SolidWorks 2010- P7

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SolidWorks 2010- P7: Whether you are a new user of SolidWorks or a professional who wants to improve your skills, this book was written for you. Learning any software can be difficult at times. You launch the software for the first time, and you feel overwhelmed, not knowing how to even start a new document. In 3D CAD programs, it can be especially difficult. Many times a whole new vocabulary and a whole new creative environment are introduced.

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Nội dung Text: SolidWorks 2010- P7

Chapter 4 Creating Your First Drawing Create a Drawing from a Part Add Views Annotate the Drawing Finalize the Drawing Share the Drawing
150 C h a p t e r 4 • C r e a t i n g Yo u r F i r s t D r a w i n g P rior to the introduction of computers to the engineering world, drawings were painstakingly drawn by hand by drafters who were artists in their own right. Using straight edges, triangles, scales, and graphite pencils of varying hardness, drafters would create drawings that could be placed on the walls in any art museum. Not only were they created with a certain artistic flair, these hand-drawn drawings were precise instructions that gave the manufacturer all the information needed to accurately produce the product being depicted. Gone is the era of hours, days, weeks, and even months of hand-cramping draw- ings. With today’s 3D CAD applications such as SolidWorks, creating an accurate drawing is easier than ever. In SolidWorks, models are created to capture the design intent and to be 100 percent accurate. The models are then used to create the draw- ings. As the models are revised, the drawings will automatically update as well. This, of course, all depends on whether the correct procedures are followed. Drawings that are incorrectly produced may still be dimensionally accurate, but revisions often take longer to document than the original drawing did. But by following the steps described in this chapter, you will be able to quickly create drawings that will be even easier to revise in the future. Some of the steps may seem like they create extra work, but we promise you that they will all be worth it in the future. As you might have noticed so far in this book, many tasks in SolidWorks can be performed in different ways yet still have the same result. The steps described in this chapter are just one approach to creating drawings, but throughout the book we will be introducing you to alternative approaches as well. Create a Drawing from a Part In the previous chapter, you created a 3D model of the lamp base, and you will be using that model to create a drawing. There are more than a couple of ways to create drawings from models, but this chapter will concentrate on probably the quickest and easiest ways. This chapter will use a drawing template that has been created with predefined drawing views. Predefined drawing views are cre- ated in templates to automatically create orthographic drawing projections from a model. Without predefined drawing views, you would need to create the pro- jections manually when creating a new drawing. The most common way to make a drawing is to insert the part into a drawing and then create the necessary projections before applying dimensions. When com- pared to using a template that has predefined drawing views, this approach adds only a minute or two to the overall time it takes to create a drawing. But when you begin making many drawings for a large project, those couple of extra minutes per
Create a Drawing from a Part 151 drawing can really add up. That is why we use a variety of drawing templates for each sheet size ranging from no predefined views up to all six views that would nor- mally be used for an orthographic drawing. Although this chapter concentrates on creating a drawing from a template with predefined drawing views, it is not the only, or even the best way, to create drawings. That is why we will show you how to use a variety of techniques to create drawing views throughout this book. Download and Install the Drawing Template Before going any further, you will need to download the drawing template named FDC Size B from the companion site. After downloading it, save the template to the Document Templates folder. If you don’t place the template into the correct folder, it will not show up in the New SolidWorks Document window. Not only is the Document Templates folder used for drawing templates, but it is also used for part templates, assembly templates, and other templates. The folder can reside on your computer’s hard drive, or it can reside on a network drive. In fact, many companies, to ensure that all drawing, parts, and assemblies are consistent, will store all of their templates in a public folder on the network that will be shared by all installations of SolidWorks. If you do not know where your Document Templates folder is located, you can check where SolidWorks is looking for templates. You can find this information in the File Locations section of the System Properties window. The File Locations section not only specifies where document templates can be found but also where sheet formats, color swatches, the materials database, and other files are located. To look up the location of the Document Templates folder, do the following: 1. Enter the System Options window by clicking the Options button in O the menu bar. In Chapter 15, you 2. Click the File Locations link in the left pane of the System Options will learn how to window. create the template used in this chapter. 3. In the File Locations section of the System Options window, click the Show Folders For field, and select Document Templates from the list if it is not already selected. 4. In the Folders field, you will see the full path of the Document Templates folder. Make note of the folder path shown in the field. 5. Using Windows Explorer, browse to the folder specified in the System Options window. Copy the template downloaded from the companion site, and close Windows Explorer.
