after choosing the unit system button

Modifying the Snap and Grid Settings

In the sketching environment of SolidWorks, you can make the cursor jump through a specified distance while creating the sketch. Therefore, if you draw a sketched entity, its length will change in the specified increment. For example, while drawing a line, if you make the cursor jump through a distance of 10 mm, the length of the line will be incremented by a distance of 10 mm. To modify the snap and grid settings, choose the Options button from the Menu Bar to display the System Options - General dialog box. To ensure that the cursor jumps through the specified distance, you need to activate the snap option. Select the Relations/Snaps sub-option of the Sketch option to display the related settings. From the options available on the right, select the Grid check box. Next, clear the Snap only when grid is displayed check box, if it is selected. If this check box is selected, then the cursor will snap the sketched entities only when the grid is displayed.

Next, choose the Go To Document Grid Settings button to invoke the Document Properties - Grid/Snap dialog box, refer to Figure 2-14. The distance through which the cursor jumps is dependent on the ratio between the values in the Major grid spacing and Minor-lines per major spinners available in the Grid area. For example, if you want the coordinates to increment by 10 mm, you will have to make the ratio of the major and minor lines to 10. This can be done by setting the value of the Major grid spacing spinner to 100 and that of the Minor-lines per major spinner to 10. Similarly, to make the cursor jump through a distance of 5 mm, set the value of the Major grid spacing spinner to 50 and that of the Minor-lines per major spinner to 10.

Note

Remember that these grid and snap settings will be applicable for the current documents only. When you open a new document, it will have the default settings that were defined while installing SolidWorks.

Figure 2-14  The Document Properties - Grid/Snap dialog box

Tip

If you want to display the grid in the sketching environment, select the Display grid check box from the Grid area of the Document Properties - Grid/Snap dialog box. Alternatively, choose Hide/Show Items > View Grid from the View (Heads-Up) toolbar.

While drawing a sketched entity by snapping through grips, the grips symbol will be displayed below the cursor on the right.

LEARNING SKETCHER TERMS

Before you learn about various sketching tools, it is important to understand some terms that are used in the sketching environment. These tools and terms are discussed next.

Origin

The origin is represented by a blue colored point displayed at the center of the sketching environment screen. By default, there are two arrows at the origin displaying the horizontal and vertical directions of the current sketching plane. The point of intersection of these two axes is the origin point and the coordinates of this point are 0,0. To display or hide the origin, choose Hide/Show Items > View Origins from the View (Heads-Up) toolbar.

Inferencing Lines

The inferencing lines are the temporary lines that are used to track a particular point on the screen. These lines are the dashed lines and are automatically displayed when you select a sketching tool in the sketching environment. These lines are created from the endpoints or the midpoint of a sketched entity or from the origin. For example, if you want to draw a line from the point where two imaginary lines intersect, you can use the inferencing lines to locate the point and then draw the line from that point. Figure 2-15 shows the use of inferencing lines to locate the point of intersection of two imaginary lines. Figure 2-16 shows the use of inferencing lines to locate the center of a circle. Notice that the inferencing lines are created from the endpoint of the line and from the origin.

Figure 2-15  Using inferencing lines to locate a point

Figure 2-16  Using inferencing lines to locate the center of a circle

Note

The inferencing lines that are displayed on the screen will be either blue or yellow. The blue inferencing lines indicate that the relations are not added to the sketched entity and the yellow inferencing lines indicate that the relations are added to the sketched entity. You will learn about various relations in the later chapters.

Inferencing lines will be displayed only when a sketching tool is active.

Tip

You can disable the inferencing line temporarily by pressing and holding the CTRL key.

Select Tool

SolidWorks menus: Tools > Select

The Select tool is used to select a sketched entity or exit any sketching tool that is active. You can select the sketched entities by selecting them one by one using the left mouse button. You can also hold the left mouse button and drag the cursor around the multiple sketched entities to define a box and select the multiple entities. There are two methods of selection, box selection and cross selection. You can also select multiple entities by pressing the SHIFT and CTRL keys. These selection methods are discussed next.

