The third level in the Oxford Practice Grammar Series. Grammar structures are explained in depth with practice activities that stretch your language skills.
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SECRETARIES
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SolidWorks® 2012
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Advanced Part Modeling
Dassault Systèmes SolidWorks Corporation 175 Wyman Street Waltham, Massachusetts 02451 USA
The information and the software discussed in this document are subject to change without notice and are not commitments by Dassault Systèmes SolidWorks Corporation (DS SolidWorks). No material may be reproduced or transmitted in any form or by any means, electronically or manually, for any purpose without the express written permission of DS SolidWorks. The software discussed in this document is furnished under a license and may be used or copied only in accordance with the terms of the license. All warranties given by DS SolidWorks as to the software and documentation are set forth in the license agreement, and nothing stated in, or implied by, this document or its contents shall be considered or deemed a modification or amendment of any terms, including warranties, in the license agreement.
In the event that you receive a request from any agency of the U.S. government to provide Software with rights beyond those set forth above, you will notify DS SolidWorks of the scope of the request and DS SolidWorks will have five (5) business days to, in its sole discretion, accept or reject such request. Contractor/Manufacturer: Dassault Systèmes SolidWorks Corporation, 175 Wyman Street, Waltham, Massachusetts 02451 US.
SolidWorks® 3D mechanical CAD software is protected by U.S. Patents 5,815,154; 6,219,049; 6,219,055; 6,611,725; 6,844,877; 6,898,560; 6,906,712; 7,079,990; 7,477,262; 7,558,705; 7,571,079; 7,590,497; 7,643,027; 7,672,822; 7,688,318; 7,694,238; 7,853,940 and foreign patents, (e.g., EP 1,116,190 and JP 3,517,643).
eDrawings® software is protected by U.S. Patent 7,184,044; U.S. Patent 7,502,027; and Canadian Patent 2,318,706. U.S. and foreign patents pending.
Trademarks and Product Names for SolidWorks Products and Services SolidWorks, 3D PartStream.NET, 3D ContentCentral, eDrawings, and the eDrawings logo are registered trademarks and FeatureManager is a jointly owned registered trademark of DS SolidWorks. CircuitWorks, FloXpress, TolAnalyst, and XchangeWorks are trademarks of DS SolidWorks. FeatureWorks is a registered trademark of Geometric Ltd. SolidWorks 2012, SolidWorks Enterprise PDM, SolidWorks Workgroup PDM, SolidWorks Simulation, SolidWorks Flow Simulation, eDrawings Professional, and SolidWorks Sustainability are product names of DS SolidWorks. Other brand or product names are trademarks or registered trademarks of their respective holders.
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COMMERCIAL COMPUTER SOFTWARE — PROPRIETARY The Software is a “commercial item” as that term is defined at 48 C.F.R. 2.101 (OCT 1995), consisting of “commercial computer software” and “commercial software documentation” as such terms are used in 48 C.F.R. 12.212 (SEPT 1995) and is provided to the U.S. Government (a) for acquisition by or on behalf of civilian agencies, consistent with the policy set forth in 48 C.F.R. 12.212; or (b) for acquisition by or on behalf of units 3 of the department of Defense, consistent with the policies set forth in 48 C.F.R. 227.7202-1 (JUN 1995) and 227.7202-4 (JUN 1995).
The goal of this course is to teach you how to build multibody and complex shape solid models using SolidWorks mechanical design automation software. Most of the case studies and exercises in this course are taken from industrial type applications, and the lessons primarily center around working with solids. Surfacing functions are covered in depth in the Surface Modeling course.
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About This Course
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The tools for modeling complex shapes in the SolidWorks software are quite robust and feature rich. During this course, we will cover many of the commands and options in great detail. However, it is impractical to cover every minute detail and still have the course be a reasonable length. Therefore, the focus of this course is on the fundamental skills, tools, and concepts central to successfully building multibody and complex shape solid models. You should view the training course manual as a supplement to, not a replacement for, the system documentation and on-line help. Once you have developed a good foundation in the skills covered in this course, you can refer to the online help for information on less frequently used command options.
Prerequisites
Students attending this course are expected to have the following:
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Mechanical design experience. Completed the course SolidWorks Essentials. Experience with the Windows™ operating system.
This course is designed around a process-based (or task-based) approach to training. Rather than focus on individual features and functions, a process-based training course emphasizes the processes and procedures you follow to complete a particular task. By utilizing case studies to illustrate these processes, you learn the necessary commands, options and menus in the context of completing a design task.
Course Length
The recommended minimum length of this course is two days.
Using this Book
This training manual is intended to be used in a classroom environment under the guidance of an experienced SolidWorks instructor. It is not intended to be a self-paced tutorial. The examples and case studies are designed to be demonstrated “live” by the instructor.
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Course Design Philosophy
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Laboratory Exercises
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Laboratory exercises give you the opportunity to apply and practice the material covered during the lecture/demonstration portion of the course. They are designed to represent typical design and modeling situations while being modest enough to be completed during class time. You should note that many students work at different paces. Therefore, we have included more lab exercises than you can reasonably expect to complete during the course. This ensures that even the fastest student will not run out of exercises.
SolidWorks 2012
Introduction
The drawings and dimensions given in the lab exercises are not intended to reflect any particular drafting standard. In fact, sometimes dimensions are given in a fashion that would never be considered acceptable in industry. The reason for this is the labs are designed to encourage you to apply the information covered in class and to employ and reinforce certain techniques in modeling. As a result, the drawings and dimensions in the exercises are done in a way that compliments this objective.
About the Training Files
A complete set of the various files used throughout this course can be downloaded from the SolidWorks website, www.solidworks.com. Click on the link for Support, then Training, then Training Files, then SolidWorks Training Files. Select the link for the desired file set. There may be more than one version of each file set available.
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Direct URL:
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A Note About Dimensions
www.solidworks.com/trainingfilessolidworks
The files are supplied in signed, self-extracting executable packages.
The files are organized by lesson number. The Case Study folder within each lesson contains the files your instructor uses while presenting the lessons. The Exercises folder contains any files that are required for doing the laboratory exercises.
Conventions Used in this Book
This manual uses the following typographic conventions: Convention
SolidWorks commands and options appear in this style. For example, Features > Extruded means click the Extruded Cut icon on Cut the Features tab of the CommandManager.
Typewriter
Feature names and file names appear in this style. For example, Sketch1.
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Bold Sans Serif
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Windows® 7
Meaning
Double lines precede and follow sections of the procedures. This provides separation between the steps of the procedure and large blocks of explanatory text. The steps themselves are numbered in sans serif bold.
The screen shots in this manual were made using the SolidWorks software running on Windows® 7.
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SolidWorks 2012
Use of Color
The SolidWorks software user interface makes extensive use of color to highlight selected geometry and to provide you with visual feedback. This greatly increases the intuitiveness and ease of use of the SolidWorks software. To take maximum advantage of this, the training manuals are printed in full color.
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Introduction
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Also, in many cases, we have used additional color in the illustrations to communicate concepts, identify features, and otherwise convey important information. For example, we might show the result of an operation in a different color, even though by default, the SolidWorks software would not display the results in that way.
Graphics and Graphics Cards
The SolidWorks software sets a new standard with best-in-class graphics. The combination of a highly reflective material and the realism of RealView Graphics is an effective tool for evaluating the quality of advanced part models and surfaces. RealView Graphics is hardware (graphics card) support of advanced
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shading in real time. For example, if you rotate a part, it retains its rendered appearance throughout the rotation.
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SolidWorks 2012
Color Schemes
Introduction
Out of the box, the SolidWorks software provides several predefined color schemes that control, among other things, the colors used for highlighted items, selected items, sketch relation symbols, and shaded previews of features.
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We have not used the same color scheme for every case study and exercise because some colors are more visible and clear than others when used with different colored parts.
In addition, we have changed the viewport background to plain white so that the illustrations reproduce better on white paper.
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As a result, because the color settings on your computer may be different than the ones used by the authors of this book, the images you see on your screen may not exactly match those in the book.
Hide/Show Tree Items
Certain items in the top of the FeatureManager design tree are automatically hidden if they are not used. For this course it is helpful to have some of these folders always shown. Click Tools, Options, System Options, FeatureManager. Under Hide/show tree items, set the following to Show:
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Surface Bodies folder Solid Bodies folder
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Introduction
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SolidWorks 2012
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Lesson 1 Sketching with Splines
Upon successful completion of this lesson, you will be able to: Sketch with splines.
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Insert a sketch picture.
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Manipulate spline curvature using the spline handles.
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Lesson 1
SolidWorks 2012
Sketching with Splines
Sketching Splines
A spline is a sketch element that interpolates its shape between points. Splines are very useful for modeling free-form shapes that are smooth and fair. [Fair is a term often used in boat building. A “fair curve” is one that is as smooth as it can be as it follows the path it must take around the hull of a boat; it is free of extraneous bumps or hollows.]
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Sketching with lines and arcs is fine for certain types of geometry, but lines and arcs are not appropriate for smooth, blended shapes. Since splines have continuously changing curvature, they cannot be duplicated using lines and arcs. Splines are used to sketch curves that have continuously changing curvature. Splines are defined by a series points between which the SolidWorks software uses equations to interpolate the curve geometry. You can modify a spline by adding or deleting points, moving the points, dimensioning the points, changing tangency or tangency weighting at the points or adding geometric relations. The spline can also be changed by modifying the spline handles (arrows) that control the tangency of the curve at the interpolant points or endpoints.
A spline in the SolidWorks software has several components and controls. Understanding what controls and analytical tools are available will help you get the most out of your splines.
Endpoints
Every spline has at least one endpoint. A closed loop spline has a single endpoint where the ends are tangent to one another. Open loop splines have two endpoints. An open loop spline can be converted to a closed loop spline by dragging one endpoint onto another, but a closed loop spline cannot be made open except by trimming.
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Spline Handle Endpoint
Spline Point
Control Polygon Closed Loop Spline
SolidWorks 2012
Lesson 1 Sketching with Splines I
Spline points
Most splines use one or more interpolant spline points between the endpoints. Spline points can be added (through the shortcut menu) or deleted. I
Spline handles
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Spline handles are used to change the direction and magnitude of the tangency at a spline point or endpoint. Unless a handle is being used to create tangency other than the default settings, they are not visible unless the spline is selected. Spline handles at interior spline points can be dragged asymmetrically (handles on opposite sides of the point are independent), or by holding the Alt key, the handles will behave symmetrically.
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Spline handles are composed of magnitude and direction handles. The magnitude handle can be dragged in a direction tangent to the spline, and the direction handle can be dragged in a circle around the point to which it is attached. By dragging the dot at the end of the magnitude handle, you can control both magnitude and direction at the same time. Notice that the cursor changes to indicate which control it is over.
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Direction Handle Magnitude Handle
Combination Handle
Control polygon
The control polygon is the series of dotted lines that go around the spline. It can be used in place of handles. To manipulate the control polygon, drag the control points.
Note
Moving the control polygon will move spline points but not reparameterize the curve. Moving the spline handles does not move the interpolant points but will reparameterize the spline.
Evaluating Splines
Right-click a spline and use the shortcut menu to display graphics that will help you evaluate its shape.
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Curvature comb
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The curvature comb displays graphically the curvature of the spline at that point. Mathematically, curvature is equal to the inverse of the radius (c=1/r), so the larger the curvature, the smaller the radius. This is why curvature combs are longest at sharp bends in a spline.
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Curvature Comb Inflection Point
Minimum Radius
Inflection points
Spline curvature can also change in direction. A curve that is convex in one area can be concave in a different area. Through the right mouse button menu, markers can be applied to the spline to show where the inflection changes.
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Lesson 1
SolidWorks 2012
Sketching with Splines I
Minimum radius
In several features such as fillets, offset, shell and thicken, an area of small radius can cause the feature to fail. For this reason, it is important when you create a spline to know its minimum radius. Sketching with Splines I
Smoothest curves — less is more
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Here are some general guidelines you may find useful for working with splines:
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Use as few spline points as possible to give the smoothest curve. Using many spline points is usually only viable if they are generated by a program or by Excel. Manually tweaking points that are closely spaced can lead to lumpy or uneven splines.
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Point density
You will need more spline points in areas of higher curvature (smaller radius). A long curving area will need relatively fewer points than a tightly curved section. All internal spline points are in this tightly curved area
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Control polygon
You can often get better control of the shape of a spline using the control polygon (dotted lines with handles around the spline) in conjunction with the tangency direction and magnitude handles. Two-point splines
You can create twopoint splines. A twoTwo-point point spline is just a spline with straight line until tangency tangency is applied to the ends, in which case Lines it becomes a very Two-point useful and flexible Spline sketch tool, particularly useful in situations where a sweep profile must change convexity, which an arc cannot do. Notice that this is much smoother than using a pair of tangent arcs.
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SolidWorks 2012
Lesson 1 Sketching with Splines I
The polygon controls the shape of the spline
But it is the spline points and the handles together that control the shape of the polygon. You need a minimum of two points (the endpoints). That will give you a spline that looks just like a straight line.
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To make a curved spline, you need three controls, either three points, or two endpoints and a handle. Three controls gives you a polygon with two sides (three vertices). To make an S-shape, the polygon must cross the spline. That requires a minimum of a 3-sided polygon. That means you need four controls.
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To make a W- or M-shape, you need five controls; some combination of interpolant points and handles. The table below shows three splines that are geometrically identical; their polygons are identical. In each case, the sum of the number of points and the number of handles being used are equal. Number of Controls
Resulting Spline
Number of spline points = 4 Number of handles in use = 0 Total number of polygon control points = 4 (three sides)
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Number of spline points = 3 Number of handles in use = 1 Total number of polygon control points = 4 (three sides)
Number of spline points = 2 Number of handles in use = 2 Total number of polygon control points = 4 (three sides)
Which should you use? None of these is better than the others. Your choice depends on design intent, the modeling situation, and ease of use. See Using relations on page 12.
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Lesson 1
SolidWorks 2012
Sketching with Splines I
Where you put the points matters
When sketching splines, place initial points near the min/max of the humps (bottoms of valleys, peaks of hills). Then adjust their positions. Refine the shape by dragging the points, the vertices of the control polygon, and the handles. I
Using relations
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One advantage of the spline handles over the polygon is you can add relations and dimensions to the handles. You cannot do that with the polygon vertices.