152 C h a p t e r 4 • C r e a t i n g Yo u r F i r s t D r a w i n g N O t e If you need to specify another folder for your document tem- plates, click the Add button next to the Folders field, browse to the new location in the Browse For Folder window, and click OK. Open the Drawing Template Once you’ve downloaded the drawing template and copied it to the appropriate folder, the template will be available for use in the New SolidWorks Document window. Since you are using a drawing template that contains predefined draw- ing views, it’s easier to create the drawing from the part model rather than inserting the model view into the drawing. To create a drawing from the part model, do the following: 1. Click Open on the menu bar, and browse to the folder that you saved the Base, Lamp model from Chapter 3. 2. Select the Base, Lamp model, and click Open. You can also access 3. Click the downward-pointing arrow next to the New button on the the Open window by menu bar, and select Make Drawing From Part/Assembly. pressing Ctrl+O on your keyboard. 4. In the New SolidWorks Document window, click the Advanced button located in the lower-left corner of the window. t I p You can always return to the simple interface for opening templates by clicking the Novice button in the lower-left corner of the New SolidWorks Document window. 5. In the Advanced view of the New SolidWorks Document window, select the FDC Size B drawing template, and click OK (see Figure 4.1). As soon as you click OK in the New SolidWorks Document window, the new drawing will be created with the predefined views displaying the projected views of the lamp base, as shown in Figure 4.2. This cuts out at least a couple of minutes that would otherwise be used to place the initial views and create the required projections.
Create a Drawing from a Part 153 F I g u r e 4 . 1 Advanced view of New SolidWorks Document window F I g u r e 4 . 2 Drawing created with predefined views 6. Click the Save button on the menu bar, and ensure that you are in the current folder that the Base, Lamp model is saved. Enter Base, Lamp in the File Name field, and click Save.
154 C h a p t e r 4 • C r e a t i n g Yo u r F i r s t D r a w i n g Add Views In the previous section, you saw firsthand the advantages of creating a drawing template with predefined views. Taking the extra couple of minutes of planning when creating the template will save time in the long run, especially when you consider how many drawings you may create in an average week. A couple of saved minutes per drawing adds up when you are responsible for making hun- dreds of drawings. Even though you were able to eliminate the need to create all the views in the drawing by adding predefined views, it is impossible to add every view that is necessary to fully tell the story. So, in addition to the views that were created automatically, you will need to add a couple more views to the drawing. The drawing is going to require the addition of a section view, a projected view, a broken-out section, and a detail view, all of which are required to be able to fully describe what is going on with the part. Since this is a fairly simple part, you can get away with only a few views, but it is not unheard of to have some draw- ings with anywhere from one to hundreds of views just to describe one part. Add Sectioned Views Sectioned views are important in drawings to be able to show what is going on inside a part. Even though you could always show the part with hidden lines, this could be extremely confusing. Plus, if you have ever taken a drafting class, you may remember your instructor telling you that you cannot dimension to hidden lines. Hidden lines are meant just for reference and clarity and should not be used to actually manufacture the part. So, what is a sectioned view? Imagine taking the finished part for the lamp base and cutting it in half with a band saw. The cross section allows you to see the shape and size of the inside geometry. That is what a sectioned view in a drawing allows you to do. It is a virtual cross section of the part and gives you access to the inside features of the part for dimensioning. The section is necessary to be able to show the depth of the pocket and other information on the inside of the part that would normally be obscured. The fol- lowing steps will walk you through the process of creating a cross section of the lamp base: 1. Click the Zoom To Area button in the Heads-up View toolbar, and drag a window around the Front view of the lamp base (see Figure 4.3).
