SolidWorks Quick Start Guide

JANUARY 2008

Lesson 1 - Parts Lesson 1 guides you through the creation of your first SolidWorks model. You create this simple part:

This lesson includes: ●

Creating a base feature

●

Adding a boss feature

●

Adding a cut feature

●

Modifying features (adding fillets, changing dimensions)

●

Displaying a section view of a part

Creating a New Part Document You begin this lesson by opening a new part document. 1. Click New

on the Standard toolbar.

The New SolidWorks Document dialog box appears. 2. Click Part, then click OK. A new part window appears. When toolbar buttons have an orange-colored border, for example , you can click them in the tutorial window to flash the corresponding button in the SolidWorks window.

1

Sketching the Rectangle The first feature in the part is a box extruded from a sketched rectangular profile. You begin by sketching the rectangle. 1. Click Extruded Boss/Base

on the Features toolbar.

The Front, Top, and Right planes appear, and the pointer changes to

.

Notice that as you move the pointer over a plane, the border of the plane is highlighted. 2. Select the Front plane. The display changes so that the Front plane is facing you. The Sketch toolbar commands appear in the CommandManager, and a sketch opens on the Front plane. 3. Click Rectangle

on the Sketch toolbar.

4. Move the pointer to the sketch origin

.

The pointer is on the origin when the pointer changes to

.

5. Click the origin, then move the pointer to create a rectangle. As you move the pointer, notice that it displays the dimensions of the rectangle. 6. Click again to complete the rectangle.

You do not have to be exact with the dimensions; you will use the Smart Dimension the next topic to dimension the sketch.

7. Click Select

tool in

on the Standard toolbar.

The two sides of the rectangle that touch the origin are black. Because you began sketching at the origin, the vertex of these two sides is automatically related to the origin. (The vertex is not free to move.) 2

The other two sides (and three vertices) are blue. This indicates that they are under defined and therefore, free to move. 8. Drag one of the blue sides or drag the vertex to resize the rectangle.

Adding Dimensions In this section you specify the size of the sketched rectangle by adding and changing dimensions. The SolidWorks software does not require that you dimension sketches before you use them to create features. However, for this example, you add dimensions now to fully define the sketch. 1. Click Options

on the Standard toolbar.

2. On the System Options tab, click General. 3. Clear Input dimension value , then click OK. This prevents automatic display of the Modify dialog box that is used for inputting new dimension values. 4. Click Smart Dimension The pointer changes to

on the Dimensions/Relations toolbar.

.

5. Click the top edge of the rectangle, then click where you want to place the dimension. The vertical line at the right changes from blue to black. By dimensioning the length of the top of the rectangle, you fully defined the position of the rightmost segment. You can still drag the top segment up and down (first click Smart Dimension

to turn the tool off). Its blue color

indicates that it is under defined.

6. Be sure Smart Dimension

is selected and click the right edge of the rectangle, then click

to place its dimension. The top segment and the remaining vertices turn black. The status bar in the lower-right corner of the window indicates that the sketch is fully defined.

3

Changing the Dimension Values In this section you change the dimensions. 1. Double-click one of the dimensions. The Modify dialog box appears. The current dimension is highlighted. 2. Set the value to 120, then click

.

The sketch changes size to reflect the new dimension. The dimension value is now 120mm. 3. Click Zoom to Fit

on the View toolbar to display the entire rectangle at full size and to

center it in the graphics area. 4. Double-click the other dimension and change its value to 120. 5. Click Zoom to Fit

again to center the sketch.

Extruding the Base Feature The first feature in any part is called the base feature. You create this feature by extruding the sketched rectangle. 1. Click Exit Sketch

on the Sketch toolbar.

The Extrude PropertyManager appears in the FeatureManager design tree (left panel), the view of the sketch changes to trimetric, and a preview of the extrusion appears in the graphics area. 2. In the PropertyManager, under Direction 1: ●

Select Blind in End Condition.