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There is another consideration regarding spline handles, relations, and the complexity of the polygon, and hence the mathematics of the curve: splines are rarely used in isolation; they usually have something like tangent relations applied to their ends. If you create the four-point spline shown in the table on the previous page, then add tangent relations to the ends, you will create two additional controls (the two handles) which will increase the complexity of the polygon and thus the mathematics of the curve. In this situation, a better choice would be to start with fewer spline points, add the tangent relations to the ends, and then manipulate the resulting spline handles to achieve the desired shape.
Keep it simple
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Just because you can drag the spline handles doesn’t mean you should. The spline shown at the right is the same shape as the ones in the table on the previous page. However, notice how much more complex its polygon is. That is because all of the spline handles were used, and putting a handle into use increases the number of polygon sides.
SolidWorks 2012
Lesson 1 Sketching with Splines I
Equal curvature
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For the smoothest connections between entities, splines support a sketch relation called Equal Curvature. This means the spline will start from the other entity with a matching curvature rather than making an abrupt jump. This is most important when combining splines with sketch elements other than straight lines. Here notice the difference in the curvature combs between tangency and equal curvature elements. Equal Curvature
Tangency
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Show entity points
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Splines are easier to work with when the setting to show sketch points is turned on. This is setting found under Tools, Options, System Options, Sketch, Display entity points in part/assembly sketches. If this option is cleared, you must select the spline in order to see endpoints or spline points.
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Proportional splines
Proportional splines retain their shape when you drag an endpoint; the entire spline resizes proportionally. To make a spline into a proportional spline, select the spline and click the Proportional option in the PropertyManager. To apply this, there must be no external relations on the spline or spline points. However, after you make the spline proportional, you can add relations to it. Symmetrical splines
There are three ways to work with symmetrical splines. 1. One way is to sketch a spline and mirror it. This is the easiest way, but because it creates two separate splines, geometry created from the mirrored spline will have edges on the model face corresponding to the endpoints of the splines. 2. The second method is more involved, but gives better results. It involves building a set of horizontal or vertical construction lines, and making them symmetric about another construction line corresponding to the line of symmetry. This can be very time intensive for complex splines. 3. A third method which combines the benefits of the previous two is to use the first technique with the mirrored spline, and then use Fit Spline to combine the two into a single spline. As usual with Fit Spline, make sure that the final spline matches the shape closely enough for your needs.
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Lesson 1
SolidWorks 2012
Sketching with Splines I
Fully defined sketches
It is common practice to leave splines under defined. Fully defined splines require two dimensions or fixed sketch relations for each spline point. Making changes becomes far more difficult. If you must fully define the spline, use the Fully Define Sketch tool to automatically add dimensions to under defined points.
Sketch Picture
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A Sketch Picture is a picture which has been inserted into a 2D sketch. Sketch pictures are often used for reference to trace around when modeling a part. Sketch pictures can be set up in multiple planes, simulating drawing views in the 3D model.
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When choosing a picture to use as a sketch picture, it is best to select high resolution, high contrast images. Tracing over a crisp edge is easier than a fuzzy edge. The ideal image would be a black and white (no colors or gray scale) line drawing.
Sketch pictures can be hidden in two different ways. First, you can hide the sketch the picture is in. Second, you can suppress the image independently of the sketch itself.
Introducing: Sketch Picture
An image file of the format .bmp, .gif, .jpg, .jpeg, .tif, or .wmf can be inserted into a sketch as a sketch picture. (Certain types of compression may cause tif or gif images to be unusable by SolidWorks.) The image can be seen from both sides, but cannot be seen through solid geometry. Transparency can be set for the image background. The image can be resized or moved by dragging or via the PropertyManager. Images can also be mirrored or rotated.
Where to Find It
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Menu: Tools, Sketch Tools, Sketch Picture
The best way to learn how to sketch with splines is to trace something.
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New part.
Open a new part using the Part_MM template.
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New sketch.
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Open a new sketch on the Front reference plane.
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Name the sketch Picture.
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SolidWorks 2012
Lesson 1 Sketching with Splines
3
Sketch picture. Click Sketch Picture.
In the Case Study folder for this lesson select the file Fleur-de-lis.jpg and click Open.
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Resize the picture.
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Make sure Lock aspect ratio is checked and scale the image by setting the Height to 200mm.
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The picture comes in with its (0, 0) coordinate at the sketch origin and an initial size of 1 pixel per 1mm, and locked aspect ratio. Since this is a high resolution image, the picture comes in very large. Note that the Width is over 1400 millimeters.
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Lesson 1
SolidWorks 2012
Sketching with Splines
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Position the picture.
To take advantage of the symmetry of the picture we want to center the picture on the origin.
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Click OK.
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Set the Origin X Position to -90.625mm and the Origin Y Position to -100mm.
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Centerline.
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Sketch a vertical centerline through the origin.
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SolidWorks 2012
Lesson 1 Sketching with Splines
7
Check the alignment of the picture.
The image is a bit too far to the right of the centerline. We cannot to move the centerline since it passes through the origin. Therefore, we have to tweak the position of the picture. 8
Move the picture.
Double-click the picture to open the Sketch Picture PropertyManager.
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Change the Origin X Position to -91.125mm.
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Zoom in on where the centerline intersects the tip of the image.
Click OK. Exit the sketch.
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New sketch.
Open a new sketch on the Front reference plane.
You can sketch the splines in the same sketch as the picture, but best practice is to use a separate sketch.
10 Sketch a spline. Click Spline .
Sketch a spline over the first portion of the image. Make sure that the end of the spline is coincident with the centerline.
Use as few controls as possible. Four points, three points and a handle, or two points and two handles are sufficient for this shape. We will use three points and a handle.
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11 Adjust the spline.
Adjust the polygon and the spline handle to make the spline conform to the image.
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Tips
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Zoom in as necessary to get a good view of the spline and the image. You may have to move the middle spline point. Drag the combination handle to change both the direction and the length of the tangent at the same time.
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Lesson 1
SolidWorks 2012
Sketching with Splines
12 Continue sketching splines.
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Sketch additional splines, one for each segment of the image. Most of the segments can be sketched with two-point splines.
13 Last segment.
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Before sketching the last segment, sketch a horizontal centerline coincident to the vertical centerline. After you sketch the two-point spline, add a Tangent relation between the spline and the horizontal centerline. This ensures that the spline will be tangent to its copy when you mirror it.
14 Copy the centerline. Use Convert Entities to copy the vertical centerline from the Sketch Picture sketch into the active sketch. This is the mirror axis.
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SolidWorks 2012
Lesson 1 Sketching with Splines
15 Mirror. Use Select Chain to select the splines.
Click Mirror Entities and use the vertical centerline as the mirror axis to mirror the splines. .
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Right-click the Sketch Picture sketch and click Hide
16 Exit, save, and close.
Exit the sketch.
Hide the Sketch Picture sketch.
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Save and close the part.
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Review
The following table summarizes and reviews the steps and techniques to follow when sketching splines. It is illustrated using the example of an acoustic guitar body.
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Lesson 1
SolidWorks 2012
Sketching with Splines
2. Place the spline points at the “hills and valleys” of the curve, that is, at the locations of convex and concave curvature.
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3. Add any necessary tangency conditions to the ends of the curve. In this case we added Vertical relations to the two end handles.
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1. Use as simple a spline as possible. This usually means keeping the number of interpolant spline points to a minimum.
4. Fine tune the positions of the spline points by dragging the points themselves, or dragging the polygon vertices. If you can get the shape you need this way, great. Otherwise, you will need to adjust the spline handles.
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5. Orient the angle of the spline handles so the tangency flows around the curve properly. As you do this, you may need to refine the positions of the spline’s interpolant points.
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6. If necessary, adjust the length or magnitude of the spline handles. When adjusting the length, first adjust them symmetrically by holding the Alt key as you drag. Then, if necessary, adjust them asymmetrically. 7. Repeat steps 4 through 6 as necessary to achieve the shape you desire.
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SolidWorks 2012
Exercise 1 Spline Practice
Exercise 1: Spline Practice
In this exercise you will use splines to trace a sketch pictures of the four playing card suit symbols: spades, hearts, diamonds, and clubs. I I
Sketching Splines on page 8. Sketch Picture on page 14.
Units: millimeters Procedure
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This lab reinforces the following skills:
Open a new part using the Part_MM template. 1
New sketch.
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Open a new sketch on the Front reference plane. Name the sketch Picture.
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Sketch picture.
Click Sketch Picture.
Browse to the Exercises folder of this lesson. Select the file Card Suit Symbols.bmp and click Open.
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Scale and position.
Make sure Lock aspect ratio is checked.
Scale and position the image as desired. You can use the PropertyManager or you can drag and resize the image in the graphics window.
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Exit the picture sketch and open a new sketch.
Open a new sketch on the Front reference plane.
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Trace.
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Trace the sketch picture using splines and other sketch entities as necessary. Take advantage of symmetry by mirroring where appropriate.
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Exit, save, and close.
Exit the sketch. Hide the Picture sketch. Save and close the part.
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Exercise 2
SolidWorks 2012
Fun with Splines
Exercise 2: Fun with Splines
In this exercise you will use splines to trace a sketch picture of your choosing. This lab reinforces the following skills: I I
Sketching Splines on page 8. Sketch Picture on page 14.
Open a new part using the Part_MM template.
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Procedure
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Units: millimeters
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New sketch.
Open a new sketch on the Front reference plane. Name the sketch Picture.
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Sketch picture. Click Sketch Picture.
Browse to the Zodiac Signs folder in the Exercises folder of this lesson. Select one of the 12 zodiac symbols and click Open.
Taurus
Gemini
Cancer
April 20-May 20
May 21-June 21
June 22-July 22
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Aries
March 21-April 19
Virgo
Libra
Scorpio
August 23-September 22
September 23-October 23
October 23-November 21
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Leo
July 23-August 22
Sagittarius
Capricorn
Aquarius
Pisces
November 22-December 21
December 22-January 19
January 20-February 18
February 19-March 20
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SolidWorks 2012
Exercise 2 Fun with Splines
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Transparency.
All of the images have a black background. Make the background transparent. In the Sketch Picture PropertyManager, under Transparency, click User defined. , sample the black background.
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With the eyedropper cursor
Set Matching tolerance to 0.00 and Transparency to 1.00. 4
Scale and position.
Make sure Lock aspect ratio is checked.
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Scale and position the image as desired. You can use the PropertyManager or you can drag and resize the image in the graphics window.
If the image has symmetrical elements in it, Gemini for example, you should sketch a centerline through the origin and use that as an aid in sizing and positioning the image. With an arbitrary shape like such as Virgo, there is no compelling reason to position the image in any particular spot relative to the origin.
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Exit the picture sketch and open a new sketch. Open a new sketch on the Front reference plane. Trace.
Trace the sketch picture using splines and other sketch entities as necessary.
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Exit, save, and close.
Exit the sketch.
Hide the Picture sketch.
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Save and close the part.
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Exercise 2
SolidWorks 2012
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Fun with Splines
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Lesson 2 Multibody Solids: How They Work
Upon successful completion of this lesson, you will be able to: Create multibody solids using a variety of techniques.
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Pattern solid bodies.
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Combine solid bodies.
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Modify a multibody cut using feature scope.
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Lesson 2
SolidWorks 2012
Multibody Solids: How They Work
Multibody solids occur when there is more than one continuous solid in a single part file. Often times, multibody techniques are useful for designing parts that require specific distance separation of features. These bodies can be accessed and modified separately and later merged into a single solid.
Creating a Multibody
Multibody solids are created in several ways. The following commands have the option of creating multiple solid bodies from a single feature: I I I I I
Extruded bosses and cuts (including thin features) Revolved bosses and cuts (including thin features) Swept bosses and cuts (including thin features) Lofted cuts Thickened cuts Cavities
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I
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Multibody Solids
Merge Result
The most direct way to create a multibody solid is by clearing the Merge result check box for specific boss and cut features.
Do
No
However, this option does not appear for the first feature.
26
SolidWorks 2012
Lesson 2 Multibody Solids: How They Work
Multibody Techniques
In this case study we will examine several different techniques of working in a multibody environment. 1
New part.
Create a semi cylinder as the first feature using the Right reference plane as the sketch plane.
2
Create a multibody.
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Create a cylinder as shown, also on the Right reference plane.
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Open a new part using the Part_MM template.
When boss features are created without intersecting the first feature, they are saved as multiple bodies. The Merge result check box remains checked by default, and the bodies will merge if they intersect as a result of a later change.
Note
R
Introducing: Solid Bodies Folder
The Solid Bodies folder holds all solid bodies in the part. Each solid body may be hidden from the folder. The names are taken from the last feature added to that body.
Where to Find It
FeatureManager design tree: Expand the Solid Bodies folder.
No
I
Do
3
Note
Explore the Solid Bodies folder.
The second cylinder causes the creation of another solid body. In the FeatureManager, expand the Solid Bodies folder to view these features. If the part contains one solid, the folder will contain a single feature.
27
Lesson 2
SolidWorks 2012
Multibody Solids: How They Work
4
Create a third solid body. Open a new sketch on the Front reference
plane and sketch a parallelogram as shown.
Tip
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Clear the Merge result check box.
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Extrude the sketch as a boss using the end condition Through All in both directions.
The color scheme is defined so the edges of solid bodies are black. Notice there are no edges displayed where the third body intersects the other two. This is a visual clue that the bodies are not merged.
5
Sketch.
Create the sketch as shown on the Right reference plane.
The body created in step 4 has been hidden for illustration purposes.
Do
No
Note
28
SolidWorks 2012
Lesson 2 Multibody Solids: How They Work
6
Through All cut. Click Extruded Cut
.
Reverse the direction and set the end condition to Through All. 7
Click Detailed Preview . Under Options, click Show only new or modified bodies.
Clear the Highlight new or modified faces check box.
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Click Flip side to cut.
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Examine the preview. It shows that the feature will cut the third body to the correct shape, but it will also cut the first two bodies. Do not click OK yet.
8
Feature Scope
Turn off Detailed Preview.
The Feature Scope allows you to select which bodies are affected by a feature. The Feature Scope option exists in the following tools: I I I I I I
9
Extrude Revolve Sweep Loft Cut with Surface Thicken
Set the feature scope.
Expand the Feature Scope group box.
Do
No
Clear the Auto-select check box.
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Lesson 2
SolidWorks 2012
Multibody Solids: How They Work
10 Select body.
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Select the third body that was created in step 4 and click OK.
11 Results.
The cut feature only affects the selected body.
Notice that the cut feature did not merge the three bodies.
Each type of pattern feature can be used to create instances of solid bodies. The Bodies to Pattern field is used to identify which body or bodies will be patterned.