Add Views 155 F I g u r e 4 . 3 Zooming in on the Front view of the lamp base 2. Press S on your keyboard, and click the Drawings button on the short- cut bar. In the Drawings flyout, select the Section View flyout and then Section View, as shown in Figure 4.4. The mouse pointer will change to a pencil with a blue line under it to signify that a line must be drawn. F I g u r e 4 . 4 Selecting Section View in the shortcut bar t I p Throughout this book, you’ll use the shortcut bar almost exclu- sively. Instead of pressing S on your keyboard each time, you can assign the Shortcut Bar command to the mouse gesture guides. Select Tools ➢ Customize, and select the Mouse Gestures tab. Type Shortcut in the Search For field, and assign a direction to the command. 3. Move the mouse pointer to the midpoint of the top of the boss on the Front view, and slowly move it up once the pointer includes a small yellow icon representing the coincident relation, as shown in Figure 4.5.
156 C h a p t e r 4 • C r e a t i n g Yo u r F i r s t D r a w i n g F I g u r e 4 . 5 Icon next to pointer representing coincident relation 4. With the mouse pointer a small distance above the top of the boss, click the left mouse button and release to begin drawing a line. 5. Draw the line vertically down, bisecting the lamp base. 6. When the line extends slightly below the bottom of the lamp base, click and release the left mouse button to complete the line, as shown in Figure 4.6. F I g u r e 4 . 6 Drawing a line to bisect the part model 7. A section arrow will now be drawn where the line was created, and all that is left to do is place the section view. Press F on your keyboard or double-click the scroll wheel to fit the entire drawing on the screen. 8. Move the section view to the left of the Front view of the lamp base, and then click and release the left mouse button. 9. In the Section View PropertyManager, enable the Flip Direction option, as shown in Figure 4.7. Click the green check mark to accept the changes.
Add Views 157 F I g u r e 4 . 7 Section View PropertyManager The part has now been sectioned, giving you access to the inner geometry for dimensioning. The new section view will automatically be labeled as Section A-A, as shown in Figure 4.8, and if you were to create a second sectioned view, it would be labeled as Section B-B. N O t e In later chapters, you will be exploring the section views in more detail, but in the meantime, we encourage you to explore the options available in the Section PropertyManager. Simply select the section view in the graphics area, and you will be able to make adjustments to the view in the PropertyManager. F I g u r e 4 . 8 Newly created section labeled Section A-A Add Projected Views The drawing template downloaded from the companion site already has pre- defined views for the Front, Top, Right, and Isometric views. For many draw- ings, these views are more than sufficient to fully describe the part. For this particular part, you will need a couple of additional views in order to be able to show the features on the back and bottom of the part.
158 C h a p t e r 4 • C r e a t i n g Yo u r F i r s t D r a w i n g Using projected views allows you to add these views and take on the properties from the parent view such as Scale and Display Style. These new projected views will also be connected to the original views, which means that if one of the views is moved on the sheet, the dependant view will move along with it, ensuring that the integrity of the drawing layout is preserved. The following steps describe the process for creating the two new views from the existing views instead of adding new views to the drawing: 1. Select the Right view by clicking and releasing the left mouse button with the pointer inside the bounding area of the view. 2. Press S on your keyboard, and click the Drawing Commands button. In the flyout, click the Projected View button. 3. Place the projected view of the back of the lamp base to the right of the view. 4. Select the Front view of the lamp base, and once again click the Projected View button in the shortcut bar. 5. Place the new projection below the Front view to create a view of the bottom of the lamp base, as shown in Figure 4.9. F I g u r e 4 . 9 Projected view of bottom of lamp base