●

Set Depth

to 30. 4

3. Click OK

to create the extrusion.

The new feature, Extrude1, appears in the FeatureManager design tree and in the graphics area. 4. If you need to zoom to view the entire model, press Z to zoom out or press Shift+Z to zoom in. 5. Click the plus sign

beside Extrude1 in the FeatureManager design tree.

Sketch1, which you used to extrude the feature, is listed under the feature.

Saving the Part Now, you save the part. 1. Click Save

on the Standard toolbar.

The Save As dialog box appears. 2. In the File name box, type Tutor1 and click Save. The extension .sldprt is added to the filename, and the file is saved. File names are not case sensitive. That is, files named TUTOR1.sldprt, Tutor1.sldprt, and tutor1.sldprt are all the same part.

5

Sketching a Boss To create additional features on the part (such as bosses or cuts), you sketch on the model faces or planes, then extrude the sketches.

You sketch on one face or plane at a time, then create a feature based on one or more sketches.

1. Click Hidden Lines Removed 2. Click Extruded Boss/Base

on the View toolbar. on the Features toolbar.

3. Move the pointer over the front face of the part. The pointer changes to

, and the edges of the face become highlighted to show that the

face is available for selection.

4. Select the front face of the part. A sketch opens on the front face of the part. The Sketch toolbar commands appear in the CommandManager. 5. Click Circle

on the Sketch toolbar.

The pointer changes to

.

6. Click near the center of the face and move the pointer to sketch a circle. Click again to complete the circle.

Dimensioning and Extruding the Boss To establish the location and size of the circle, add the necessary dimensions. 6

1. Click Smart Dimension

on the Dimensions/Relations toolbar.

2. Select the top edge of the face, select the circle, then click a location for the dimension.

3. Double-click the dimension, set the value to 60 in the Modify dialog box, and click

to

dimension the circle to the top edge of the face.

4. Repeat the process to dimension the circle to the side edge of the face. Set this value to 60.

7

5. Still using Smart Dimension

, select the circle to dimension its diameter. Move the pointer

around to see the preview for the dimension. When the dimension is aligned horizontally or vertically, it appears as a linear dimension; if it is at an angle, it appears as a diameter dimension. 6. Click a location for the diameter dimension. Set the diameter to 70.

The circle turns black, and the status bar indicates that the sketch is fully defined. 7. Click Exit Sketch

on the Sketch toolbar.

The Extrude PropertyManager appears. 8. In the PropertyManager, under Direction 1, set Depth defaults, and click OK

to 25, leave the other items at the

to extrude the boss feature.

Extrude2 appears in the FeatureManager design tree.

Creating the Cut Create a cut concentric with the boss. To complete this, you create a sketch of the cut and dimension it. Next, you add relations to center the sketched circle on the boss. Finally, you extrude the cut. First, sketch and dimension the cut.

8

1. Click Shaded With Edges

on the View toolbar.

Occasionally a toolbar is longer than the length of your screen. If this occurs, click the arrows at the end of the toolbar to access the hidden toolbar buttons.

2. Click Extruded Cut

on the Features toolbar.

3. Select the front face of the circular boss. 4. Click Normal To

on the Standard Views toolbar.

The part is turned so that the selected model face is now facing you. 5. Sketch a circle near the center of the boss as shown. Click Smart Dimension

on the

Dimensions/Relations toolbar, and set the diameter of the circle to 50.

Next, add a concentric relation. 6. Click Add Relation

on the Dimensions/Relations toolbar.

The Add Relations PropertyManager appears. 7. Select the sketched circle (the inner circle) and the edge of the boss (the outer circle). The selections appear under Selected Entities. 8. Under Add Relations, click Concentric

.

Concentric0 appears under Existing Relations. The inner and outer circles now have a concentric relation. 9. Click OK

.

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Next, finish the cut. 10. Click Exit Sketch

on the Sketch toolbar.