No
Patterning Bodies
The Bodies to Pattern field exists in the following pattern tools: I
Do
I
30
I I I I
Linear Circular Mirror Table Driven Sketch Driven Curve Driven
SolidWorks 2012
Lesson 2 Multibody Solids: How They Work
12 Mirror body. Insert a Mirror pattern using the Right reference plane.
Select Cut-Extrude1 as the Bodies to Mirror.
Note
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Keep Merge solids cleared. Click OK.
There is no point selecting Merge solids because that only merges the results of the mirror operation with the body being mirrored. Since the mirrored copy and its parent don’t touch each other, they cannot be merged. The other two bodies are not part of the mirror operation, thus they are not affected by it.
13 Create a bridge.
Create a sketch on the Front reference plane using the edges of the two angled bodies. Extrude the sketch 8mm using the Midplane end condition.
No
Click Merge result.
Do
The Solid Bodies folder now displays only one solid, Boss-Extrude4.
Merge Result
Features, such as fillets, using the edges formed by merged solid bodies, will fail if Merge result is unchecked in a later operation. The following rebuild error will appear: Fillet1: Multiple bodies not supported for this feature.
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Lesson 2
SolidWorks 2012
Multibody Solids: How They Work
The tool body technique is used to add or remove model volume using specialized “tool” parts.
Introducing: Insert Part
You can use the Insert Part command to add one or more solid bodies into the active part, placing the origin of the inserted part on that of the active part. The inserted parts are then oriented using the Locate Part dialog.
Entities to Transfer
When you insert a part you have the option of transferring with it any combination of the following:
I
Solid bodies Axes Cosmetic threads Unabsorbed sketches Coordinate systems Hole Wizard data
I
Menu: Insert, Part
I I I
I I I
Surface Bodies Planes Absorbed sketches Custom properties Model dimensions
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I
I
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Tool Body
I
Where to Find It
I
14 Insert a part. Click Insert, Part. Browse to the Case Study folder of this
lesson and select the part
Mounting Lug.
The part being inserted is simply a standard part file.
Under Transfer, select Solid bodies at a minimum.
For this example, also select Planes and Model dimensions.
No
Transferring other items is optional.
Do
Make sure Locate part with Move/Copy feature is checked.
32
Click in the graphics area to locate the part and click OK.
SolidWorks 2012
Lesson 2 Multibody Solids: How They Work
15 Results. The Locate Part PropertyManager appears and an instance of the Mounting Lug is added to the
active part.
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You can locate the part using mates (constraints), similar to the way components are mated in an assembly, or by specifying translation and/or rotation with respect to the X, Y, and Z axes.
Introducing: Move/Copy Bodies
Use Move/Copy Bodies to orient solid bodies within a part. Bodies can moved be using two different methods:
Note
No
1. Mates, similar to the way components are mated in an assembly 2. Specifying translation and/or rotation with respect to the X, Y, and Z axes.
Do
Where to Find It
The Locate Part PropertyManager is the same as the Move/Copy Bodies PropertyManager. I
Menu: Insert, Features, Move/Copy
This example illustrates using mates to locate the solid body. For an example using explicit translation, see Exercise 3: Soda Bottle on page 39. The Translate/Rotate and Constraints buttons toggle between the explicit translation and rotation method and the mate method respectively.
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Lesson 2
SolidWorks 2012
Multibody Solids: How They Work
16 Select the planes.
Select the Front PlaneMounting Tab and the Right reference plane of
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the host part.
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Verify that you are on the Mate Settings page of the PropertyManager.
17 Mate the body.
The system selects Coincident as the default mate type. In cases when this is not what you want, select a different type.
Do
No
Verify the orientation of the Mounting Lug. If it is incorrect, as in the picture above, change the Mate Alignment to match the picture below.
Click Add to apply the mate. For more information about mates, see the SolidWorks Essentials training manual.
34
SolidWorks 2012
Lesson 2 Multibody Solids: How They Work
18 Additional mate. Add a Coincident mate between the bottom faces of the Mounting Lug and
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the host part.
19 Additional mate. Add a Distance mate between the Front plane of the host part and the Right Plane-Mounting Lug.
Set the Distance to 38mm and click Add.
Click OK.
This completes positioning the lug.
20 Examine the feature. Expand the Mounting Lug
feature listing.
No
The reference planes are listed in the Planes folder.
Do
The feature representing the Locate Part command is listed as a child of the Mounting Lug.
Note
If you selected other items to transfer, such as axes or sketches, when you inserted the part (see Entities to Transfer on page 32), they would be in their own corresponding folders. 21 Explore the solid bodies.
A second solid body is listed in the folder.
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Lesson 2
SolidWorks 2012
Multibody Solids: How They Work
22 Mirror body. Insert a Mirror pattern using the Front
reference plane.
Keep Merge solids cleared.
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Click OK.
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Select Mounting Lug as the Bodies to Mirror.
Combining Bodies
The Combine command is used to combine the volumes of multiple solid bodies into a single body by adding, subtracting or intersecting.
Introducing: Combine
The Combine command has three options:
I
Add
The Add option uses the Bodies to Combine list to merge the bodies into a single solid by adding all volumes. This operation is also known as a union in other systems.
I
Subtract The Subtract option uses the Main Body and Bodies to Combine list
to merge the bodies into a single solid by subtracting the bodies to combine from the main body.
I
Common The Common option uses the Bodies to Combine list to merge the
bodies into a single solid by finding the volume that is common to all. This operation is also known as a intersection in other systems. Menu: Insert, Features, Combine
I
Tip
The Solid Bodies filter
No
Where to Find It
is useful when selecting solid bodies.
Do
23 Combine the solid bodies. Click Combine.
36
Use the Add option for Operation Type. Select all three bodies from the Solid Bodies folder for Bodies to Combine. Click OK.
SolidWorks 2012
Lesson 2 Multibody Solids: How They Work
Examples of Combined Solids
The following table displays the results from various combining techniques available. Add Body1
Body3 Body2
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Result
Subtract
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Body1
Result
Body2
Common - 2 Bodies Intersecting Body1
Result
Body2
Common - 3 Bodies Intersecting
No
Body2
Body1
Do
Result
Body3
37
Lesson 2
SolidWorks 2012
Multibody Solids: How They Work
24 Add features.
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Add holes and cuts.
25 Add fillets and rounds. Finish the part with 1.5mm radius fillets
and rounds.
Do
No
26 Save and close the part.
38
SolidWorks 2012
Exercise 3 Soda Bottle
Exercise 3: Soda Bottle
In this exercise you will model a 20oz. (591ml) soda bottle. Since these bottles are filled and handled by automated equipment, the bottom of the bottle and the neck are standard parts. Your task is to design the area in between. It is this portion of the bottle that gives it its look and feel, and establishes the branding for the soft drink company. Multibody Solids on page 26.
I
Insert Part on page 32.
I
Move/Copy Bodies on page 33.
I
Sketching with Splines on page 10.
I
Combining Bodies on page 36.
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This lab reinforces the following skills:
Units: inches or centimeters, your choice.
Procedure
Note
Decide whether you want to build the part using English or metric units. Then open a new part using the appropriate template and name it Soda Bottle. The illustrations in this exercise have the material PET, transparency of 0.2, and the color green applied.
1
Insert part.
Click Insert, Part.
Browse to the Exercises folder of this lesson and select the part Bottle Bottom.
This part was created from a neutral format file.
Under Transfer, select Solid bodies at a minimum.
Clear Locate part with Move/Copy feature.
No
Click OK.
2
Insert part.
Do
Browse to the Exercises folder of this lesson and select the part Bottle Neck.
Select Locate part with Move/Copy feature. Click OK.
39
Exercise 3
SolidWorks 2012
Soda Bottle
3
Locate part.
This part was built with the top of the neck at the origin.
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Click OK.
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When the Locate Part PropertyManager appears, translate the part 8.75” (22.2cm) in the positive Y direction.
4
Sketch.
Open a sketch on the Front plane.
Using a combination of splines and other sketch geometry, sketch the profile of the bottle. The shape is up to you. Be as conservative or outlandish as you wish.
You will need a centerline because this is going to be a revolved, thin feature.
Do
No
Pay attention to how the splines connect to the bottom and neck of the bottle. The ends should be coincident with both the face and the silhouette edge of the bodies. You may also want to apply tangency.
40
SolidWorks 2012
Exercise 3 Soda Bottle
5
Create a revolved thin boss feature. Set the Thickness to 0.012” (0.03cm) and verify
that the thickness is being applied to the inside of the bottle. Make sure Merge result is checked.
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Explore the Solid Bodies folder. There should be only one solid body in the folder. If there are more, check your sketch and the thin feature for errors.
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6
7
Check the volume.
Open a sketch on the Top reference plane and sketch a rectangle large enough to completely enclose the bottle. The exact dimensions do not matter. Extrude the rectangle as a boss.
Set the Distance to 7.5” (19.0cm).
Clear the Merge result check box.
Combine. Click Combine
No
8
.
Do
Use the Subtract option for Operation Type. Select the extruded boss for the Main Body and the bottle for the Bodies to Combine. Click OK.
41
Exercise 3
SolidWorks 2012
Soda Bottle
Bodies to keep.
Subtracting the bottle from the extruded block divides the block into two solid bodies. The system prompts you, asking which of the bodies you want to keep.
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Since you are interested in the volume of the bottle, keep that and discard the outside.
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9
10 Mass properties. Click Evaluate > Mass Properties
.
If you are working in English units, the volume should be 36 cubic inches. In metric units, the volume should be 591 cubic centimeters. If the volume is incorrect, edit the sketch of the revolved feature and adjust the shape of the spline.
11 Suppress.
When you are satisfied with the shape and the volume of the bottle, suppress the Boss-Extrude1 and Combine1 features.
Do
No
12 Save and close the part.
42
SolidWorks 2012
Exercise 4 Positioning Inserted Parts
Exercise 4: Positioning Inserted Parts
Create this part by following the steps as shown.
I
Insert Part on page 32.
I
Move/Copy Bodies on page 33.
Procedure
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Units: millimeters
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This lab reinforces the following skills:
1
Existing part.
Open the part named Base.
2
Insert part.
Insert the part Lug and position it as shown.
3
Second body.
Add another instance of the Lug.
You can repeat Insert, Part or make a copy of the existing instance of the Lug using Move/ Copy Body, whichever you prefer.
Do
No
Tip
43
Exercise 4
SolidWorks 2012
Positioning Inserted Parts
4
Continue.
5
Combine bodies and add fillets.
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Create two more copies of the Lug, positioned as shown.
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Combine all the solid bodies into one. Add 8mm and 2mm fillets as shown.
6
7
Modify sketch. Open the Lug part and change the 45mm dimension to 60mm.
Propagate change.
Do
No
Return to the main part.
8
44
Save and close the part.
SolidWorks 2012
Exercise 5 Copying Bodies
Exercise 5: Copying Bodies
Create this part by following the steps as shown.
I
Insert Part on page 32.
I
Move/Copy Bodies on page 33
I
Patterning Bodies on page 30.
Units: millimeters
Open a new part using the Part_MM template and name it Mbody4.
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Procedure
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This lab reinforces the following skills:
1
Insert parts.
Insert and position parts 1A, 1B, 2A and 2B as shown.
2
Add patterns.
Do
No
Pattern the solid bodies as shown.
45
Exercise 5
SolidWorks 2012
Copying Bodies
3
Connect bodies.
Pattern bridge with 3 instances.
4
Create plate.
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Create a bridge that connects the bodies without merging.
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Sketch on the Top reference plane to create the Plate feature.
Extrude the feature 6mm and click Merge result. Add fillets and rounds. Finish part with 3mm radius fillets and rounds.
Do
No
5
46
SolidWorks 2012
Exercise 5 Copying Bodies
6
Modify referenced part. Right-click the feature 2B and choose Edit in Context.
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Change the depth of the extrusion to 58mm.
7
Propagate change.
No
Return to the main part.
Save and close the part.
Do
8
47
Exercise 5
SolidWorks 2012
Do
No
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Copying Bodies
48
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Lesson 3 Uses of Multibody Solids
Upon successful completion of this lesson, you will be able to: Identify the different uses of a multibody solid.
I
Combine solid bodies with add, subtract and common.
I
Deform a solid body using the Indent feature.
I
Use various techniques to split a part into multiple bodies.
I
Save solid bodies as discrete part files.
I
Create an assembly from a multibody part.
Do
No
I
49
Lesson 3
SolidWorks 2012
Common Bodies
There are three ways to combine multiple bodies into a single solid body: Add, Subtract, and Common. Add and Subtract are fairly intuitive because they mimic manufacturing process such as welding and machining. The Common method, sometimes referred to as a Boolean intersection, is more abstract. This example uses Common to model a protective screen. 1
New part.
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Uses of Multibody Solids
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Open a new part using the Part_MM template. Save the part naming it Protective Screen.
2
Create a sketch.
Using the Front reference plane, sketch the profile shown. I I
I
I
Sketch a 3 point arc coincident to the two points and dimension it as shown.
Extend the ends of the arc beyond the sketch points.
Do
No
Tip
Sketch and dimension the centerline. Insert two sketch points and add Vertical relations between them and the ends of the centerline. Dimension the sketch points.
50
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
3
Revolved thin feature.
Since the sketch is open, you will be asked if you want to close it. Click No because you want to create a thin feature. Use Midplane with an Angle of 90°.
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Set the Thickness to 1.00mm and make sure the material is added to the outside of the sketch.
4
Sketch.
Open a new sketch on the Top reference plane.
Create the sketch shown at the right. Use mirroring to create the necessary symmetry.
Do
No
This sketch defines the outline of the screen.
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Lesson 3
SolidWorks 2012
Uses of Multibody Solids
5
Extrude.
Extrude the sketch using the end condition Through All.
Offset plane.
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6
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Clear the Merge result option.
Important!
Create a plane offset 1mm below the top face of the extruded body.
This plane will be used later, in step 9.
7
Shell.
Shell the extruded boss using a Thickness of 3mm.
Do
No
Remove the uppermost face.
8
Sketch.
Open a new sketch on the plane you created in step 6. Sketch a line for a rib as shown at the right.
52
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
9
Rib.
Click Rib
.
For Selected body, select the shelled body. Click OK.
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10 Linear pattern.
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Set the Rib Thickness to 1mm and click Normal to Sketch.
Pattern the rib using a Spacing of 12.75mm and Number of Instances = 14.