Add Views 159 Once you place the projected views, you can move them around to clean up the arrangement of the views on your drawing. But, you will only be able to move the views in line with the projection unless you break the alignment of the view. Very rarely will you need to break the alignment, but when the time comes, it is a good skill to know. To be able to move a projected view elsewhere on the drawing, right- click the view, and select Break Alignment in the Alignment flyout of the menu. Add a Broken-out Section A broken-out section is similar to a section view in that it is used to show the internal geometry of a part, but instead of creating a new view that shows the section, the parent view shows a broken area. This is equivalent to getting a hammer and knocking off a chunk of the part to be able to see the inside. The rest of the view shows the outside geometry, but in the broken-out section, the inside geometry can be seen and dimensioned. The advantage of using a broken-out section is that you will not need to create a new view, which is extremely important if space is a consideration. Plus, if you need to show only a small area of the part, it seems to be overkill to create a large section view. In the example drawing, instead of creating a new section view to be able to show the cross section of the AC cord hole, you’ll use a broken-out sec- tion. Here’s how to do it: 1. Zoom in closer to the Bottom view by using the Zoom To Area button in the Heads-up View toolbar or by using the scroll wheel on your mouse. 2. Select the Bottom view by clicking and releasing the left mouse but- ton with the mouse pointer directly over the view. 3. In the Heads-up View toolbar, click the Display Style button, and click the Hidden Lines Visible button in the flyout. 4. Select the Sketch tab in the CommandManager, and click the Spline tool. 5. Create a closed spline profile that completely surrounds the hid- den lines that represent the hole on the back of the base by clicking around the area as many times as required to create a spline that somewhat represents the one shown in Figure 4.10. N O t e Splines are 2D or 3D curves that are defined with multiple points. As points are selected, a continuous smooth line is created. Splines have many uses in SolidWorks, and you will be using them throughout your career as a SolidWorks designer. But in this section, you will be using the spline solely for creating the break-out section.
160 C h a p t e r 4 • C r e a t i n g Yo u r F i r s t D r a w i n g F I g u r e 4 . 1 0 Creating a closed spline profile 6. After creating the closed spline profile, press S, and click the Drawings button on the shortcut bar. 7. Click Broken-Out Section in the flyout. 8. Pan to the Back view of the lamp base, and select the circumference of the hole, as shown in Figure 4.11. This will set the depth of the cut- out to be exactly the center point of the hole. F I g u r e 4 . 1 1 Defining the depth of a broken-out section W a r N I N G You can also define the depth of the broken-out sec- tion in the PropertyManager, but if you take that approach, the depth will not change as the surrounding geometry changes. This is why here you have selected the circle that makes up the hole in the back of the lamp base. If the location or size of the hole changes, the broken-out section will always be based on the center of the hole. 9. Click the Preview option in the Broken-Out Section PropertyManager to see what the broken-out section will look like when created (see
Add Views 161 Figure 4.12). Make sure that the hole along with the lead-in chamfer can be seen clearly without hidden lines. F I g u r e 4 . 1 2 Previewing the broken-out section 10. Click the green check mark in the Broken-Out Section PropertyManager to complete the section. 11. Make sure the Bottom view is selected, and click the Hidden Lines Removed button in the Heads-up View toolbar. The broken-out section is now ready to be dimensioned, but because of the size of the part, it may be a little difficult. So, in the next section, you will be creating a detailed view that will allow you to apply dimensions to a larger repre- sentation of the section. Add a Detailed View A detailed view is a partial view of a part that is most often at a larger scale than the original part, allowing for greater detail. Using detailed views allows you to dimension smaller features of a part without having to increase the overall scale of the drawing, which is another way to conserve valuable sheet real estate. The following steps will create a detail of the broken-out section created in the previ- ous section: 1. Press S on your keyboard, and click the Drawing Commands button in the shortcut bar. 2. In the Drawing Commands flyout, click the Detail View button. 3. Click near the center of the cross section of the hole in the broken- out section you just created. 4. Drag the circle out from the center until the entire broken-out sec- tion falls completely inside. Click the left mouse button to create the circle, as shown in Figure 4.13.