The Cut-Extrude PropertyManager appears. 11. In the PropertyManager, under Direction 1, select Through All in End Condition. 12. Click OK

.

13. Click Trimetric

14. Click Save

on the Standard Views toolbar.

on the Standard toolbar to save the part.

You created the hole as a cut-extrude feature. However, you can also create holes using the Hole Wizard.

Rounding the Corners In this section you round the four corner edges of the part using a fillet feature. Because the fillets all have the same radius (10mm), you can create them as a single feature. First you change several display options to make it easier to see what happens as you create the fillets. 1. Click Options

on the Standard toolbar.

2. On the System Options tab, click Display/Selection.

10

3. Under Hidden edges displayed as, select Solid. This option makes it easier to see hidden lines when you use the Hidden Lines Visible view. 4. Under Part/Assembly tangent edge display, select As visible. This option makes it easier to see the filleted edges when you create them. 5. Click OK. 6. Click Hidden Lines Visible

on the View toolbar.

This view enables you to see the hidden edges. Next, you fillet the four corner edges of the part. 7. Select the first corner edge.

Notice how the faces, edges, and vertices highlight as you move the pointer over them, identifying selectable objects. Also, notice that the pointer changes: - Edge

- Face

- Vertex

8. Hold down the Ctrl key and select the remaining three corner edges.

11

You can use the Rotate View tool to help you select the edges. Click Rotate View View toolbar and drag to rotate the part, then click Rotate View the edges.

9. Click Fillet

on the

again and continue to select

on the Features toolbar.

In the PropertyManager, under Items To Fillet, the Edges, Faces, Features, and Loops box shows the four selected edges. If you move the pointer over a box or an icon in the PropertyManager, a tooltip appears with the name of the box or icon.

10. Under Items To Fillet, select Full preview. A preview of the fillets appears in the graphics area. 11. Set Radius 12. Click OK

to 10. .

The four selected corners are rounded. The Fillet1 feature appears in the FeatureManager design tree.

Adding More Fillets Now add fillets to other sharp edges of the part. You can select faces and edges either before or after opening the B PropertyManager. 1. Click Hidden Lines Removed

on the View toolbar.

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2. Click Fillet

on the Features toolbar.

3. Select the front face of the base.

A preview of the fillet appears on the outside edge of the base-extrude and the boss. The Edges, Faces, Features, and Loops list shows that one face is selected. The callout in the graphics area indicates the Radius 4. Under Items To Fillet, set Radius

. to 5, and click OK

.

The inside and outside edges are filleted in a single step.

5. Click Fillet

on the Features toolbar.

6. Select the front face of the circular boss.

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7. Set Radius

to 2, and click OK

.

Notice that the features listed in the FeatureManager design tree appear in the order in which you created them. 8. Click Shaded With Edges

on the View toolbar, then click Rotate View

on the View

toolbar and rotate the part to display different views.

9. Click Save

on the Standard toolbar to save the part.

Shelling the Part Next, you shell the part. Shelling hollows out the part by removing material from the selected face, leaving a thin-walled part. 1. Click Back

on the Standard Views toolbar.

14

2. Click Shell

on the Features toolbar.

The Shell PropertyManager appears. 3. Select the back face. The selected face appears under Parameters in the Faces to Remove 4. Under Parameters, set Thickness

to 2, then click OK

list.

.

The shell operation removes the selected face and leaves a thin-walled part.

5. To see the results, click Rotate View View

on the View toolbar and rotate the part. Click Rotate

again to turn the tool off.

Editing Existing Features You can edit any feature at any time. This section illustrates a way to change a dimension of an extruded feature. 1. Click Trimetric

on the Standard Views toolbar.

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2. Double-click Extrude1 in the FeatureManager design tree. The feature dimensions appear in the graphics area.

3. Double-click 30. The Modify dialog box appears. 4. Set the value to 50, then click 5. Click Rebuild

6. Click Save

.

on the Standard toolbar to update the feature with the new dimension.

to save the part.