Selecting Entities Using the Box Selection

A box is a window that is created by pressing the left mouse button and dragging the cursor from left to right in the drawing area. The selection box will be displayed by continuous lines. When you create a box, the entities that lie completely inside it will be selected. The selected entities will be displayed in light blue and a pop-up toolbar will be displayed near the cursor.

Selecting Entities Using the Cross Selection

When you press the left mouse button and drag the cursor from right to left in the drawing area, a box of dashed lines is drawn. The entities that lie completely or partially inside this box or the entities that touch the dashed lines of the box will be selected. The selected entities will be displayed in light blue and a pop-up toolbar will be displayed near the cursor. This method of selection is known as cross selection.

Selecting Entities Using the Lasso Selection

Lasso selection is a freehand selection. To make a freehand selection, click-drag the mouse pointer; a continuous loop will be displayed. The entities that lie completely inside the loop will be selected and highlighted. Also, a pop-up toolbar will be displayed near the mouse pointer. Note that you need to change the default selection method for using lasso selection. To do so, choose Tools > Lasso Selection from the SolidWorks menus.

Selecting Entities Using the SHIFT and CTRL Keys

You can also use the SHIFT and CTRL keys to manage the selection procedure. To select multiple entities, press and hold the SHIFT key and select the entities. After selecting some entities, if you need to select more entities using the windows or cross selection, press and hold the SHIFT key. Now, create a window or a cross selection; all the entities that touch the crossing or are inside the window will be selected.

If you need to remove a particular entity from a group of selected entities, press the CTRL key and select the entity. You can also invert the current selection using the CTRL key. To do so, select the entities that you do not want to be included in the selection set. Next, press the CTRL key and create a window or a cross selection.

Note

1. When a sketching tool is active, you can invoke the select tool or press the ESC key to exit the sketching tool. You can also right-click and choose the select option from the shortcut menu to exit the tool.

2. In SolidWorks, when you select an entity, a pop-up toolbar will be displayed with options to edit the sketch. You will learn about these options in the later chapters.

Invert Selection Tool

SolidWorks menus: Tools > Invert Selection

Toolbar: Selection Filter > Invert Selection

The Invert Selection tool will be active only when an entity is selected and is used to invert the selection set. This tool is used to remove entities from the current selection set and select all other entities that are not in the current selection set. To invert the selection, select the entities that you do not want to be included in the final selection set and then choose Tools > Invert Selection from the SolidWorks menus. You can also invoke the Invert Selection tool from the shortcut menu. All entities that were not selected earlier will now be selected and the entities that were in the selection set earlier will now be removed from the selection set.

Now, you are familiar with the important sketching terms. Next, you will learn about the sketching tools available in SolidWorks.

DRAWING LINES

CommandManager: Sketch > Line flyout > Line

SolidWorks menus: Tools > Sketch Entities > Line

Toolbar: Sketch > Line flyout > Line

Lines are one of the basic sketching entities available in SolidWorks. In general terms, a line is defined as the shortest distance between two points. As mentioned earlier, SOLIDWORKS is a parametric solid modeling tool. This property allows you to draw a line of any length and at any angle so that it can be forced to the desired length and angle.

To draw a line in the sketching environment of SOLIDWORKS, invoke the Line tool from the Line flyout in the Sketch CommandManager; the Insert Line PropertyManager will be displayed, as shown in Figure 2-17. Alternatively, right-click in the drawing area; a shortcut menu will be displayed with tools and options. Choose the Line tool from the shortcut menu to display the Insert Line PropertyManager. You will notice that the cursor, which was an arrow, is replaced by the line cursor. You can also invoke the Line tool by pressing the L key.

The Message rollout of the Insert Line PropertyManager informs you to edit the settings of the next line or sketch a new line. The options in this PropertyManager can be used to set the orientation and other sketching options to draw a line. All these options are discussed next.