11 Second rib and linear pattern.
No
Select the uppermost face of the shelled body for the sketch plane. This is necessary because for the rib to extend across the ribs from the previous step, the sketch has to be above the upper face of the existing ribs.
Do
Create a second rib just like the first one, this time starting at the other corner.
53
Lesson 3
SolidWorks 2012
Uses of Multibody Solids
Use the Common option for Operation Type and select both bodies. Click OK.
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13 Save and close the part.
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12 Combine the solid bodies. Click Combine.
Indent Feature
The Indent feature is used to reshape thin walls of the Target Body to the shape of one or more intersecting Tool Bodies. The indentation thickness and optional clearance are controlled by numeric values. I
Target Body The Target Body is the body being indented.
I
Tool Body Region The Tool Body Region is a selection of both a solid body (tool)
and a region as the tool body is divided by the target body.
Menu: Insert, Features, Indent
I
Using Indent
In this example, Indent is used to reshape the protective screen we just built. The selection of the tool body region determines to which side of the target body the indent feature is applied.
No
Where to Find It
Do
1
54
Open the part Protective Screen - Indent. This is a copy of the previous part as it existed at step 13.
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
2
Rollback.
You will get a message indicating that the sketch will be unabsorbed. Click OK.
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Once Sketch2 is unabsorbed, position the rollback bar just below it.
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Expand the Boss-Extrude2 feature and drag the rollback bar so it is positioned between the feature and its sketch.
3
New sketch.
Open a new sketch on the Top reference plane. Show Sketch2.
Create an offset 2mm inside the contour of Sketch2.
The revolved thin feature is hidden for illustration purposes.
Note
4
Extrude.
Extrude the new sketch. Use Offset From Surface for the end condition. Set the Offset Distance to 1mm and make sure the offset is above the face of the revolved feature. Clear the Merge result option.
Do
No
Important!
55
Lesson 3
SolidWorks 2012
Uses of Multibody Solids
5
Fillet.
6
Indent.
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Click Indent.
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Apply a 0.5mm radius fillet to the four vertical edges of the extruded body.
Select the revolved feature as the Target body. Select the curved face of the extruded body as the Tool body region. Under Parameters, set the Thickness to 1mm and the Clearance to 0mm.
Click OK.
Important!
Click inside the uppermost face of the extruded body as shown.
7
Hide body.
Do
No
Hide the tool body to see the results.
56
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
8
Fillet.
Apply 0.5mm fillets to the concave edges of the indented region.
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Apply 1.5mm fillets to the convex edges as shown in the section view below.
9
Roll forward.
No
The system rebuilds the part incorporating the changes you’ve made.
Do
Introducing: Delete Body
Where to Find It
Delete Body or Delete Solid/Surface is used to delete a solid or surface body from the Solid Bodies or Surface Bodies folders but
keep the body available for calculations prior to that deletion. I I
Menu: Insert, Features, Delete Body Shortcut Menu: Right-click a body and click Delete Body
57
Lesson 3
SolidWorks 2012
Uses of Multibody Solids
10 Delete body. Expand the Solid Bodies folder, right-click the tool body (Fillet1), and click Delete Body.
Click OK.
11 Save and close the part.
Local Operations
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A Body-Delete1 feature is added to the feature tree and the Fillet1 body is removed from the Solid Bodies folder.
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The local operations technique is used to make specific modifications on one body without affecting another body. A common example of this technique is a variation on shelling. The shelling operation, by default, affects all features of the solid body that precede it. In this example, a shelling problem will be solved using Merge result and Combine.
1
2
Open the part Local Operations.
Shell part.
Add a 4mm shell that removes the bottom face.
3
Section view.
Do
No
Create a section view parallel to the Front reference plane, at an Offset Distance of -42mm.
58
Notice in the section view that the shell affects the entire part. We only want it to affect the bottom plate. Click OK to keep the section view active.
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
4
Modify feature. Use Edit Feature on these three
bosses: I I
Vertical_Plate Circular_Boss Rib_Under
Clear the Merge result check box for each boss and click OK. 5
Explore the solid bodies.
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I
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After clearing the Merge result check box for each boss, the model breaks into four solid bodies. Expand the Solid Bodies folder to view them.
Click on them to highlight in the graphics area.
6
Combine the solid bodies.
Click Combine.
Use the Add option for Operation Type.
Select all four bodies from the Solid Bodies folder for Bodies to Combine. Click OK.
7
Explore the single solid.
The part now exists as a single solid body Combine1.
Do
No
The name is assumed from the last feature added to the body.
Tip
8
Turn off the section view.
9
Save and close the part.
Features, such as fillets, that use the edges formed by merged solid bodies, will fail if Merge result is unchecked in a later operation. The following rebuild error will appear: Fillet1: Multiple bodies not supported for this feature.
59
Lesson 3
SolidWorks 2012
Using Local Operations to Solve Filleting Problems
Many times success in filleting depends on the order in which you apply the fillets. Multibody solids and local operations give you the ability to alter the sequence in which fillets are applied. This can be very helpful with particularly difficult filleting problems.
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Uses of Multibody Solids
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Thanks to Keith Pedersen at Computer-Aided Products, Inc. for submitting this example.
1
Open the part Fillet Problem.
2
Attempts at filleting.
Do
No
Various attempts to apply a 6mm fillet do not yield satisfactory results. This is because the fillets are affected by adjacent faces. The solution is to fillet the bodies separately.
60
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
3
Unmerge the solids. Right-click the Angled Piece feature and click Edit Feature.
Fillet the Angled Piece feature. Apply a 6mm fillet to the uppermost face of the Angled Piece.
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4
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Clear the Merge results check box and click OK.
5
Combine the solids.
Click Combine.
Merge the two solids using the Add option.
No
Click OK.
6
Fillet.
Do
Apply the remaining 6mm fillet as shown.
7
Save and close the part.
61
Lesson 3
SolidWorks 2012
Modeling Negative Space
Consider a part where the design and placement of holes, voids, and cavities, relative to each other and the origin, are of primary importance. One example of this is a hydraulic manifold. The working medium of this design is hydraulic fluid, not steel.
You could start with a block of steel and model all the passages as cut features. An alternative approach is to model the empty, or negative space, and subtract it from the main body.
The example that follows is a very simple one and because of that, it is somewhat unrealistic. However, it serves to illustrate the concept of modeling negative space.
1
Open the part Hydraulic Manifold.
The part contains multiple solid bodies representing interconnected cavities in the manifold.
2
Sketch a rectangle.
Do
No
Open a new sketch on the Top reference plane and sketch a rectangle whose four sides are colinear with the planar faces of the cavity bodies.
62
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
3
Extrude.
Extrude the rectangle in two directions. I
Direction 1 (up): Up To Surface Direction 2 (down): Blind; Depth = 30mm
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I
4
Combine the solid bodies.
Do
No
Using the extruded block as the Main Body and the remaining solid bodies as the Bodies to Subtract, combine with a Subtract operation.
Transparency has been applied to the extruded block for illustration purposes.
Note
5
Save and close the part.
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Lesson 3
SolidWorks 2012
Uses of Multibody Solids
Using Cut to Create Multibodies
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Certain cut features will split a part into multiple solid bodies. If this happens the Bodies to Keep dialog box appears. You can control how to split the part.
1
2
Open the part Cut into Bodies. Create multibodies.
Do
No
Using Sketch3, create a Through All cut with the All bodies option.
64
3
Explore the Solid Bodies folder. The cut feature creates two solid bodies.
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
You can save one or more of the solid bodies in a multibody part as separate part files. There are several commands to do this, each with different characteristics. Some commands give you the option to also generate an assembly from the saved parts.
Default Templates
The commands in this section create new SolidWorks documents – either a part or an assembly or both as appropriate. You have the option of specifying a document template or allowing the system to use the default template. This choice is determined by the settings in Tools, Options, System Options, Default Templates.
Introducing: Insert into New Part
Insert into New Part allows you to save individual solid bodies as part
files. Each resulting part file is linked by an external reference back to the source part. A Stock- feature appears in the saved part. This feature carries the external reference. For more information about external references, refer to the Assembly Modeling training course.
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Note
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Saving Solid Bodies as Parts and Assemblies
If you select multiple bodies or the Solid Bodies folder, the saved part will be a multibody part with a Stock feature for each body. Insert into New Part does not create a feature in the source part. The
solid bodies are saved as they are after the last part feature is rebuilt. Any changes you make to the source part will propagate to the saved parts.
Where to Find It
I
4
Shortcut Menu: Expand the Solid Bodies folder, right-click the body you want to save, and click Insert into New Part
Insert the solid bodies into new parts.
Expand the Solid Bodies folder. Use Insert into New Part to create the parts as shown below, one part for each body. The new parts are opened automatically.
Do
No
clamp top
clamp bottom 5
Create an assembly.
Open a new assembly. Add the saved parts. Name the assembly clamp_assy.
65
Lesson 3
SolidWorks 2012
Uses of Multibody Solids
6
Newly created part.
Make changes to the source part.
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7
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Switch to one of the newly created parts. Examine the FeatureManager. Note the Stock feature. This carries the external reference.
Switch back to the source part.
Sketch two 13mm circles on the planar face on the underside of the bottom half of the clamp as shown.
8
Through All cut.
Click Extruded Cut
.
Set the end condition to Through All.
9
Click Detailed Preview
.
Under Options, click Show only new or modified bodies. Clear the Highlight new or modified faces check box.
No
Examine the preview. It shows that the feature will cut through both bodies.
Do
Do not click OK yet.
66
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
10 Set the feature scope. Expand the Feature Scope group box.
Clear the Auto-select check box.
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Select the bottom half of the clamp and click OK.
11 Results.
The cut feature only affects the selected body.
No
12 Second Through All cut feature. Create another Through All cut feature as shown. Use the Feature Scope to limit its effect to just the
Do
upper half of the clamp.
67
Lesson 3
SolidWorks 2012
Uses of Multibody Solids
13 Examine the individual parts.
Introducing: Save Bodies
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14 Save and close the files.
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The changes made to the source part propagated to the saved files.
Save Bodies also allows you to save individual solid bodies as part
files. You can indicate which bodies you want to save. Optionally you can generate an assembly from the saved parts.
Save Bodies adds a Save Bodies feature in the FeatureManager of the
source part.
The bodies are saved at the point in the part history where the Save Bodies feature appears. Any subsequent features added to the source part will not propagate to the saved files. Each resulting part file is linked by an external reference back to the source part. A Stock- feature appears in each saved part. This features carries the external reference.
Where to Find It
I I
Menu: Insert, Features, Save Bodies Shortcut Menu: Right-click the Solid Bodies folder and click Save
Bodies
1
Open the part Boat Cleat.
No
There are two solid bodies representing the core and the pattern. One body is shown semi-transparent for illustration purposes.
Do
2
68
Edit appearance.
Right-click the topmost feature in the FeatureManager. Click Appearances
. Click Advanced. Click the Illumination tab.
Remove the transparency.
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
3
Saving the bodies. Click Save Bodies. The PropertyManager
appears. As you move the cursor over the model, the individual bodies highlight. Sometimes it is hard to tell which callout points to which body. Changing the view usually helps.
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Tip
4
Saving the bodies.
In the PropertyManager, under Resulting Parts, double-click the name field. The Save As dialog appears.
Save the bodies as Core and Pattern.
When you save the bodies you can specify an origin location. If you do not, the saved parts have the same origin as the source part.
Note
5
Resultant bodies state.
No
Clear the Consume cut bodies option. This will keep the solid bodies in the source part visible.
Creating an Assembly
If you want to create an assembly do the following:
Do
1. In the Create Assembly group box, click Browse. The Save As dialog opens. 2. Browse to where you want to save the assembly. 3. Give the assembly a name and click Save. In this example it is not necessary to save the assembly. If later you decide you need an assembly you can always create one from the saved parts using traditional bottom-up assembly modeling techniques.
6
Click OK.
The saved parts open.
69
Lesson 3
SolidWorks 2012
Uses of Multibody Solids
7
FeatureManager.
Examine the FeatureManager design tree of the source part. A Save Bodies feature has been added. This records the point in the part’s history when the bodies were saved. Changes made to the source part after this feature will not propagate to the saved parts. Make changes to the source part. Make sure the source part, Boat Cleat, is
active. Click Combine. Subtract the core from the pattern.
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8
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The results are shown in a section view for clarity. 9
Examine the Pattern part.
The change made to the source part did not propagate to the saved files.
Do
No
10 Save and close the files.
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SolidWorks 2012
Lesson 3 Uses of Multibody Solids
Sometimes it is easier to start a design as a single part. Then, after form, fit, and function are defined, the part is split into its individual components. This is particularly handy when aesthetics are important.
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Splitting a Part into Multibodies
Introducing: Split
Split allows you to break a part into multiple solid bodies using
splitting tools such as sketches, faces, planes, or surfaces.
No
The Split command creates a Split feature in the FeatureManager of the source part. This means the bodies are saved at the point in the part history where the Split feature appears. Any subsequent features added to the source part will not appear in the saved files. If you delete the Split feature in the original part, the new parts still exist, but the status of the external reference in the new parts is dangling.
Do
Where to Find It
I
Menu: Insert, Features, Split
71
Lesson 3
SolidWorks 2012
Uses of Multibody Solids
1 2
Open the part Handle. Split the part.
3
Trim tools.
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Select the Front reference plane as the trim tool.
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Click Split.
4
Cut the part. Click Cut Part. The
system computes the intersection of the trim tools with the part and calculates the results.
Do
No
As you move the cursor over the model, the individual bodies highlight. Click on the bodies you want to create.
72
In this case, click both resulting bodies. Click OK.
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
Saving the Bodies
5
Saving the bodies. Click Save Bodies.
In the graphics area select one of the bodies. A callout appears. Double-click the name field.
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The Save As dialog appears. Type in the name. Do this for both bodies.
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In the Split command you have the option to save the resulting bodies as individual part files. However, doing this within the Split command is not recommended because if you edit the split feature later, you will have to remap the saved bodies. It is a better practice to save the bodies as a separate operation using the Save Bodies command.
Name the bodies Handle Left Side and Handle - Right Side.
Note
When you save the bodies you can specify an origin location. If you do not, the saved parts have the same origin as the source part.
6
Resultant bodies state.
Clear the Consume cut bodies option. This will keep the solid bodies in the source part visible.
7
Click OK.
The new part files are created. Open them in their own windows. You would now finish modeling the details of each part.
Do
No
Note: View rotated for clarity.