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Displaying a Section View You can display a 3D section view of the model at any time. You use model faces or planes to specify the section cutting planes. In this example, you use the Right plane to cut the model view. 1. Click Trimetric

on the Standard Views toolbar.

2. Click Shaded

on the View toolbar.

3. Click Section View

on the View toolbar.

The Section View Property Manager appears. Under Section 1, the Front plane appears by default in the Reference Section Plane/Face box. 4. Under Section 1, click Right 5. Type 60 for Offset Distance

to select the Right plane. , and press Enter.

A section cut plane appears, offset 60mm from the Right plane.

You can also change the value for Offset Distance by clicking the up and down arrows Each time you click the arrows, the preview updates in the graphics area.

6. Click OK

.

.

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The section view of the part is displayed. Only the display of the part is cut, not the model itself. The section display is maintained if you change the orientation or zoom.

7. Click Section View

on the View toolbar to clear the section view.

The part returns to a complete view.

Congratulations! You have completed this lesson.

Lesson 2 - Assemblies An assembly is a combination of two or more parts, also called components, within one SolidWorks document. You position and orient components using mates that form relations between components. In this lesson, you build a simple assembly based on the part you created in Lesson 1. This lesson discusses the following: Adding parts to an assembly Moving and rotating components in an assembly

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Creating the Base Feature You can use the same methods you learned in Lesson 1 to create the base for a new part. 1. Click New

on the Standard toolbar, and open a new part.

2. Click Extruded Boss/Base

on the Features toolbar, and select the Front plane.

A sketch opens on the Front plane. 3. Sketch a rectangle beginning at the origin. 4. Click Smart Dimension

on the Dimensions/Relations toolbar, and dimension the rectangle

to 120mm x 120mm. 5. Click Exit Sketch

on the Sketch toolbar.

The Extrude PropertyManager and a preview of the extrusion appear. 6. Under Direction1: ●

Set End Condition to Blind.

●

Set Depth

to 90.

•

Click OK

to create the extrusion.

•

Click Hidden Lines Visible

•

Click Fillet

on the View toolbar

on the Features toolbar, and select the four edges shown.

19

•

In the PropertyManager, under Items to Fillet, set Radius

•

Click OK

to 10.

to fillet the selected edges.

Next, you shell the part.

7. Click Hidden Lines Removed 8. Click Shell

on the View toolbar.

on the Features toolbar.

The Shell PropertyManager appears. 9. Select the front face of the model.

The face is listed in Faces to Remove 10. Under Parameters, set Thickness 11. Click OK

in the PropertyManager. to 4.

.

12. Save the part as Tutor2.

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Creating a Lip on the Part In this section, you use the Convert Entities and Offset Entities tools to create sketch geometry. Then you create a cut to make a lip to mate with the part from Lesson 1.

1. Click Zoom to Area Click Zoom to Area

on the View toolbar, and drag-select to a corner of the part, as shown. again to turn off the tool.

2. Select the front face of the thin wall. The edges of the face are highlighted.

3. Click Extruded Cut

on the Features toolbar.

A sketch opens on the selected face. 4. Click Convert Entities

on the Sketch toolbar.

The outer edges of the selected face are projected (copied) onto the sketch plane as lines and arcs.

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5. Click the front face again. 6. Click Offset Entities

on the Sketch toolbar.

The Offset Entities PropertyManager appears. 7. Under Parameters, set Offset Distance

to 2.

The preview shows the offset extending outward. 8. Select Reverse to change the offset direction.

9. Click OK

.

A set of lines is added to the sketch, offset from the outside edge of the selected face by 2mm. This relation is maintained if the original edges change.

10. Click Exit Sketch

on the Sketch toolbar.

The Cut-Extrude PropertyManager appears. 22

11. Under Direction 1, set Depth

to 30, then click OK

.

The material between the two lines is cut, creating the lip.

12. Click Zoom to Fit

on the View toolbar.

Changing the Color of a Part You can change the color and appearance of a part or its features.