Figure 2-17  Partial view of the Insert Line PropertyManager

Orientation Rollout

The Orientation rollout is used to define the orientation of the line to be drawn. By default, the As sketched radio button is selected, so that you can draw the line in any orientation. If you need to draw only horizontal lines, select the Horizontal radio button. On selecting this radio button, the Parameters rollout will be displayed and you can specify the length of the line in the Length spinner provided in this rollout. You will learn more about dimensioning in the later chapters. After specifying the parameters, choose the start point and the endpoint in succession to create the horizontal line.

Similarly, to draw a vertical line, select the Vertical radio button, specify the parameters in the Parameters rollout, and then choose the start point and the endpoint in succession.

Note

If the value 0 is set in the Length spinner of the Parameters rollout, you can draw horizontal/vertical line of any length.

The Angle radio button is selected to draw lines at a specified angle. When you select this radio button, the Parameters rollout will be displayed, where you can set the values of the length of the line and the angle or the orientation of the line.

Options Rollout

Select the For construction check box available in this rollout to draw a construction line. You will learn more about construction lines later in this chapter. To draw a line of infinite length, select the Infinite length check box. Select the Midpoint line check box to draw a line by defining its midpoint and one of its endpoints.

On selecting the As sketched radio button in the Orientation rollout, you can draw lines by using two methods. The first method is to draw continuous lines and the second method is to draw individual lines. Both these methods are discussed next.

Drawing Continuous Lines

This is the default method of drawing lines. In this method, you have to specify the start point and the endpoint of the line using the left mouse button. As soon as you specify the start point of the line, the Line Properties PropertyManager will be displayed. The options in the Line Properties PropertyManager will not be activated at this stage.

After specifying the start point, move the cursor away from it and specify the endpoint of the line using the left mouse button. A line will be drawn between the two points. You will also notice that the line has filled squares at the two ends. The line will be displayed in light blue color because it is still selected.

Move the cursor away from the endpoint of the line and you will notice that another line is attached to the cursor. The start point of this line is the endpoint of the last line and the length of this line can be increased or decreased by moving the cursor. This line is called a rubber-band line as this line stretches like a rubber-band when you move the cursor. The point that you specify next on the screen will be taken as the endpoint of the new line and a line will be drawn such that the endpoint of the first line is taken as the start point of the new line and the point you specify is taken as the endpoint of the new line. Now, a new rubber-band line is displayed starting from the endpoint of the last line. This is a continuous process and you can draw a chain of as many continuous lines as needed by specifying the points on the screen using the left mouse button.

You can exit the process of drawing continuous line by pressing the ESC key, by double-clicking on the screen, or by invoking the Select tool from the Menu Bar. You can also right-click to display the shortcut menu and choose the End chain (double-click) or Select option to exit the Line tool.

Figure 2-18 shows a sketch drawn using continuous lines. You need to draw this sketch from the lower left corner and in this sketch, the horizontal line has to be drawn first. Draw the other lines and to close the loop, move the cursor attached to the last line close to the start point of the first line; you will notice that an orange colored circle will be displayed at the start point. If you specify the endpoint of the line at this stage, the loop will be closed and no rubber-band line will be displayed now. This is because the loop is already closed and you may not need another continuous line now. However, the Line tool is still active and you can draw other lines.

Figure 2-18 Sketch drawn using continuous lines

Note

When you terminate the process of drawing a line by double-clicking on the screen or by choosing End chain (double-click) from the shortcut menu, the current chain ends but the Line tool still remains active. As a result, you can draw other lines. However, to exit the Line tool, you can choose the Select option from the shortcut menu or press the ESC key.

Drawing Individual Lines

This is the second method of drawing lines. This method is used to draw individual lines in which the start point of the new line will not necessarily be the endpoint of the previous line. To draw individual lines, you need to press and hold the left mouse button to specify the start point, and then drag the cursor without releasing the mouse button. Once you have dragged the cursor to the endpoint, release the left mouse button; a line will be drawn between the two points.