73
Lesson 3
SolidWorks 2012
Uses of Multibody Solids
Once the solid bodies have been saved as part files, you can use them to create an assembly just as you would with any other parts. You can create an assembly manually using traditional bottom-up assembly modeling techniques, or you can automate the process.
Introducing: Create Assembly
Create Assembly collects the part files saved by one or more Save Bodies or Split features and creates a new assembly from them.
Where to Find It
I I
Shortcut Menu: Right-click the Save Bodies or Split feature and click Create Assembly Menu: Insert, Features, Create Assembly
Create Assembly. Switch to the Handle part.
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8
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Creating an Assembly
Click Create Assembly. The PropertyManager opens.
9
Click Browse.
The Save As dialog box appears.
Browse to the folder where you want to save the assembly, and type a name for the assembly in the File name box.
10 Click Save. The Save As dialog box closes and the file name appears under Assembly file in the PropertyManager. 11 Click OK.
The new assembly document opens.
There are no mates in this assembly. Both components are fixed with their origins at the assembly origin.
Note
No
12 Save and close the files.
Do
Summary
74
There is quite an assortment of tools and techniques for saving individual solid bodies as part files and for creating assemblies from multibody parts. All of the techniques create an external reference between the saved part file and the original source part. The various commands and techniques are summarized in the table on the following page.
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
Technique
Allows you to create new parts from the bodies in the Solid Bodies folder.
If you use Insert into New Part on the Solid Bodies folder instead of an individual body, you will create a multibody part that is linked back to the original part. Each body will be represented by its own Stock feature.
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Insert into New Part
Results
Insert into New Part does not add a feature in the FeatureManager of the source part. Therefore, any features you add to the bodies in the source part will propagate to the saved files. Also it is not possible to navigate to the child part from the source part.
Adds a Split feature in the FeatureManager of the source part.
Allows you to split a single solid body into multiple bodies.
The bodies are saved at the point in the part history where the Split feature appears. Any subsequent features added to the source part will not appear in the saved files. Any features added before the Split feature will propagate to the saved files. While you cannot directly access the saved files from the source part, editing the Split feature will give you their full path names.
Save Bodies
Adds a Save Bodies feature in the FeatureManager of the source part.
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Split Part
Like Split Part without the splitting tools. It takes existing bodies in the part and lets you write them out as parts. Create Assembly
Optionally you can generate an assembly from the saved parts.
This is a convenience tool that automates generating an assembly from a Split feature. You could do exactly the same thing by manually opening a new assembly and adding all the saved parts. Create Assembly does not add a feature in the FeatureManager of
the source part. Therefore, it is not parametric in the sense that if you create more solid bodies later, they do not automatically appear in the assembly.
No
Collects the part files saved by one or more Split features and creates a new assembly from them.
The bodies are saved at the point in the part history where the Save Bodies feature appears. Any subsequent features added to the source part will not appear in the saved files.
Insert, Part
Do
Inserts a part into the current part.
Adds a Stock feature to the current part. Insert, Part does not add any features to the parent or source part, but it will insert all bodies from the source. Often, a Delete Bodies feature is used after inserting multiple bodies. This has the advantage of being more robust if the number of bodies in the source changes, but has the disadvantage of not being able to access the child from the source, and not being able to control the point in the source part history where the part is taken.
75
Lesson 3
SolidWorks 2012
Uses of Multibody Solids
Using Split Part with Legacy Data
You can use Split Part to modify imported geometry or legacy parts that would otherwise be difficult to change.
Before
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After
1
Import an IGES file. Click Open .
From the list of file types, select IGES (*.igs, *.iges). Select the file Legacy Data.IGS and click Open.
2
Import Diagnostics.
Sometimes imported data will have faulty geometry. When you import a model with faults, a message asks if you want to run Import Diagnostics.
Click Yes.
Click Attempt to Heal All. The system repairs the faults. Click OK.
3
Cutting plane.
No
Define a reference plane that is parallel to the Front plane and that passes through the vertex shown.
Do
This will be used as the cutting plane in the Split Part command.
76
Vertex
SolidWorks 2012
Lesson 3 Uses of Multibody Solids
4
Split Part.
Using the plane created in the previous step, split the part into two separate bodies.
Move/Copy Body.
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5
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The bodies are shown here in different colors for illustration purposes.
Note
Click Move/Copy Bodies.
Use mates to rotate the body 180° and move the body 0.75” with respect to the Z axis as indicated by the reference triad.
Filling the Gap
No
How you fill in the gap depends on the shape on the part geometry. In this example a simple extrude feature will work. For an example of how a loft feature can be used to fill in a gap, see Merging a Multibody with Loft on page 234.
6
Bridge the gap with an extruded boss.
Do
Create a sketch on the flat face of the rear body.
Use Convert Entities of the face.
to copy the edges
Extrude the sketch using the end condition Up To Next. Be sure the Merge results check box is selected.
77
Lesson 3
SolidWorks 2012
Uses of Multibody Solids
Results.
8
Save and close the part.
Do
No
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7
78
SolidWorks 2012
Exercise 6 Combining a Multibody Part
Exercise 6: Combining a Multibody Part
Create this part by following the steps as shown.
I
Multibody Solids on page 26.
I
Combining Bodies on page 36.
Units: millimeters Procedure
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This lab reinforces the following skills:
Open a new part using the Part_MM template and name it Mbody1. 1
Sketch first profile.
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Use lines and fillets to create an open profile for a Thin Feature.
Extrude the profile 57mm using the Mid Plane end condition and a Thickness of 9.5mm.
2
Sketch second profile.
Extrude as required.
3
Combine bodies.
Combine the two solid bodies into one.
4
Add features.
No
Add boss, cut, hole wizard and fillet features.
Do
Finish the part with 1.5mm radius fillets and rounds.
5
CBORE for M5 Pan Head Machine Screw
Save and close the part.
79
Exercise 7
SolidWorks 2012
Bridging a Multibody Part
Exercise 7: Bridging a Multibody Part
Create this part by following the steps as shown.
I
Multibody Solids on page 26.
I
Merge Result on page 31.
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Units: millimeters
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This lab reinforces the following skills:
Design Intent
The design intent for this part is as follows: 1. Part is not symmetrical. 2. Holes are through all. 3. All fillets and rounds are 5mm radius.
Procedure
Open a new part using the Part_MM template and name it Mbody2. Create a multibody part.
Do
No
1
80
SolidWorks 2012
Exercise 7 Bridging a Multibody Part
2
Finish part with bridge technique.
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Use Merge Result to combine the bodies.
Save and close the part.
Do
No
3
81
Exercise 8
SolidWorks 2012
Indent
Exercise 8: Indent
In this exercise, Indent is used to reshape an existing thin walled feature for a hole, fastener and clearance for tools. This lab reinforces the following skills:
Procedure
Indent Feature on page 54.
Use the following procedure: 1
Open the part Indent.
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I
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It includes two intersecting solid bodies.
2
Circular pattern.
Add a Circular Pattern of the tool body as shown.
3
Indent. Click Indent and select the large solid as the Target body.
No
Select the three revolved solid bodies as the Tool body region.
Do
Under Parameters, set the Thickness to 6mm and Clearance to 1.25mm.
Important!
82
Click OK. The preview shows the indent. Make the tool body region selections from the underside of the target body as shown.
SolidWorks 2012
Exercise 8 Indent
4
Section View. Use the Section View tool with the Front Plane to cut the display.
5
Delete body.
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Delete the tool bodies.
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Note how the Clearance is applied. It can be reversed if necessary.
6
Fillet.
Apply a 2mm fillet to the edge of each cavity.
Save and close the part.
Do
No
7
83
Exercise 9
SolidWorks 2012
Modeling for Rapid Tooling
Exercise 9: Modeling for Rapid Tooling
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When modeling a part it is tempting to think only of how the finished part will be and not consider how to make the part ready for manufacture, and especially how to minimize the cost and time needed for tooling. One way you can leverage your CAD Many thanks to Steve Prentice of Steve Prentice Design model is to prepare it for the Limited for providing this example. www.StevePrenticeDesign.com rapid creation of tooling. By utilizing multibodies, you can model the necessary sand cores and patterns, save them out individual parts, and still have the finished, as-machined version of the part. It is the quickest and least expensive path from design to the delivery of the finished castings. This lab reinforces the following skills:
Procedure
I
Modeling Negative Space on page 62.
I
Saving Solid Bodies as Parts and Assemblies on page 65.
I
Combining Bodies on page 36.
Use the following procedure:
1
Open the part Motorcycle_Gear_Case.
To save time all the necessary sketches have be created in advance.
Do
No
Three of the layout sketches are shown below. The one highlighted in blue represents the pitch circles of the gears. The black one is the parting line of the gear case. The orange one represents the bosses for the mounting bolts.
84
SolidWorks 2012
Exercise 9 Modeling for Rapid Tooling
2
Outline for core.
Hide the sketches named Gears, Body, and Bosses.
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Show the sketch named Core Outline. This sketch was made by converting entities from the Body and Bosses sketches and then sketching and trimming additional geometry.
3
Extrude the core.
Do
No
Extrude the sketch 50mm upwards and 11mm downwards, with 2° of inward Draft in both directions.
85
Exercise 9
SolidWorks 2012
Modeling for Rapid Tooling
4
Fillets. Apply 5mm fillets to the vertical edges.
Use the FilletXpert and the option Connected to start face to simplifying selecting all the edges.
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Tip
5
Revolved cut.
Do
No
Use the sketch Core Face Cut to create a revolved cut feature.
86
SolidWorks 2012
Exercise 9 Modeling for Rapid Tooling
6
Extruded cut.
Use the sketch Core Bridge Cut to extrude a cut 5mm upwards and Through All downwards.
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Apply 2° of Draft so that the draft goes inward in the up direction and outward in the down direction.
7
Extruded cut.
Do
No
Use the sketch Bosses for Gears to extrude a Through All cut Offset 8.5mm above the sketch plane, with 3° of outward draft.
87
Exercise 9
SolidWorks 2012
Modeling for Rapid Tooling
Fillets. Apply 5mm fillets to the edges shown.
Do
No
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8
88
SolidWorks 2012
Exercise 9 Modeling for Rapid Tooling
9
More fillets. Apply 2mm fillets to the edges shown. Be sure to fillet all four edges
Do
No
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on the underside.
10 Save body. Use the Save Bodies command to save the body and name it Sand Core. 11 FeatureManager folders.
In the FeatureManager design tree, expand the Pattern Features folder so you can access the next group of sketches. Select all the features that make up the core body and put them in a new folder and name it Core Features.
89
Exercise 9
SolidWorks 2012
Modeling for Rapid Tooling
12 Hide.
Hide the core body. 13 Extrude the pattern. Use the sketch Outside Body to extrude a boss 43mm upwards and 11mm downwards. Apply Draft of 2°. Use inward draft in the up
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direction and outward draft in the down direction so that all the draft goes in the same direction. Clear Merge results.
14 Revolved cut.
Do
No
Use the sketch Outside Revolved Cut to create a revolved cut feature.
90
SolidWorks 2012
Exercise 9 Modeling for Rapid Tooling
15 Extruded cut.
Use the sketch Bridge Cut to extrude a cut 2mm towards the body and Through All away from the body.
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Apply 2° of Draft so that the draft goes inward in the direction towards the body and outward in the direction away from the body.
16 Fillet.
Do
No
Apply a 2mm fillet to the edges shown.
91
Exercise 9
SolidWorks 2012
Modeling for Rapid Tooling
Do
No
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17 More fillets. Apply 8mm fillets to the edges shown.
18 Save body. Use the Save Bodies command to save the body and name it Body Pattern. 19 FeatureManager folders.
Put the features that make up the pattern body into the Pattern Features folder. Expand the Machined Features folder so you can access the next group of sketches.
92
SolidWorks 2012
Exercise 9 Modeling for Rapid Tooling
20 Combine.
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Show the core body and subtract it from the pattern body.
21 First machining operation. Use the sketch Machining to create a Through All cut. Pay attention
Do
No
to which side of the material is being removed.
93
Exercise 9
SolidWorks 2012
Modeling for Rapid Tooling
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22 Second machining operation. Use the sketch Machined Bosses to create a Through All cut.
Do
No
23 Third machining operation. Use the sketch Spot Face to create a Blind cut 18mm deep.
94
SolidWorks 2012
Exercise 9 Modeling for Rapid Tooling
24 Fourth machining operation. Use the sketch Bearings to create a Blind cut 30.50mm deep to form
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the seats for the bearings.
25 Last machining operation. Use the sketch Bolts to extrude a Through All cut Offset 25mm above
Do
No
the sketch plane to form the counterbores for the mounting bolts.
26 Conclusion.
You now have parts representing the sand core, the pattern for the cast body, and the finished machined part. Providing the pattern maker with complete and accurate CAD data saves time and money. 27 Save and close all files.
95
Exercise 10
SolidWorks 2012
Split Part
Exercise 10: Split Part
Using the part provided, create multiple parts that are related to the original.
I
Splitting a Part into Multibodies on page 71.
Units: inches Procedure
Use the following procedure:
Open the part USB Flash Drive. This part represents the conceptual design of the product.
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1
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This lab reinforces the following skills:
2
Split the part.
Split the part to separate the cap from the remainder of the body. Name the saved part
Cap - USB Drive.sldprt.
Click OK.
3
Resultant bodies state.
Right-click the cap and click Hide from the shortcut menu.
This will hide the cap making it easier to split the remaining body along the parting line.
4
Add a boss.
Do
No
Create the sketch shown below and extrude a boss a distance of 0.160”.
96
SolidWorks 2012
Exercise 10 Split Part
5
Split the part.
Split the part to create the upper and lower halves of the body. Use the Parting Surface as the trim tool. The surface is hidden. If you selected it from the Surfaces folder, it does not have to be visible in order to use it as a trim tool.
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Name the parts as shown in the illustration below.
6
Open the individual parts.
No
Add any additional design details needed.
Create an assembly.
8
Save and close all files.
Do
7
97
Exercise 10
SolidWorks 2012
Do
No
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Split Part
98
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Lesson 4 Introduction to Sweeping
Upon successful completion of this lesson, you will be able to: Understand the unique requirements of working with multi-sketch features.
I
Create boss and cut features by sweeping.
I
Understand the importance of using the Pierce relation to tie the sweep profile to the guide curves.
I
Create a sweep with guide curves.
I
Create a Dome feature.
I
Use the SelectionManager to select extended sets of entities such as edges and sketch entities together, a subset of the entities within a sketch, or entities across multiple sketches.