1. Click Shaded With Edges

on the View toolbar.

2. Select the Tutor2 icon at the top of the FeatureManager design tree. 3. Click Edit Color

on the Standard toolbar.

The Color And Optics PropertyManager appears.

4. Under Favorite, select the desired color on the color palette, then click OK

.

5. Save the part.

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Creating the Assembly Now create an assembly using the two parts.

1. If Tutor1.sldprt is not open, click Open 2. Click New

on the Standard toolbar and open the part.

on the Standard toolbar, click Assembly, then click OK.

The Insert Component PropertyManager appears. 3. Under Part/Assembly to Insert, select Tutor1. A preview of Tutor1 appears in the graphics area, and the pointer changes to

4. Click Keep Visible

.

in the PropertyManager, so you can insert more than one component

without having to re-open the PropertyManager. 5. Click anywhere in the graphics area to place Tutor1. 6. In the PropertyManager under Part/Assembly to Insert, select Tutor2. 7. Click in the graphics area to place Tutor2 beside Tutor1. 8. Click OK

.

9. Click Zoom to Fit

.

10. Save the assembly as Tutor. (The .sldasm extension is added to the file name.) If you see a message about saving referenced documents, click Yes.

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Mating the Components In this topic, you define assembly mating relations between the components, making them align and fit together.

1. Click Mate

on the Assembly toolbar.

The Mate PropertyManager appears. 2. In the graphics area, select the top edge of Tutor1, then select the outside edge of the lip on the top of Tutor2.

The Mate pop-up toolbar appears, and the components move into place, previewing the mate. The edges are listed in the Entities to Mate

box under Mate Selections in the

PropertyManager. 3. On the Mate pop-up toolbar, do the following:

●

Click Coincident

as the mate type.

●

Click Add/Finish Mate

.

A coincident mate appears under Mates in the PropertyManager. The position of Tutor2 is not fully defined yet. It still has some degrees of freedom to move in directions that are not yet constrained by mates.

25

Test degrees of freedom by moving the components. 4. In the graphics area, select the Tutor2 component and hold down the left mouse button.

5. Drag the component from side to side to observe the available degrees of freedom.

Adding More Mates 1. Select the rightmost face of one component, then select the corresponding face on the other component.

2. On the Mate pop-up toolbar, click Coincident

, then click Add/Finish Mate

.

Another coincident mate appears under Mates in the PropertyManager.

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3. Repeat steps 1 and 2, but select the top faces of both components, to add another Coincident mate.

4. Click OK

.

5. Save the assembly.

Using Display States You can change the display settings of the components and save the settings in a display state.

1. At the top of the FeatureManager design tree, select the ConfigurationManager 2. Expand Default

and Display State

tab.

. 27

3. Right-click Display State

and select Add Display State.

4. On the FeatureManager design tree

tab, click

(to the right of the tabs) to show the

Display Pane. The Display Pane shows the different display settings (color, texture, etc.) of each component. 5. Move the pointer over Tutor2 in the FeatureManager design tree, then: ●

Move the pointer into the Display Mode

●

When the pointer changes to

6. On the ConfigurationManager

column.

, click, then select Hidden Lines Visible

.

tab, double-click Display State-1.

The assembly returns to its original display state.

Congratulations! You have completed this lesson!

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Lesson 3 - Drawings In this lesson, you create a multi-sheet drawing of the parts and assembly from Lessons 1 and 2. This lesson includes: ●

Opening a drawing template and editing a sheet format

●

Inserting standard views of a part model

●

Adding model and reference annotations

●

Adding another drawing sheet

●

Inserting a named view

●

Printing the drawing

Opening a Drawing Template First you open a drawing template.

1. Click New

on the Standard toolbar.

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2. Click Drawing, then click OK. A new drawing appears in the graphics area, and the Model View PropertyManager appears.

Next you edit the sheet format by changing some text properties. Since you are working on the sheet format, and not inserting a model in the drawing yet, cancel the PropertyManager.