162 C h a p t e r 4 • C r e a t i n g Yo u r F i r s t D r a w i n g F I g u r e 4 . 1 3 Selecting part of the model to view in detail 5. Move the mouse pointer (with the detail view attached) to an empty area of the drawing, and click the left mouse button to place the view (see Figure 4.14). F I g u r e 4 . 1 4 Placing a detail view in the drawing Unlike projected views and sections, a detail view can be moved anywhere in the drawing sheet without limitations. In fact, if it is necessary, you can move the detail view to a completely different sheet in the drawing. This is hugely helpful if you are short on space in the drawing. Also, the scale of the detail view can be changed independently from the rest of the views in the drawing. If you think the current detail view is still too small at its current scale, select the view and adjust the scale in the PropertyManager. Annotate the Drawing With all the required views created on the drawing, it is time to start applying dimensions. Many users opt to add dimensions manually at this point, but that approach would cause you to miss out on one of the greatest advantages to cre- ating drawings in SolidWorks—bidirectionality. When done correctly, not only are dimensions on the drawing updated when the part model is revised, but it
Annotate the Drawing 163 can go the other way. If you make a change to a dimension in the drawing, the model will update at the same time. Dimensions that are manually placed on the drawing are actually reference dimensions. Many users or organizations tend to change the system options of SolidWorks to display reference dimensions as regular dimensions. Although not technically correct, many users find that this approach to annotating a drawing is quicker and easier. Reference dimensions that are manually added to a draw- ing do not affect the part geometry but will update automatically as the part is updated. However, if the part was not created with fully defined sketches or the sketches were not defined with the design intent in mind, adding reference dimensions would be quicker and easier than making changes to the part model. With the steps described in this section, you will learn how to use the pre- ferred method of annotating a drawing, but we would like to stress that it is not the only accepted technique. Instead of adding dimensions to the drawing, you will be importing the dimensions that you used to fully define the lamp base model in both the sketches and features. This is one of the main reasons we’re stressing the importance of design intent when defining sketches and features. If you did the model correctly, the model dimensions that are imported into the drawing would be those required to make the part per your design intent with- out the need for adding too many extra dimensions. Of course, as we have mentioned a few times already, there is more than one way to do most things in SolidWorks. The steps described here are not the only way and may not be the preferred method to some users, but we find these are the easiest ways to annotate your drawing. In later chapters, you will be explor- ing more options for annotating drawings that will also meet the requirements. U n d e r s ta n d i n g d i m e n s i o n s Throughout this book, we will often mention the various elements of a dimension. It is important to understand what the different elements that make up a dimension are before continuing. You can see a dimension, dimension line, and extension line here. Extension Line Dimension Dimension Line
164 C h a p t e r 4 • C r e a t i n g Yo u r F i r s t D r a w i n g Dimension Lines A dimension line is a straight or curved line with arrows used to specify the extents and the direction of the dimension being applied. The dimen- sion line is often broken to include the dimension value, depending on the drafting standard used. extension Lines Extension lines are lines drawn perpendicular to the dimension line and are used to connect the dimension line to the part surface or points. A small gap is made between the end of the extension lines and the area being dimen- sioned to prevent the extension line from obscuring the area. If space is a concern, the extension lines can be made oblique, or slanted, to the part. Import Annotations As long as the dimensions that you used to define the sketches in the part are marked for use in the drawing, you can import those dimensions directly into the drawing. Luckily, all the dimensions are automatically marked for drawing, but if that weren’t the case, you could right-click dimensions and select Mark For Drawing from the menu. The dimensions that will be inserted into the drawing are the ones used in the sketch and features to create the model. This is one of the reasons that when creating sketches, the sketch should be dimensioned to define the design intent. If you just arbitrarily placed dimensions in the sketches, the dimensions imported into your drawing would not make any sense, and you might be forced to manually dimension the drawing views. Here are the steps to perform the import: 1. Press S to view the shortcut bar, and click the Annotations button to view the tools available in the flyout. 2. Select Model Items from near the top of the menu. 3. In the Source/Destination section of the Model Items PropertyManager, ensure that the source is set to Selected Feature. Also, make sure that the Import Items Into All Views option is enabled in the same section.