Do
No
I
99
Lesson 4
SolidWorks 2012
Introduction to Sweeping
Sweeping
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A swept feature, either a boss or a cut, is created by moving a profile along a path. A sweep can be simple or complex.
Not to scale
Swept features can incorporate 3-dimensional curves or model edges as paths, and the sweep section can be made to vary as it moves along a set of other curves called guide curves. In this lesson we will review basic sweeping using a 2D path and a simple, sketched profile. In later lessons we will explore more advanced and complicated applications of sweeping as well as using 3D curves as paths or guide curves.
Sweep Components
The following is a description of two of the major components used in sweeping.
I
Profile
No
Sweeping only supports a single profile sketch. It must be a closed, non-self-intersecting boundary. However, the sketch can contain multiple contours – either nested or disjoint. Path
Do
Path
Nested contours Disjoint contours
100
SolidWorks 2012
Lesson 4 Introduction to Sweeping I
Sweep Path
Sweeps are created from a series of intermediate sections made by replicating the profile at various positions along the path. The intermediate sections are then blended together.
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The system also uses the path to position the intermediate sections along the sweep. Assuming the profile plane is normal to the path: I
The Orientation/Twist Type option Follow Path means that the intermediate sections will always stay normal to the path.
I
If the Keep Normal Constant option is used, the intermediate sections will stay parallel to the plane of the profile sketch.
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These options will be covered in more detail in Orientation and Twist Control on page 196 in Lesson 6: Advanced Sweeping.
Case Study: Faux Raised Panel Door
Traditional raised panel doors are assemblies of five components: two rails, two stiles, and a raised panel. Lower cost alternatives mimic the look but are made from a single piece of material, usually medium density fiberboard.
1
Open the part Faux Raised Panel Door.
Do
No
Examine the part. It consists of a rectangular extruded boss, a userdefined reference plane, and two sketches: the path (in blue) and the profile (in orange).
101
Lesson 4
SolidWorks 2012
Introduction to Sweeping
2
Sweep a cut. Click Swept Cut
.
For the Profile, select the sketch named Profile.
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For the Path, select the sketch named Path.
Click OK.
View the results.
No
3
Do
4
Practice Exercises
102
Save and close the part.
Before continuing with this lesson, complete the following: I I
Exercise 11: Oval Foot Drawer Pull on page 110. Exercise 12: Tire Iron on page 113.
SolidWorks 2012
Lesson 4 Introduction to Sweeping
Sweep with Guide Curves
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Sweeps can contain multiple guide curves which are used to shape the sweep. As the profile is swept, the guide curves can control the profile sketch’s shape, size or orientation. One way to think of guide curves is to visualize them driving a parameter such as a radius. In the illustration below, the profile is attached to the guide curve. As the profile is swept along the path, the radius of the circle changes.
Case Study: Bottle
Modeling complex shapes requires some techniques for creating features that are quite unlike the extruded or revolved shapes built in the basic course. Over the course of the next few lessons, we will go through the steps of creating the molded plastic bottle shown here. We will start by building the basic shape. Other details and features will be added later.
Begin by opening a new part using the Part_IN template.
No
Procedure
1
Sweep path.
Select the Front reference plane and open a sketch.
Do
Sketch a vertical line, starting at the Origin. Dimension this line to a length of 9.125”. This will be used as the sweep path. Exit the sketch and name it Sweep Path.
2
New sketch.
Open a new sketch on the Front reference plane.
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Lesson 4
SolidWorks 2012
Introduction to Sweeping
3
Sketch picture. Click Sketch Picture.
In the Case Study folder for this lesson open the folder named Bottle Images, select the file Front of Bottle.tif, and click Open.
I I
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I
Origin X Position = -2.390in Origin Y Position = -0.100in Width = 4.79in
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Size and position the sketch picture so it is centered on the sweep path and the bottom of the neck is even with the top of the sweep path. The following settings will help:
Exit the sketch and name it Picture - Front.
4
Second sketch picture.
Repeat the previous step, this time inserting the picture named Side of Bottle.tif. Use the same settings to size and position the picture. Exit the sketch and name it Picture - Side.
5
Sketch first guide curve.
No
Open a new sketch on the Front reference plane and sketch a spline using Picture - Front as a guide.
Do
Add Horizontal relations between the ends of the spline and the ends of the sweep path.
104
Add a 0.5” dimension between the end of the spline and the path. Exit the sketch and name it First Guide.
SolidWorks 2012
Lesson 4 Introduction to Sweeping
6
Sketch the second guide curve. Open a new sketch on the Right reference plane and sketch a spline this time using Picture - Side as a
guide.
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Again, add Horizontal relations between the ends of the spline and the ends of the sweep path. Since we want the neck of the bottle to be both a particular size and circular, again add a 0.5” dimension between the end of the spline and the path.
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Exit the sketch and name it Second Guide.
7
Sweep section.
Select the Top reference plane and open a sketch.
Click Ellipse and sketch an ellipse with its center at the Origin.
8
Relating the sweep section to the guide curves.
We want the profile of the sweep section to be related to the guide curves. This way the guide curves will control the size of the ellipse. We do this using a Pierce relation. This is why we created the guide curves before the profile.
No
Press the Ctrl key, and select the point at the end of the major axis and the first guide curve. Right-click and click Pierce. Repeat this procedure for the minor axis and the second guide curve.
Do
9
Fully defined.
Since the Pierce relation on the major axis defines its size and orientation, we do not need to further constrain it. If we had used a dimension to control the size of the major axis, we would need to control the orientation of the major axis in some way.
10 Exit the sketch.
The sweep section is now fully defined so you can exit the sketch. We are now ready to sweep the bottle. Name the sketch Sweep Profile.
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Lesson 4
SolidWorks 2012
Introduction to Sweeping
Sweep Options
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The Sweep PropertyManager contains selection lists for several types of objects: Profile, Path and Guide Curves. It also has options to determine how the system orients the sections while sweeping. The dialog is divided into five sections or group boxes: I I I I
Options
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I
Profile and Path Options Guide Curves Start/End Tangency Thin Feature
The Options group box contains one or more of the following controls depending whether the sweep is a boss or a cut, a base feature, or a multibody.
I
Orientation/twist type
With a simple sweep, the orientation of the profile is controlled by choosing either Follow path, Keep normal constant, Twist Along Path or Twist Along Path With Normal Constant. If the sweep includes guide curves, the orientation of the profile can be controlled by choosing either: Follow path and 1st guide curve, Follow 1st and 2nd guide curves. This is optional.
I
Path alignment type (Available when Follow Path is selected as the Orientation/twist type). Stabilizes the profile when small and uneven curvature
fluctuations along the path cause the profile to misalign. Options are: I
None
Aligns the profile normal to the path. No correction is applied.
I
Minimum Twist (For 3D paths only)
No
Prevents the profile from becoming self-intersecting as it follows the path.
I
Direction Vector
Do
Aligns the profile in the direction selected for Direction Vector. Select entities to set the direction vector.
Note
106
I
All Faces
When the path includes adjacent faces, makes the sweep profile tangent to the adjacent face where geometrically possible. For more detailed information and examples of the Orientation/twist type and the Path alignment type options, see Orientation and Twist Control on page 196.
SolidWorks 2012
Lesson 4 Introduction to Sweeping I
Merge tangent faces
With this option on, it merges tangent faces together, creating an approximation. Planar, cylindrical and conic faces are not merged. I
Show preview
I
Merge result
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With this option on, it displays a shaded preview of the sweep, changing as each component is added. The more complex the sweep, the longer a preview takes.
With this option off, the sweep generates an additional solid body. This option is not available when the sweep is the first feature in the part. I
Align with end faces
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With this option on, it will continue the sweep beyond the geometric end. For more information, see Align with End Faces on page 213. This option is not available when the sweep is the first feature in the part.
Sweep with Guide Curves
As the profile is swept, the guide curves control the profile sketch’s shape, size or orientation. In this example, the guide curves control the length of the major and minor axes of the ellipse.
11 Sweep with guide curves. Click Swept Boss/Base .
12 Select profile and path. Make sure the Profile box is active and select the ellipse. When you select the profile, the Path
box automatically becomes active. Select the vertical line for the path. Callouts appear on each selection.
Do
No
The preview displays the result without the effect of any guide curves.
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Lesson 4
SolidWorks 2012
Introduction to Sweeping
13 Guide curves. Expand the Guide Curves group box.
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A callout appears only on the last guide you select.
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Click in the selection list, and select the two curves indicated.
Showing Intermediate Sections
When sweeping a complex shape, you can see how the intermediate sections will be generated by clicking the Show Sections option. When the system computes the sections, it displays a spin box listing the number of the intermediate section. You can click the up and down arrows to display any of them.
14 Showing Sections. Click Show Sections
, and use the spin box to display the intermediate sections.
Notice how the shape of the ellipse is driven by its relationship with the guide curves.
15 Options.
Do
No
Expand the Options group box, and make sure that the default Follow Path is selected.
Expand the Start/End Tangency group box, and make sure both tangency conditions are set to None. Click OK.
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SolidWorks 2012
Lesson 4 Introduction to Sweeping
16 Finished sweep.
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The swept feature is shown at the right in a Trimetric view.
Do
No
17 Save and close the part.
109
Exercise 11
SolidWorks 2012
Oval Foot Drawer Pull
Exercise 11: Oval Foot Drawer Pull
This lab reinforces the following skills:
I
Procedure
Sketching Splines on page 8. Sweeping on page 100.
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I
Open a new part using the Part_MM template and name it Drawer Pull. 1
Sketch construction geometry.
Open a sketch on the Top reference plane.
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Sketch two centerlines and dimension them as shown below. The midpoint of the long, horizontal centerline is coincident with the Origin.
2
Sketch a spline.
Sketch a three-point spline connecting the endpoints of the construction lines.
Add relations. Add Vertical relations to the drag handles at the two ends of the spline.
No
3
Do
Do not modify the drag handles at the middle point of the spline.
110
SolidWorks 2012
Exercise 11 Oval Foot Drawer Pull
4
Symmetry.
To properly capture the required symmetry in the path, the lengths of the two drag handles must be equal. However, this poses a challenge. If you select the two drag handles, you cannot add an Equal relation to them. If you select the two drag handles and the construction line, you cannot add a Symmetric relation.
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But you can dimension their lengths and use a global variable to make them equal.
Exit the sketch.
5
Sketch the profile.
Open a new sketch on the Front reference plane.
Sketch an ellipse, dimensioned as shown, with its center coincident with the end of the spline.
Exit the sketch.
In order to execute the Sweep command, you must exit the sketch.
No
Note
6
Insert sweep.
Do
Sweep the profile along the path.
111
Exercise 11
SolidWorks 2012
Oval Foot Drawer Pull
7
Oval foot.
Open a new sketch on the Front reference plane. Offset the profile sketch a distance of 4mm to the outside.
8
Fillets.
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Apply a 4mm fillet to the top edge, highlighted in blue, of the extruded boss.
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Extrude a boss to a Depth of 3mm.
Apply a 0.5mm fillet to the edge between the extruded boss and the swept boss.
9
Mirror.
No
Mirror the extruded boss and both fillets with respect to the Right reference plane.
Do
10 Save and close the part.
112
SolidWorks 2012
Exercise 12 Tire Iron
Exercise 12: Tire Iron
Create this by following the steps as shown.
Design Intent
I
Sweeping on page 100.
I
Dome on page 115.
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This lab reinforces the following skills:
The design intent for this part is as follows:
Procedure
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1. Regular end is symmetrical using angled cuts. 2. Wrench end is created using a hexagon cut. 3. Section is constant diameter.
Open a new part using the Part_IN template and name it Tire Iron.
1
Create the sweep path.
Do
No
Create the sketched lines then add the fillet.
113
Exercise 12
SolidWorks 2012
Tire Iron
2
Insert sweep.
Revolved feature.
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3
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Create a new reference plane and use it to sketch the sweep profile. Sweep the profile along the path.
Create a revolved feature on the angled end of the sweep feature. This boss will hold the hexagon cut.
4
Hexagonal cut.
Do
No
Create a hexagonal cut using the Polygon tool .
114
SolidWorks 2012
Exercise 12 Tire Iron
The Dome feature lets you deform the face of a model creating either a convex (default) or concave shape.
Introducing: Dome
To create a dome, select the face or faces you wish to deform. Specify a distance and optionally, a direction. By default the dome is created normal to the selected faces. You can select faces whose centroid lies outside the face. This allows you to apply domes to irregularly shaped faces.
Where to Find It
I I
CommandManager: Features > Dome Menu: Click Insert, Features, Dome
Round the bottom of the cut using the Dome feature. Click Dome .
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5
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Dome Feature
Select the hexagonal face at the bottom of the cut. Clear the Continuous dome check box. Specify a Distance of 0.25”.
Click Reverse Direction concave.
to make the dome
Click OK.
6
Through all cut.
Create the flat end of the part using a sketch and a through all cut.
Save and close the part.
Do
No
7
115
Exercise 13
SolidWorks 2012
Build Your Own Bottle
Using sweep with guide curves, design your own bottle. The shape is not critical. The intent is to practice and understand how guide curves control the shape of the profile as it is swept. The images below are just examples to give you some ideas. Use your imagination.
No
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Exercise 13: Build Your Own Bottle
This lab reinforces the following skills: I
Sweep with Guide Curves on page 103.
Do
Units: your choice
116
SolidWorks 2012
Exercise 14 Hanger Bracket
Exercise 14: Hanger Bracket
Create this by following the steps as shown. This lab reinforces the following skills: Multibody Solids on page 26.
I
Sweep with Guide Curves on page 103.
I
SelectionManager on page 119.
Units: millimeters
Design Intent
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I
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The design intent for this part is as follows: 1. All fillets and rounds are 3mm. 2. Part is symmetrical with respect to the parting line. 3. Draft is 3°.
Procedure
Open a new part using the Part_MM template and name it Hanger Bracket.
1
Create sweep ends.
Do
No
Create two extruded solid bodies to represent the ends of the sweep.
117
Exercise 14
SolidWorks 2012
Hanger Bracket
2
Create sweep path and guide curve.
Sketch the path referencing the existing geometry.
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In the same sketch, sketch the guide curve referencing the existing geometry, including the path.
Path
Guide Curve
3
Create the sweep profile.
Do
No
Create the sweep profile as a sketch using the dimensions shown below.
Path and Guide in the Same Sketch
118
The sweep path and the guide are built in the same sketch because that was a very easy way to sketch them. However, when it comes to selecting them in the Sweep command, you need a way to tell the system to use some of the entities in the sketch for the path, but not all of them. Likewise, you need to do the same with the guide curve.