To make the sketching process easy in SolidWorks, you are provided with the PropertyManager. The PropertyManager is a table that will be displayed on the left of the screen as soon as you select a sketched entity. The PropertyManager has all parameters related to the sketched entity such as the start point, endpoint, angle, length, and so on. You will notice that as you start dragging the mouse, the Line Properties PropertyManager is displayed on the left of the drawing area. All options in the Line Properties PropertyManager will be available when you release the left mouse button. Figure 2-19 shows partial view of the Line Properties PropertyManager.

Note

The Line Properties PropertyManager also displays additional options about relations. You will learn more about relations in the later chapters.

Figure 2-19  Partial view of the Line Properties PropertyManager

After you have drawn the line, modify the parameters in the Line Properties PropertyManager to create the line to the desired length and angle. You can also modify the line dynamically by selecting its endpoints and then dragging them.

Line Cursor Parameters

When you draw lines in the sketching environment of SOLIDWORKS, you will notice that a numeric value is displayed above the line cursor, refer to Figure 2-20. This numeric value indicates the length of the line you draw. This value is the same as the one displayed in the Length spinner of the Line Properties PropertyManager. The only difference is that in the Line Properties PropertyManager, the value will be displayed with more precision.

The other thing that you will notice while drawing horizontal or vertical line is that two symbols are displayed below the line cursor. These are the symbols of the Vertical and Horizontal relations.SOLIDWORKS applies these relations automatically to lines. These relations ensure that the lines you draw are vertical or horizontal. Figure 2-21 shows the symbol of the Vertical relation on a line andFigure 2-22 shows the symbol of the Horizontal relation on a line.

Figure 2-20 The length of the line displayed on the screen while drawing it

Note

In addition to the Horizontal and Vertical relations, you can apply a number of other relations such as Tangent, Concentric, Perpendicular, Parallel, and so on. You will learn about all these relations and other options in the Line Properties PropertyManager in the later chapters.

Figure 2-21 Symbol of the Vertical relation

Figure 2-22 Symbol of the Horizontal relation

Drawing Tangent or Normal Arcs Using the Line Tool

SolidWorks allows you to draw tangent or normal arcs originating from the endpoint of the line while drawing continuous lines. Note that these arcs can be drawn only if you have drawn at least one line, arc, or spline. To draw such arcs, draw a line by specifying the start point and the endpoint. Move the cursor away from the endpoint of the last line to display the rubber-band line. Now, when you move the cursor back to the endpoint of the last line, the arc mode will be invoked. The angle and the radius of the arc will be displayed above the arc cursor. You can also invoke the arc mode by right-clicking and choosing the Switch to arc (A) option from the shortcut menu or pressing the A key on the keyboard.

To draw a tangent arc, invoke the arc mode by moving the cursor back to the endpoint of the last line. Now, move the cursor through a small distance along the tangent direction of the line; a dotted line will be drawn. Next, move the cursor in the direction in which the arc should be drawn. You will notice that a tangent arc is drawn. Specify the endpoint of the tangent arc using the left mouse button. Figure 2-23 shows an arc tangent to an existing line.

To draw a normal arc, invoke the arc mode. Next, move the cursor through a small distance in the direction normal to the line and then move it in the direction of the endpoint of the arc; the normal arc will be drawn, as shown in Figure 2-24.

As soon as the endpoint of the tangent or the normal arc is defined, the line mode will be invoked again. You can continue drawing lines using the line mode or move the cursor back to the endpoint of the arc to invoke the arc mode.

Note

If the arc mode is invoked by mistake while drawing lines, you can cancel the arc mode and invoke the line mode again by pressing the A key. Alternatively, you can right-click and choose Switch to Line (A) from the shortcut menu or move the cursor back to the endpoint and press the left mouse button to invoke the line mode.

Figure 2-23 Drawing a tangent arc using the line tool

Figure 2-24 Drawing a normal arc using the line tool

Tip

You can flip the tangency of a tangent arc by right-clicking on the arc drawn and then selecting the Reverse Endpoint Tangent option from the short-cut menu displayed.