3. Click Cancel

in the PropertyManager.

4. Right-click anywhere in the drawing sheet, and select Edit Sheet Format. 5. In the title block, double-click the text .

You can use the zoom tool to make selection easier. Click Zoom to Area toolbar, and drag-select to the title block at the lower right. Click Zoom to Area

on the View again to turn off

the tool.

The text appears in an edit box. 6. Change the text to the name of your company. 7. Click outside of the text area to save your changes. 8. Click the text again. 9. In the PropertyManager, click Font and change the font, size, or style, then click OK.

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You can also use the Formatting toolbar to change the font, size, or style. If the Formatting toolbar is not visible, click View, Toolbars, Formatting.

10. Click outside of the text area to save your changes. 11. Click Zoom to Fit

on the View toolbar.

12. Right-click anywhere in the drawing sheet, and select Edit Sheet to exit the edit sheet format mode.

Saving the Drawing Sheet Format Next you save the updated sheet format. This is different from saving the drawing itself. 1. To replace this format as the standard A-Landscape format, click File, Save Sheet Format. 2. In Save in, navigate to \data\. 3. Click a-landscape.slddrt, then click Save. 4. Click Yes to confirm that you want to overwrite the existing sheet format. When you choose this sheet format for your own drawings, you do not need to perform these edits again. To save the sheet format with a new name and to not overwrite the standard sheet format, click File, Save Sheet Format. Navigate to the directory where you want to save the format. Type a name and click Save.

Setting the Detailing Options Next, set the default dimension font, and set the style of dimensions, arrows, and other detailing options. For this lesson, use the settings described below. Later, you can set the detailing options to match your company’s standards.

1. Click Options

on the Standard toolbar. 31

2. On the Document Properties tab, click Detailing. 3. Under Dimensioning standard, select Remove in Trailing zeroes to remove all trailing zeroes from the dimensions displayed. 4. Click Annotations Font. 5. Under Annotation type, select Dimension. The Choose Font dialog box appears. 6. Under Height, set Points to 12, then click OK. 7. Click OK again to close the dialog box.

Creating a Drawing of a Part 1. Open Tutor1.sldprt if it is not open. Then return to the drawing window.

2. Click Model View

on the Drawing toolbar.

The pointer changes to

.

3. In the PropertyManager, do the following: a.Under Part/Assembly to Insert, select Tutor1. b.Click Next

.

c.Under Orientation: •

Select View orientation.

•

Click *Front

•

Select Preview to display a preview in the graphics area.

under Standard views.

1. Under Options, select Auto-start projected view to automatically display the Projected View PropertyManager when you place an orthogonal model view. 2. Under Display Style, click Hidden Lines Removed

.

3. Under Scale, select Use custom scale, User Defined, and set to 1:4. 32

3. Move the pointer into the graphics area.

The pointer changes to

with a preview of the front view of Tutor1.sldprt.

4. Click to place the front view as Drawing View1, as shown below.

After the PropertyManager is closed, when you move the pointer over this view, the tooltip identifies it as Drawing View1.

5. Move the pointer up, and click to place Drawing View2, then move to the side and click to place Drawing View3.

6. VClick OK

.

This tutorial uses Third angle projection, so Drawing View2 is the Top view, and Drawing View3 is the Right view.

To use First angle projection, right-click anywhere on the drawing sheet, and click Properties. Then select First angle in the Sheet Properties dialog box. In first angle projection, Drawing View2 is the Bottom view and Drawing View3 is the Left view.

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Moving Drawing Views You move a view by clicking and dragging when the pointer changes to include . This pointer appears when you are over the view border, a model edge, and so on. You can drag the view in its allowed directions. 1. Click Drawing View2 (the upper left view on the sheet), then drag it up and down. 2. Click Drawing View3 (the lower right view), then drag it left and right. Drawing View2 and Drawing View3 are aligned to Drawing View1, and move in only one direction to preserve the alignment. 3. Click Drawing View1 and drag it in any direction. The other two views move to maintain alignment with Drawing View1. 4. Move the views on the drawing sheet to the approximate positions shown.