SolidWorks 2012
Exercise 14 Hanger Bracket
Introducing: SelectionManager
The SelectionManager enables you to select only some of the entities in a sketch, select entities across multiple sketches, as well as select them in combination with model edges. The SelectionManager is available in the loft, sweep, and boundary features only.
Where to Find It
I
Shortcut Menu: Right-click in the graphics area and click
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SelectionManager
Tool
Description
Accepts the selection.
Cancel
Cancels the selection and closes the SelectionManager.
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OK
Clears all items in the selection set being created or edited.
Select Closed Loop
Selects the entire closed loop when you select any segment of the closed loop.
Select Open Loop
Selects all chained entities when you select one entity.
Select Group
Selects one or more individual entities. Selections can propagate to include tangent entities on both ends of a selected entity.
Select Region
Selects parametric regions in the same way as Contour Selection when in 2D sketch mode.
Standard Selection
Uses regular selection, the same as available when the SelectionManager is not activated.
Sweep the boss. Click Swept Boss/Base.
No
4
Clear All
Do
Select the sweep profile you sketched in step 3.
119
Exercise 14
SolidWorks 2012
Hanger Bracket
5
SelectionManager.
and Click Select Open Loop select one of the entities that makes up the path. The system selects all the connected entities.
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Click OK using the right mouse button , or click OK on the SelectionManager.
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Right-click in the graphics area and click SelectionManager from the shortcut menu.
6
Select the guide curve.
Repeat the above process to select the guide curve.
7
Resulting swept boss. Use the Merge result option to
combine all the solid bodies.
Do
No
Click OK on the Sweep PropertyManager.
120
SolidWorks 2012
Exercise 14 Hanger Bracket
8
Create through holes.
Insert fillets and rounds. Add 3mm fillets and rounds, shown here
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9
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Add two through hole cuts to the model.
in red, to complete the model.
Tip
Filleting by feature works best.
Do
No
10 Save and close the part.
121
Exercise 15
SolidWorks 2012
Starship
Exercise 15: Starship
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Create this by following the steps as shown.
This lab reinforces the following skills: SelectionManager on page 119.
I
Inserting Image Files as Background Pictures on page 133.
No
I
Units: centimeters
Procedure
Open a new part using the Part_MM template.
Do
1
122
Units.
Change the part units to CGS (centimeter, gram, second). 2
Viewport background. Click Tools, Options, System Options, Colors.
Under Background appearance, click Plain (Viewport Background color above). Then, set the Viewport Background color to white.
SolidWorks 2012
Exercise 15 Starship
3
Save.
Name the part Starship. 4
Sweep path.
Sketch a vertical line 1525cm long, as shown. Name the sketch Path and exit the sketch. 5
First guide curve.
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Open a new sketch on the Top reference plane.
Open a new sketch on the Top reference plane.
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Select the line in the Path sketch and click Convert Entities. Change the converted line to construction geometry. Sketch a line and tangent arc as shown below.
Exit the sketch and name it Side Guide.
6
Second guide curve.
Open a new sketch on the Right reference plane.
Select the line in the Path sketch and click Convert Entities. Change the converted line to construction geometry.
Do
No
Sketch a line and three tangent arcs as shown. The arc without a dimension has an Equal relation to the R762 arc.
Exit the sketch and name it Top Guide.
123
Exercise 15
SolidWorks 2012
Starship
7
Sweep profile.
Open a new sketch on the Front reference plane. Sketch a semi-ellipse as follows:
I I I I
8
The centerpoint is Coincident with the end of the Path. The major axis has a Pierce relation with the Side Guide. The minor axis has a Pierce relation with the Top Guide. The two endpoints have a Horizontal relation to each other. The start point has a Coincident relation with the major axis.
Bottom half of sweep profile.
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I
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Continuing in the same sketch, sketch a second semi-ellipse as follows: I I I I
9
The centerpoint is Coincident with the end of the Path. The major axis is Coincident with the endpoint of the first ellipse. The minor axis is as yet undefined. Both endpoints are Coincident with the endpoints of the first ellipse.
Construction lines.
Sketch two construction lines from the center to the end of the minor axis, and then to the end of the major axis.
No
Add an angular dimension and set the value to 60°.
Do
Exit the sketch and name it Section.
124
SolidWorks 2012
Exercise 15 Starship
10 Sweep with guide curves.
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Select the profile, path, and both guide curves.
There are two important options in the sweep command that affect the quality of the resulting faces. They are Merge tangent faces which is located in the Options box, and Merge smooth faces which is located in the Guide Curves box. If the sweep profile has segments that are tangent, Merge tangent faces causes the corresponding surfaces to be tangent. Clearing Merge smooth faces improves performance of sweeps with guide curves. However, it will break the faces into segments at all points where the guide curve or path is not curvature continuous.
Results with both Merge tangent faces and Merge smooth faces cleared.
Do
No
Results with Merge tangent faces selected and Merge smooth faces cleared.
Results with both Merge tangent faces and Merge smooth faces selected.
125
Exercise 15
SolidWorks 2012
Starship
11 Rename.
Name the swept feature Fuselage. 12 Sweep path for wing.
Sketch a line for the sweep path as shown. Exit the sketch and name it Wing Path. 13 Guide for trailing edge.
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Open a new sketch on the Top reference plane.
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Open a new sketch on the Top reference plane.
Sketch a line as shown.
Exit the sketch and name it Wing Trailing Edge.
14 Wing section.
Open a new sketch on the Right reference plane. Sketch three lines and an arc as shown at the right.
Dimension and constrain the sketch according to the illustration. Exit the sketch and name it Wing Section.
15 Sweep with guide curves. Clear the Merge results check
Do
No
box.
Because of the symmetry in the model, our plan is to build the wing and engine and then mirror them. However, patterning features such as a sweep with guide curves can be problematic, even with the Geometry Pattern option. A much better approach is to create the wing and engine as a disjoint body and then mirror the body. Rename the feature Wing.
126
SolidWorks 2012
Exercise 15 Starship
16 Fillets. Add a 91.50cm radius fillet to the leading edge of the Wing.
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Add a 160cm radius fillet to the trailing edge of the Wing.
17 Engine.
From the Design Library, in the Exercises folder for this lesson, drag the library feature named Engine Profile and drop it on the planar face at the end of the wing.
18 Edit the sketch.
Do
No
In the sketch there is a small, vertical construction line. This is used to locate the profile.
127
Exercise 15
SolidWorks 2012
Starship
19 Add relations. Add a Midpoint relation
Drag the other end of the construction line and make it Coincident with the upper edge of the wing. Click Finish to exit the sketch.
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20 Revolve.
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between the bottom end of the construction line and the bottom edge of the wing.
Select the sketch and click Revolve Boss/Base. Since sketches can be shared between features, it is not necessary to dissolve the library feature first. Be sure Merge result is selected so the revolved feature merges with the Wing. Rename the feature Engine.
No
21 Fillet.
Create a 15cm radius fillet between the Wing and the Engine. Fillet both the upper and lower sides of the Wing.
Do
Name the fillet Wing/Engine Blend.
128
SolidWorks 2012
Exercise 15 Starship
22 Mirror.
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23 Combine. Click Combine
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Mirror the Engine with respect to the Right reference plane.
.
Do
No
For Operation Type, click Add and select all three solid bodies.
129
Exercise 15
SolidWorks 2012
Starship
24 Fillets. Create 120cm fillets between the Wing and the Fuselage.
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Name the fillet Upper Blend.
25 Sketch for aft section.
Open a new sketch on the planar face at the aft end of the Fuselage.
Expand the Fuselage feature and select the Section sketch.
Use Convert Entities to copy it into the active sketch.
Sketch a line through the minor axis and trim away half of the profile.
26 Revolve.
Create a revolved feature with an Angle of 180°.
Do
No
Name the feature Aft Dome.
130
SolidWorks 2012
Exercise 15 Starship
27 Edit color.
Select the topmost feature and change the part color to medium gray. The R, G, B values are 128, 128, 128.
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Select the two pointed faces (the engine exhaust) and change their color to red (255, 0, 0).
28 DisplayManager.
Click the DisplayManager tab
in the Manager Pane. Then click .
View Scenes, Lights, and Cameras
29 Lights.
Expand the Lights folder.
Right-click Ambient and select Off in SolidWorks from the shortcut menu. Double-click Directional1.
Adjust the settings to match the illustration at the right.
Do
No
The color is light cyan. The R, G, B values are 128, 255, 255.
30 Add two spot lights. Right-click the Lights folder and click Add Spot Light from the shortcut menu.
Repeat this to add a second spot light.
131
Exercise 15
SolidWorks 2012
Starship
31 Adjust settings.
Do
No
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Adjust the settings of the two spot lights to match the illustrations below. The color of Spot2 is dark maroon. The R, G, B values are 128, 0, 64.
132
SolidWorks 2012
Exercise 15 Starship
You can import an image file and use it as a background of a part or assembly. Supported file types include: I I I I I I
Windows bitmap (*.bmp) Portable Network Graphics (*.png) High Dynamic Range (*.hdr) Tagged Image File (*.tif) Adobe PhotoShop (*.psd) Joint Photographic Expert Group [JPEG] (*.jpg)
32 Scene editor.
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Inserting Image Files as Background Pictures
In the DisplayManager, right-click the Scene folder and click Edit Scene.The system will prompt you with the following message:
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To view the document scene you must set the background appearance option to 'Use document scene' (Tools->Options>System Options->Colors). Would you like to set the background appearance to 'Use Document Scene?'
Click Yes.
33 Add a background picture. On the Basic tab click Browse and select Nebula.tif from the Exercises folder of this lesson.
Do
No
Click OK.
133
Exercise 15
SolidWorks 2012
Starship
34 Change the view. Click Perspective
to turn on a perspective view.
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Rotate the view until you are satisfied with the appearance.
To turn off the reference triad, click Tools, Options, System Options, Display/Selection and clear the Display reference triad check mark.
Tip
35 Save.
Save the view state. Then save and exit the part.
Try using some of the other TIFF images that are supplied in the Exercises folder as backgrounds.
Do
No
Optional
134
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Lesson 5 Working with Curves
Upon successful completion of this lesson, you will be able to: Create a 3D sketch.
I
Create a helix.
I
Create a 3D curve from orthogonal views.
I
Create a composite curve from multiple entities.
I
Fit a spline within a tolerance to a set of sketch entities.
I
Sweep a profile along a 3D curve.
I
Create a non-planar curve by projecting a sketch onto a surface.
I
Create a multi-thickness shell.
I
Model threads.
I
Create a curve through a list of X, Y, and Z coordinates.
I
Create and use sketch blocks as a way to reuse data.
I
Create equation driven curves.
Do
No
I
135
Lesson 5
SolidWorks 2012
Working with Curves
This example illustrates several techniques for creating sweep paths while modeling a moderately complex coil spring.
Sweeping Along a 3D Path
In Lesson 4: Introduction to Sweeping we worked through a couple of simple cases of sweeping using a 2D path. In this lesson we will look at a more complex case – using a 3D path. 3D paths can be constructed from 3D sketches, projected curves and helixes among others.
3D Sketching
As the name implies, the entities in a 3D sketch are not constrained to a single plane as they are in a traditional 2D sketch. This makes 3D sketches very useful for applications such as sweeping and lofting. However, 3D sketching can sometimes be a bit of a challenge.
Where to Find It
I
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Case Study: Modeling a Spring
I
CommandManager: Sketch > Sketch Menu: Insert, 3D Sketch
> 3D Sketch
3D sketching with standard reference planes allows you to sketch in 3D by switching between standard reference planes that exist in the model. By default, you sketch relative to the default coordinate system (Front reference plane) in the model. To switch to one of the other two default planes, press Tab while the sketch tool is active. The origin of the current sketch plane is displayed. To switch to a reference plane other than the standard ones, Ctrl-click it.
Subset of Sketch Entities and Relations
There are fewer entities and sketch relations available in 3D sketches compared to 2D sketches. However, other relations such as Along X, Along Y, and Along Z are only available in a 3D sketch.
No
Using Reference Planes
Do
Space Handle
136
When working in a 3D sketch, a graphical assistant is provided to help you maintain your orientation while you sketch on several planes. This assistant is called a Space Handle. The space handle appears when the first point of a line or spline is defined on a selected plane. Using the space handle, you can select the axis along which you want to sketch.
SolidWorks 2012
Lesson 5 Working with Curves
1
New part.
Open a new part using the Part_MM template. Name the part 3D Sketch. Open a new 3D sketch.
Click 3D Sketch 3
.
Centerlines.
Click Centerline
.
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2
Press Tab until the cursor displays the YZ symbol.
Start sketching at the Origin. Sketch the centerline using the Along Y marker to keep it on the Y axis of model space.
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Make the line about 3mm long.
Sketch a second centerline using the Along Z marker the Z axis of model space.
to keep it on
Make this line about 3mm long also.
Dimension the lines to lengths of 3.25mm and 3mm respectively, as shown.
First centerline
4
Second centerline
Dimensions
Sketching a line. Click Line .
No
Press Tab until the cursor displays the XY symbol.
Do
Start sketching at the end of the second centerline.
Drag the line using the to keep it on the X axis of model space. Along X marker
Make the line about 10mm long.
137
Lesson 5
SolidWorks 2012
Working with Curves
5
Continue sketching.
Sketch the next line at approximately a 45° angle below the horizontal as shown. Even though we are sketching parallel to the Front reference plane, no Parallel relation is automatically captured.
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Make the line about 3mm long.
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The symbol next to the cursor indicates that we are sketching parallel to the XY plane. However, the lack of a yellow background like we saw with the Along X marker means this is a reference indicator only. No sketch relation is being created. We will add the Parallel relation in step 9.
6
Switch sketch planes.
Press the Tab key to switch to the YZ plane.
Sketch the line using the Along Z marker model space.
Do
No
Make the line about 3mm long.
138
to keep it on the Z axis of
SolidWorks 2012
Lesson 5 Working with Curves
7
Viewports.
3D sketching in an isometric view can be disorienting. It can be difficult to tell how something moves when you drag it. Multiple viewports can help. , Four
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On the Heads-up View toolbar, click View Orientation View .
8
Drag.
Do
No
Drag the endpoint that is shared between the two blue lines. With multiple viewports, it is easy to see how the angled line moved off of the Front reference plane.
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9
Add relations and dimensions. Select the Front reference plane and the angled line. Add a Parallel
relation.
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Dimension the sketch as shown below.