Drawing Construction Lines or Centerlines

CommandManager: Sketch > Line flyout > Centerline

SolidWorks menus: Tools > Sketch Entities > Centerline

Toolbar: Sketch > Line flyout > Centerline

The construction lines or the centerlines are the ones that are drawn only for the aid of sketching. These lines are not considered while converting the sketches into features. You can draw a construction line similar to the sketched line by using the Centerline tool. You will notice that when you draw a construction line, the For construction check box in the Options rollout of the Line Properties PropertyManager is selected. You can also draw a construction line using the Line tool. To do so, invoke the Insert Line PropertyManager by choosing the Line tool, select the For construction check box in the Options rollout, and draw the line.

Drawing Midpoint Line

CommandManager: Sketch > Line flyout > Midpoint Line

SOLIDWORKS menus: Tools > Sketch Entities > Midpoint Line

Toolbar: Sketch > Line flyout > Midpoint Line

The Midpoint Line tool is used to draw a line by specifying its midpoint and end point. To invoke this tool, choose the Midpoint Line tool from the Line flyout of the Sketch toolbar.

Drawing the Lines of Infinite Length

SolidWorks allows you to draw lines of infinite length. Note that these lines can be drawn only if the Line or Centerline tool is invoked. To draw lines of infinite length, invoke the Insert Line PropertyManager and then select the Infinite length check box available in the Options rollout of this PropertyManager. Next, specify two points in the drawing area; a line of infinite length will be drawn.

To convert a solid infinite length line to a construction infinite length line, you need to select the For construction check box in the Options rollout of the Line Properties PropertyManager. You can also set the angle value for infinite length lines in the Angle spinner available in the Parameters rollout of this PropertyManager.

Tip

When you select a line, a pop-up toolbar will be displayed. Choose the Construction Geometry button from this toolbar to convert the line into a construction line.

DRAWING CIRCLES

In SolidWorks, there are two methods to draw circles. In the first method, you can specify the center point of a circle and then defining its radius. In the second method, you can draw a circle by defining three points that lie on its periphery. The tools for drawing a circle are grouped together in the Circle flyout in the Sketch CommandManager. To draw a circle, select the down arrow on the Circle tool; a flyout with both the tools will be displayed. Invoke a tool from this flyout; the Circle PropertyManager will be displayed, as shown in Figure 2-25. Alternatively, right-click and then choose the Circle option from the shortcut menu to display the Circle PropertyManager. You can also invoke the Circle tool by using the Mouse Gesture. After invoking the Circle PropertyManager, select the appropriate method from the Circle Type rollout to draw the circle. Both methods to draw the circles are discussed next.

Figure 2-25 Partial view of the Circle PropertyManager

Drawing Circles by Defining their Center Points

CommandManager: Sketch > Circle flyout > Circle

SolidWorks menus: Tools > Sketch Entities > Circle

Toolbar: Sketch > Circle flyout > Circle

When you invoke the Circle PropertyManager, the Circle button is chosen by default in the Circle Type rollout. Also, the arrow cursor is replaced by the circle cursor. Specify the center point of the circle and then move the cursor away from the point to define its radius. The current radius of the circle will be displayed above the circle cursor. This radius will change as you move the cursor. Click on the drawing area away from the center point to define the radius. This radius can be modified by using the Circle PropertyManager. Also, the coordinates of the center point of the circle can be modified by using the Circle PropertyManager. Figure 2-26 shows a circle being drawn using the Circle tool by specifying the center point and dragging the cursor.

Figure 2-26 Drawing a circle by specifying the center point

Drawing Circles by Defining Three Points

CommandManager: Sketch > Circle flyout > Perimeter Circle

SolidWorks menus: Tools > Sketch Entities > Perimeter Circle

Toolbar: Sketch > Circle flyout > Perimeter Circle

The Perimeter Circle tool is used to draw a circle by defining three points that lie on the periphery of a circle. To draw a circle using this method, choose the Perimeter Circle tool from the Circle flyout. Alternatively, invoke the Circle PropertyManager and choose the Perimeter Circle button from the Circle Type rollout; the select cursor will be replaced by a three-point circle cursor. Specify the first point of the circle in the drawing area. Next, specify the other two points of the circle. The resulting circle will be highlighted in light blue and you can modify the circle by setting its parameters in the Circle PropertyManager. Figure 2-27 shows a circle being drawn by specifying three points.