Adding Dimensions to a Drawing Drawings contain 2D views of models. You can choose to display dimensions specified in the model in all of the drawing views.

1. Click Model Items

on the Annotations toolbar.

The Model Items PropertyManager appears. You can select which types of dimensions, annotations, and reference geometry to import from the model.

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2. Under Source/Destination: ●

Under Source, select Entire model in Import from to import all the model dimensions.

●

Select Import items into all views.

●

Under Dimensions:

●

Click Marked for drawing

to insert only those dimensions that are marked in parts

for drawings. ●

Select Eliminate duplicates to insert unique model items only.

3. Click OK

.

Dimensions are imported into the view where the feature they describe is most visible.

4. Drag the dimensions to position them as shown. 5. Click Save on the Standard toolbar and save the drawing document as Tutor1. The default extension is .slddrw.

Modifying Dimensions When you change a model dimension in the drawing view, the model is automatically updated to reflect the change, and vice versa. 35

1. In Drawing View2, double-click the dimension for the depth (25) of the boss extrusion. The Modify dialog box appears.

2. Change the value from 25 to 40, and click Rebuild

.

The part rebuilds using the modified dimension. Both the drawing and the part are updated.

Click

.

Save the drawing. The system notifies you that the model referenced in the drawing has been modified, and asks if you want to save it. Click Yes to save both the drawing and the updated model.

Now check the part. 3. Click Window, and select the Tutor1.sldprt window. 36

4. Double-click Extrude2 in the FeatureManager design tree to display the dimensions of the feature. Notice that the depth dimension is 40mm. 5. Click anywhere in the graphics area to turn off the dimensions. Now rebuild the assembly that contains the modified part. 6. Open Tutor.sldasm if it is not still open. If a message appears asking you to rebuild the assembly, click Yes.

If the message does not appear, click Rebuild

on the Standard toolbar.

The assembly rebuilds with the new dimensions. 7. Save Tutor.sldasm, then return to the drawing window.

Adding Another Drawing Sheet Now you create an additional drawing sheet for the assembly. You then use the Browse command to insert an assembly document into the drawing.

1. If the PropertyManager is still open, click OK

to close it.

2. Right-click on any open area of the drawing sheet and select Add Sheet. Another sheet of the same size as Sheet1 is added to the drawing.

3. Click Standard 3 View

on the Drawing toolbar.

4. In the PropertyManager, select Tutor.sldasm

then click OK

.

5. Reposition the views on the sheet as shown below.

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You can use Standard 3 View can use Model View

to add all three standard views to a drawing at once, or you

to add one view at a time. The resulting views are the same.

Inserting Another View You can add more views to drawings to show the model in different orientations. In this topic you add a standard isometric view of the assembly. 1. Click Model View

on the Drawing toolbar.

2. In the PropertyManager, do the following: ●

Under Part/Assembly to Insert, select Tutor

●

Click Next

●

Under Orientation, click Isometric

●

Under Display style, click Shaded With Edges

●

Under Scale, select Use sheet scale.

.

. under Standard views. .

The pointer changes to 3. Click in the sheet to place the view. 4. Click

.

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Printing the Drawing 1. Click File, Print. The Print dialog box appears. 2. Under Print range, select All to print both sheets. 3. Click Page Setup. The Page Setup dialog box appears, where you can change printer settings such as resolution, scale, paper size, and so on. 4. Under Resolution and Scale, select Scale to fit. 5. Click OK to close the Page Setup dialog box. 6. Click OK again to close the Print dialog box and to print the drawing. 7. Click Save

on the Standard toolbar.

8. If the system notifies you that the model referenced in the drawing has been modified, and asks if you want to save it, click Yes. 9. Close the drawing.

Congratulations! You have completed this lesson. 39