Annotate the Drawing 165 4. Depending on the feature being annotated, different types of dimen- sions may be necessary. In the Dimensions section, you can specify the type of dimensions that will be used for the selected feature. In the Dimensions section of the PropertyManager, select the buttons Marked For Drawing, Instance/Revolution Count, and Hole Callout. 5. In the Options section of the PropertyManager, select Include Items From Hidden Features and Use Dimension Placement In Sketch. This will make use of the layout that was used in the sketch of the part. This is another example of why the extra steps taken in the creation of the part can help with time management later in the process. 6. Rather than spending the time to fully dimension the drawing at this time, only a couple of features will be annotated to save time. You can always go back later to finish the rest of the features. For the time being, start by zooming in on the Section A-A view. While the Model Items PropertyManager is still active, click the inside face of the counterbore for the boss, as shown in Figure 4.15. F I g u r e 4 . 1 5 Selecting a feature to import annotations
166 C h a p t e r 4 • C r e a t i n g Yo u r F i r s t D r a w i n g 7. After selecting the inside face of the counterbore, the dimensions used when creating the feature, including the chamfer, are imported into the drawing. If those were the only dimensions that were meant to be imported, you could click the green check mark in the PropertyManager to fully import the dimensions and exit the command. But since you need to select more features, you will keep the PropertyManager open so you can continue importing dimensions. However, you can take this opportu- nity to rearrange the dimensions before the view becomes too busy with the other features. Rearrange the dimensions by clicking and holding the left mouse button while dragging the dimensions into a better position. 8. As you arrange the dimensions already imported into the view, you may find it impossible to arrange the dimensions to avoid crossing over the view label, Section A-A. Rather than spend too much time with the dimensions, you can move the label a little lower in the view. Just like with dimensions, to arrange a label, click and hold the left mouse but- ton while you drag the label to a better position. After you are done, the view should look something like what is shown in Figure 4.16. F I g u r e 4 . 1 6 Arranging imported dimensions in the drawing view 9. Before exiting the Model Item PropertyManager, you need to import one more feature at this time. Click the bottom line of the section view to import the annotations for the width and the height of the base, as shown in Figure 4.17. Notice that not only are dimensions imported into the section view for the base, but there is also a dimension added to the top view. This is because the Import Items Into All Views option
Annotate the Drawing 167 was previously selected. The dimension added to the top view cannot be shown in the section view, so the most logical place for the dimension was automatically selected. F I g u r e 4 . 1 7 Importing dimensions for the base feature of the part 10. Click the green check mark in the Model Items PropertyManager to exit the command. Move Dimensions Between Views After importing the annotations from the part model into the drawing views, it is often necessary to clean up the dimensions. Since the annotations and dimen- sions that are inserted are based on the location in the sketches and features of the parts, they do not always translate well to the drawing space. Because of this, you will need to rearrange the dimensions and annotations on the drawing by distributing them throughout all the views and arranging them neatly. To dem- onstrate this, you will be moving one of the dimensions for the base of the part into another view that is a little more fitting. Sometimes dimensions are imported into views that do not show the feature being defined by the dimension. As you look through the dimensions that were imported, you will see a dimension that is not attached to any feature. This dimen- sion will need to be moved to the view that actually contains the feature. The fol- lowing steps allow you to do this and still maintain the link to the part models: 1. Zoom and pan until you can see Section A-A and the Right view as clearly as possible by spinning the scroll wheel to zoom and pressing and holding the wheel while moving the mouse to pan. 2. Move the mouse pointer on top of the vertical 1.500 dimension in Section A-A. When the dimension turns orange, click and hold the left mouse button and hold down the Shift button on the keyboard.
168 C h a p t e r 4 • C r e a t i n g Yo u r F i r s t D r a w i n g 3. While still holding the left mouse button and Shift on the keyboard, drag the 1.500 dimension to the Right view, as shown in Figure 4.18. F I g u r e 4 . 1 8 Moving an imported dimension to another view t I p You can also copy dimensions to other drawing views by holding the Ctrl button on the keyboard while dragging instead of holding the Shift button. 4. It is safe to release the left mouse button once the mouse pointer icon changes from a red circle with a line going through it to a blue dimen- sion icon. Once you release the left mouse button, the dimension will be moved to the view. Arrange Dimensions After moving dimensions to their appropriate drawing views, you can arrange them in the views to eliminate dimensions that are crossing or are inside the visible lines of the part. Also, in the case of the 1.500 dimension that was moved from the sec- tion view into the Front view, sometimes the extension lines may be shown on the wrong side of the part and should be fixed. Not only is this for aesthetic purposes, but it also ensures that the reader of the print will be able to interpret the drawing correctly.