Figure 2-27 Drawing a circle by specifying three point

Drawing Construction Circles

If you want to sketch a construction circle, draw a circle using the Circle tool and then select the For construction check box in the Options rollout of the Circle PropertyManager.

Tip

To convert a construction entity back to a sketched entity, invoke the Select tool and then select the construction entity; a popup toolbar will be displayed. Deactivate the Construction Geometry button in this toolbar.

DRAWING ARCS

In SolidWorks, you can draw arcs by using three tools: Centerpoint Arc, Tangent Arc, and 3 Point Arc. All these tools are grouped together in the Arc flyout in the Sketch CommandManager. You can invoke these tools from the flyout displayed on choosing the down arrow on the right of the Centerpoint Arc tool. The methods used to create arcs using these tools are discussed next.

Drawing Tangent/Normal Arcs

CommandManager: Sketch > Arc flyout > Tangent Arc

SolidWorks menus: Tools > Sketch Entities > Tangent Arc

Toolbar: Sketch > Arc flyout > Tangent Arc

The tangent arcs are the ones that are drawn tangent to an existing sketched entity. The existing sketched entities include the sketched and construction lines, arcs, and splines. The normal arcs are the ones that are drawn normal to an existing entity. You can draw tangent and normal arcs using the Tangent Arc tool.

To draw a tangent arc, invoke the Tangent Arc tool; the arrow cursor will be replaced by the tangent arc cursor. Move the arc cursor close to the endpoint of the entity that you want to select as the tangent entity. You will notice that an orange colored dot is displayed at the endpoint. Also, a yellow symbol is displayed with two concentric circles. Now, press the left mouse button once and move the cursor along the tangent direction through a small distance and then move the cursor to size the arc. The arc will start from the endpoint of the tangent entity and its size will change as you move the cursor. Note that the angle and radius of the tangent arc are displayed above the cursor, as shown in Figure 2-28. Click when the radius and angle values are closer to the desired values.

To draw a normal arc, invoke the Tangent Arc tool. Move the cursor close to the endpoint of the entity that you want to select as the normal entity; an orange colored dot will be displayed at the endpoint. Also, a yellow symbol is displayed with two concentric circles. Now, press the left mouse button once and move the cursor along the normal direction through a small distance and then move the cursor to size the arc, refer to Figure 2-29. Click when the radius and angle values are closer to the desired values.

Figure 2-28 Drawing a tangent arc

Figure 2-29 Drawing a normal arc

On invoking the Tangent Arc tool, the Arc PropertyManager will be displayed. However, the options in the Arc PropertyManager will not be enabled at this stage. These options will be enabled on selecting the completed tangent or normal arc.

You can draw an arbitrary arc and then modify its value using the Arc PropertyManager. Figure 2-30 shows partial view of the Arc PropertyManager.

Note

When you select a tangent entity to draw a tangent arc, the Tangent relation is applied between the start point of the arc and the tangent entity. Therefore, if you change the coordinates of the start point of the arc, the tangent entity will also be modified accordingly.

Figure 2-30 Partial view of the Arc propertyManager

Drawing Centerpoint Arcs

CommandManager: Sketch > Arc flyout > Centerpoint Arc

SolidWorks menus: Tools > Sketch Entity > Centerpoint Arc

Toolbar: Sketch > Arc flyout > Centerpoint Arc

The center point arcs are the ones that are drawn by defining the centerpoint, start point, and endpoint of the arc. When you invoke this tool, the arrow cursor is replaced by the arc cursor.

To draw a center point arc, invoke the Centerpoint Arc tool and then move the arc cursor to the point that you want to specify as the center point of the arc. Press the left mouse button once at the location of the center point and then move the cursor to the point from where you want to start the arc. You will notice that a dotted circle is displayed on the screen. The size of this circle will modify as you move the mouse. This circle is drawn for your reference and the center point of this circle lies at the point that you specified as the center of the arc. Press the left mouse button once at the point that you want to select as the start point of the arc. Next, move the cursor to specify the endpoint of the arc. You will notice that the reference circle is no longer displayed and an arc is being drawn with the start point as the point that you specified after specifying the center point. Also, the Arc PropertyManager, similar to the one that is shown in the tangent arc, is displayed on the left of the drawing area. Note that the options in the Arc PropertyManager will not be available at this stage.

If you move the cursor in the clockwise direction, the resulting arc will be drawn in the clockwise direction. However, if you move the cursor in the counterclockwise direction, the resulting arc will be drawn in the counterclockwise direction. Specify the endpoint of the arc using the left mouse button. Figure 2-31 shows the reference circle displayed when you move the mouse button after specifying the center point of the arc and Figure 2-32 shows the resulting center point arc.

Figure 2-31 Reference circle displayed after specifying the center point of the arc

Figure 2-32 The resulting center point arc

Drawing 3 Point Arcs

CommandManager: Sketch > Arc flyout > 3 Point Arc

SolidWorks menus: Tools > Sketch Entities > 3 Point Arc

Toolbar: Sketch > Arc flyout > 3 Point Arc

The three point arcs are the ones that are drawn by defining the start point and the endpoint of the arc, and a point on the circumference or the periphery of the arc. On invoking this tool, the arrow cursor is replaced by the three-point arc cursor.

To draw a 3 point arc, invoke the 3 Point Arc tool and then move the three-point arc cursor to the point that you want to specify as the start point of the arc. Press the left mouse button once at the location of the start point and then move the cursor to the point that you want to specify as the endpoint of the arc. As soon as you invoke the 3 Point Arc tool, the Arc PropertyManager will be displayed. Note that when you start moving the cursor after specifying the start point, a reference arc will be displayed. However, the options in the Arc PropertyManager will not be activated at this stage.

Specify the endpoint of the arc using the left mouse button. You will notice that the reference arc is no longer displayed. Instead, a solid arc is displayed and the cursor is attached to it. As you move the cursor, the arc will also be modified dynamically. Using the left mouse button, specify a point on the screen to create the arc. The last point that you specify will determine the direction and radius of the arc. The options in the Arc PropertyManager will be displayed once you draw the arc. You can modify the properties of the arc using the Arc PropertyManager. Figure 2-33 shows the reference arc drawn by specifying the start point and endpoint of the arc and Figure 2-34 shows the third point being specified for drawing the arc.

Figure 2-33  Specifying the start point and endpoint of the arc

Figure 2-34  Specifying the third point for drawing the arc

DRAWING RECTANGLES

In SolidWorks, the tools that are used to draw rectangles are grouped together in the Rectangle flyout. On invoking a tool from this flyout, the Rectangle PropertyManager will be displayed. Select an appropriate method to draw a rectangle from the Rectangle Type rollout. Alternatively, right-click and then choose the Corner Rectangle option from the shortcut menu to display the Rectangle PropertyManager. You can also invoke this PropertyManager by using the Mouse Gesture. Various methods to create a rectangle are discussed next.

Drawing Rectangles by Specifying their Corners

CommandManager: Sketch > Rectangle flyout > Corner Rectangle

SolidWorks menus: Tools > Sketch Entities > Corner Rectangle

Toolbar: Sketch > Rectangle flyout > Corner Rectangle

To draw a rectangle by specifying the two diagonally opposite corners, choose the Corner Rectangle button from the Rectangle Type rollout in the Rectangle PropertyManager, if it is not chosen by default. Next, move the cursor to the point that you want to specify as the first corner of the rectangle and then click the left mouse button once to specify the first corner. Now, move the cursor diagonally away from it. You will notice that the length and width of the rectangle are displayed above the rectangle cursor. The length is measured along the X-axis and the width is measured along the Y-axis. Next, specify the other corner of the rectangle using the left mouse button. Figure 2-35 shows a rectangle being drawn by specifying two diagonally opposite corners.

Figure 2-35  Drawing a rectangle by specifying two diagonally opposite corners

Drawing Rectangles by Specifying the Center and a Corner

CommandManager: Sketch > Rectangle flyout > Center Rectangle

SolidWorks menus: Tools > Sketch Entities > Center Rectangle

Toolbar: Sketch > Rectangle flyout > Center Rectangle

To draw a rectangle by specifying the centerand one of the corners, choose the Center Rectangle button from the Rectangle Type rollout in the Rectangle PropertyManager. Next, move the cursor to the point that you want to specify as the center of the rectangle and click the left mouse button. Then, move the cursor and specify one of the corners of the rectangle using the left mouse button. You will notice that the length and width of the rectangle are displayed above the rectangle cursor. The length is measured along the X-axis and the width is measured along the Y-axis. Figure 2-36 shows a rectangle being drawn by specifying its center and one of the corners.

Figure 2-36  Drawing a rectangle by specifying its center and one of the corners

Drawing Rectangles at an Angle

CommandManager: Sketch > Rectangle flyout > 3 Point Corner Rectangle

SolidWorks menus: Tools > Sketch Entities > 3 Point Corner Rectangle

Toolbar: Sketch > Rectangle flyout > 3 Point Corner Rectangle

To draw a rectangle at an angle, choose the 3 Point Corner Rectangle button from the Rectangle Type rollout in the Rectangle PropertyManager. Move the cursor to the point that you want to specify as the start point of one of the edges of the rectangle. Click the left mouse button at this point and move the cursor to size the edge. You will notice that a reference line is being drawn. Depending on the current position of the cursor, the reference line will be horizontal, vertical, or inclined. The current length of the edge and its angle will be displayed above the rectangle cursor. Specify the second point as the endpoint of the edge such that the reference line is at an angle.

Next, move the cursor to specify the width of the rectangle. You will notice that a reference rectangle is drawn at an angle. Also, irrespective of the current position of the cursor, the width will be specified normal to the first edge, either above or below it. Specify the third point using the left mouse button to define the width of the rectangle, as shown in Figure 2-37; the reference rectangle will be converted into a sketched rectangle.

Figure 2-37 Drawing a rectangle an angle

Drawing Centerpoint Rectangles at an Angle

CommandManager: Sketch > Rectangle flyout > 3 Point Center Rectangle

SolidWorks menus: Tools > Sketch Entities > 3 Point Center Rectangle

Toolbar: Sketch > Rectangle flyout > 3 Point Center Rectangle

To draw a centerpoint rectangle at an angle, choose the 3 Point Center Rectangle button from the Rectangle Type rollout in the Rectangle PropertyManager. Next, move the cursor to the point that you want to specify as the center point of the rectangle. Click the left mouse button once at this point and move the cursor to a distance that is equal to half the length of the rectangle to be drawn. You will notice that a reference line is being drawn. Depending on the current position of the cursor, the reference line can be horizontal, vertical, or inclined. The current length of the edge and its angle will be displayed above the rectangle cursor. Specify the second point using the left mouse button. Next, specify the third point to define the width of the rectangle.

You can select the From Corners or From Midpoints radio button from the Rectangle Type rollout to add construction lines from corner to corner or from midpoint of the sides of the rectangle respectively, as shown in Figures 2-38 and 2-39.

Figure 2-38  Specifying the third point when the From Corners radio button is selected

Figure 2-39 Specifying the third point when the From Midpoints radio button is selected

Drawing Parallelograms

CommandManager: Sketch > Rectangle flyout > Parallelogram

SolidWorks menus: Tools > Sketch Entities > Parallelogram

Toolbar: Sketch > Rectangle flyout > Parallelogram

To draw a parallelogram, choose the Parallelogram button from the Rectangle Type rollout of the Rectangle PropertyManager.