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Select the Front reference plane and the end of the third line, the one going along the Z axis. Add an On Plane relation.
10 Fillets.
Do
No
Use the Sketch Fillet tool to apply two fillets: one radius 2mm and one radius 1.25mm as shown.
11 Exit the 3D sketch.
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12 Create an offset plane.
Create a reference plane parallel to the Front plane at the endpoint of the 3D sketch.
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Insert a new sketch on the newly created reference plane.
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13 New sketch.
14 Sketch a circle.
Sketch a circle centered on the Origin, and Coincident to the end of the 3D sketch. With this circle, we are preparing to create a helix. The circle establishes the center and beginning diameter for the helix.
If you start the circle from the center and drag the cursor to the endpoint of the 3D sketch, the circle will automatically have a Coincident relationship without the need to apply it manually later.
No
Tip
Do
15 Exit the sketch.
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Working with Curves
Introducing: Helix and Spiral
Insert, Curve, Helix/Spiral creates a helical 3D curve based on a circle
Where to Find It
I
and definition values such as pitch and number of revolutions. The curve can then be used as a sweep path. CommandManager: Features > Curves
> Helix and
Spiral
Menu: Insert, Curve, Helix/Spiral
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I
.
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16 Create a variable pitch helix. Select the circle and click Helix and Spiral
Notice that this helix is variable in both pitch and diameter.
For the Region Parameters, use the settings below for Pitch, Revolutions, and Diameter: Pitch
Revolution
Diameter
1
2mm
0
6.5mm
2
2mm
4
6.5mm
3
1.25mm
5
4.5mm
4
1.25mm
7.5
4.5mm
No
The Start angle is 90° and the helix goes Counterclockwise.
Do
Click OK.
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Creating a 3D Curve from Orthogonal Views
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The ends of the spring have loops to connect to rods. The loops are curved in two different directions which are easy to describe from orthogonal views. The illustration below shows a close up view of one of the loops on the end of the spring.
Insert, Curve, Projected creates a 3D curve using one of two
Introducing: Projected Curve
techniques:
I
Sketch onto Face(s).
Projects a sketch onto a face or group of faces.
I
Sketch onto Sketch.
2D Sketches
No
Projects sketches through space and creates a curve where they intersect. The sketches are usually at right angles to one another, but this is not necessary.
Do
Where to Find It
I I
CommandManager: Features > Curves Menu: Insert, Curve, Projected
Projected Curve
> Project Curve
17 Front view of loop.
Open an new sketch on the Front reference plane and sketch a semicircle as shown.
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18 Exit the sketch. 19 Side view of loop.
Open a new sketch on the Right reference plane, and sketch the side view of the loop as shown.
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Connect the rightmost end of the sketch to end of the helix using a Pierce relation.
20 Exit the sketch.
21 Create projected curve.
Select the front and side view sketches of the loop and click Project Curve . Use the Sketch on Sketch option.
Tip
If you preselect items, SolidWorks attempts to select the appropriate type of projection. You will see a preview of the projected curve.
When seen in an isometric view, the preview of the projected curve makes sense of the two separate orthogonal views.
Do
No
Click OK.
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Introducing: Composite Curve
One of the requirements of the sweep path is that it must be a single entity. A Composite Curve enables you to combine reference curves, sketch geometry, and model edges into a single curve. All entities must touch end-to-end with no gaps or overlaps. This curve can then be used as a guide or path when sweeping or lofting.
Where to Find It
I
Curve I
Menu: Insert, Curve, Composite
22 Composite curve.
> Composite
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CommandManager: Features > Curves
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To sweep the entire spring as a single feature, you will need all of the curve elements you have created to be a single entity. One way to achieve this is to use a composite curve.
and select the 3D Click Composite Curve sketch, the helix and the projected curve. Click OK.
23 Profile.
Open a sketch on the Front reference plane, and create a circle as shown.
Do
No
Create a Pierce relation between the center of the circle and the composite curve.
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24 Exit the sketch.
Unlike an extrude or revolve feature, you must exit the sketch before you can create the sweep feature.
Sweep a boss feature using the circle as the profile and the composite curve as the path. 26 Mirror.
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25 Sweep. Click Swept Boss/Base.
Transitions
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Mirror the swept body about the end that is coincident with the Front reference plane using the Merge solids option.
You might notice that at the ends of the helix are transitions which aren’t perfectly tangent. This is a problem for 3D curves, since the 3D curves cannot be filleted like 2D sketches.
Do
No
One way of smoothing these transitions is to make the entire composite curve into a single spline. Because a spline is an “interpolated” entity (meaning the software fills in the parts of the curve between the user specified spline points), it will smooth out any tangency problems in this model. However, you should be aware that because splines are interpolated geometry, it also means that they are approximations, and will not exactly match the original entities.
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27 Convert composite curve to sketch entities.
Delete the Sweep1 feature.
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To get a smoother spring, we will use a spline for the path instead of the composite curve. Open a new 3D sketch and select the composite curve from the FeatureManager. Click Convert Entities
.
Introducing: Fit Spline
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Notice that the composite curve is converted into several entities of different types: lines, arcs, and splines. We want to join all of these into a single spline.
Where to Find It
Fit Spline creates a spline that fits over a selection of 2D or 3D sketch
or curve entities which touch end to end without gaps or overlaps. A tolerance is applied to the fit. The smaller the tolerance, the better the fit, but also the more complex the spline.
I I
CommandManager: Sketch > Spline Menu: Tools, Spline Tools, Fit Spline
> Fit Spline
28 Convert sketch entities to a spline.
Window select all the sketch entities in the 3D sketch and click Fit Spline . Clear the Closed spline option.
Do
No
Verify that the Constrained option is selected This leaves the spline constrained to the original geometry which gets converted to construction geometry.
Increase and decrease the Tolerance value. Look at the preview and notice how the Tolerance effects how well the spline fits the original entities. If the spline does not fit the geometry accurately enough, you will need to decrease (tighten) the tolerance value.
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Decrease the tolerance value to 1.25mm and see that the fit improves. However, the end near the hook does not look good until the tolerance goes below 0.1mm. Set the Tolerance to 0.1mm and click OK.
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Working with Curves
29 Recreate the sweep. Delete the Pierce relation between the center of the profile circle and
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the composite curve, and recreate it to the 3D fit spline. To do this, you will need to reorder the profile sketch to the end of the FeatureManager. Now recreate the sweep with the small circle as the profile and the fit spline as the path. Notice that the sweep is one continuous face, rather than being broken up into several faces as it was before. Also notice that it is much smoother than it was before at the transition areas.
30 Mirror the spring.
Do
No
Select the flat face nearest the Front reference plane, and mirror as before.
148
31 Save and close the part.
SolidWorks 2012
Lesson 5 Working with Curves
Applying the Label to the Bottle
We are now going to use some of the techniques we learned while modeling the spring to model some of the details of the bottle. First, we will model the outline for the label.
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The outline of the label is a swept feature. The path is a projected curve created by projecting a sketch onto the face of the bottle. The curve that is generated will be used as the Sweep Path of another swept feature. The sketch is already built and has been stored as a library feature.
Library Features
Library Features are generally applied using the Design Library (see
the SolidWorks Essentials manual) but can also be dragged and dropped from the File Explorer or Windows Explorer.
File Explorer
The File Explorer is used to search drives and folders for SolidWorks file types. The files can be dragged and dropped into SolidWorks.
1
2
Open the part Bottle. Browse to the Case Study folder of this lesson and select the part Bottle. This is as it was saved at the end of Lesson 4: Introduction to Sweeping. File Explorer.
Click the File Explorer tab of the Task Pane.
Do
No
Double-click the folders Lesson 5 and Case Study to find the library feature label.
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3
Drag and drop. Show the Front plane of
the part.
Drop the library feature on the boundary or name of the plane in the graphics area.
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Tip
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Drag the label from the File Explorer and drop it on the Front plane.
4
References.
Select the Sketch Point reference and click the part’s Origin. Although this reference is not required, selecting it avoids having to repair the dangling relation. Click OK.
The sketch appears in the FeatureManager design tree in a folder named label<1>.
Tip
Dissolve Library Feature can be used to break down the LibFeat folder. This removes the library feature icon and causes each of the features it contained to be listed individually in the FeatureManager design tree.
Do
No
The Library Feature Folder
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Projecting a Sketch onto a Surface
5
Project Curve dialog and preview.
Click Project Curve
.
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In Creating a 3D Curve from Orthogonal Views on page 143 we looked at one way of using the Project Curve command – intersecting two 2D sketches. In this example, we will create a projected curve by projecting a 2D sketch onto the curved surface of the bottle. This 3D curve will be used as the sweep path to create a boss to outline the label area on the bottle.
Select the Sketch on faces option from the list. 6
Selections.
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Click in the Sketch to Project list and select the sketch. Click in the Projection Faces list and select the model face.
Do
No
By default, the system projects the sketch normal to the sketch plane (along the positive Z axis). If you want to project the curve onto the back of the bottle, click Reverse Projection.
Click OK.
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7
Projected curve.
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The system projects the sketch onto the front surface of the bottle. This 3D curve will be used as the sweep path to create a boss to outline the label area on the bottle.
8
Sketch the profile.
Change to a Right view and select the Right reference plane. Open a sketch and draw a circle in any convenient location.
9
Pierce relation. Add a Pierce relation between the
center of the circle and the projected curve to define its location. Dimension the circle to 0.125” diameter.
Do
No
The projected curve pierces the sketch plane in two places: at the top and the bottom. The system chooses the pierce point closest to where you select the curve. If you want the circle located at the top, select the projected curve near the top. It’s that simple.
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10 Sweep the boss for the label outline.
Exit the sketch. Click Swept Boss/Base
.
Click OK.
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Select the circle as the Profile and the projected curve as the Path.
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Notice the system has no difficulty sweeping a feature with the profile located at the middle of a closed path.
11 Add the neck.
Select the top face of the bottle and open a sketch.
Use Convert Entities into the active sketch.
to copy this edge
Do
No
Extrude the sketch upward a distance of 0.625”.
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The Shell Feature command gives you the option of creating a multithickness shell, in which some walls are thicker (or thinner) than others. You should decide what thickness represents the usual case, which is applied to most faces. Then, you should determine what thickness represents the exceptions, applied to fewer faces. In the case of the bottle, all faces are 0.020” thick except the neck, which is 0.060”.
Shell the Bottle
Create a multi-thickness shell, removing the top of the bottle neck. Use a wall thickness of 0.060” for the neck and 0.020” for all the other faces. 12 Shell command. Click Shell .
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Set the Thickness to 0.020” as the default.
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Multi-thickness Shell
For the Faces To Remove, select the top face of the bottle neck.
13 Multiple thickness. Expand the Multi-thickness Settings group box.
Face selections made here will not use the default thickness.
14 Select thicker faces. Click in the Multi-thickness Faces field and select the
outside face of the bottle neck. Set the thickness to 0.060”. Click OK to create the shell.
15 Results shown in section view.
Do
No
The section view at the right shows the two different wall thicknesses.
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Lesson 5 Working with Curves
Modeling Threads
Models can contain two types of threads: standard or cosmetic threads, and nonstandard threads. Standard threads are not modeled in the part. Instead, they are represented in the model and on the drawing using thread symbols, drawing annotations, and notes.
Creating a Helix
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Nonstandard threads should be modeled. These threads, like the threads on the neck of this bottle, cannot simply be specified by a note on a drawing. Model geometry is needed because downstream applications such as NC machining, rapid prototyping, and FEA require it. A thread is modeled by sweeping a profile along a helical path. A helix can also be used to sweep springs and worm gears. The major steps in modeling threads are: Create the helix.
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I
The helix is based on a sketched circle tied to the diameter of the neck.
I
Create the sketch for the cross section of the feature.
The sketch is oriented with respect to the helix and penetrates the neck.
I
Sweep the sketch along the path (helix) either as a boss or a cut feature.
In this example, the threads are a swept boss.
Procedure
In the remainder of this example, we will build the threads on the neck of the bottle as shown at the right.
16 Offset plane.
Do
No
Create a reference plane offset 0.10” below the top of the bottle neck. This is where the threads will start.
17 Insert sketch.
With this plane selected, open a new sketch.
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18 Copy the edge.
Copy the edge of the bottle neck into the active sketch using Convert Entities. This circle will determine the diameter of the helix.
.
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19 Create the helix. Click Helix and Spiral
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This is why we dimensioned the tops of the two guide curves with respect to the path. If the distances were different, the neck of the bottle would be elliptical, and you cannot create a helix from an ellipse.
Note
For Defined By click Pitch and Revolution. Set the Pitch to 0.15” and the Revolutions to 1.5.
Click Reverse direction so the threads go down the neck.
Set the Start angle to 0° and click Clockwise. Click OK to create the helix.
20 Insert a sketch.
Using another library feature, insert the sketch used for the thread profile. In the File Explorer browse to the Lesson 5\Case Study folder.
No
Insert the library feature thread.sldlfp onto the Right reference plane.
Do
21 Relations.
Edit the sketch of the library feature. Create a relation of Collinear between the horizontal centerline of the sketch and the plane Plane1. Use a silhouette edge to add a Collinear relation between the vertical centerline and the outer edge of the model. The sketch is now fully defined. Exit the sketch.
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22 Sweep the threads. Click Swept Boss/Base
. Select the sketch as the sweep section, and the helix as the sweep path.
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Click OK.
If you are wondering what the option Align with End Faces is used for, we will cover a simple example explaining its purpose later in the course. See Align with End Faces on page 213.
Note
23 Results.
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The results of sweeping the thread are shown at the right.
24 Add the finishing details.
An easy way to round off and finish the ends of the thread is to create a revolved feature. Do this for both ends of the thread.
Tip
Use the vertical edge where the thread meets the body of the neck as the axis of revolution for the revolved feature.
25 The finished bottle.
We are finished with the bottle at this time. We will revisit it later in the course to add a couple of additional features.
Do
No
26 Save and close the part.
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Working with Curves
Curve Through XYZ Points enables you to create a curve through a
series of X, Y, Z locations. You can enter these locations directly into a spreadsheet-like dialog or you can read them from an ASCII text file. The file should have the file extension *.SLDCRV or *.txt. The curve will pass through the points in the same order as they are entered or listed in the file.
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Case Study: Creating a Curve Through a Set of Points
Important!
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Airfoil data is a good example of when you would have a file of X, Y, Z coordinates, although since an airfoil cross section is 2D, the Z coordinate would be zero.
Where to Find It
I
CommandManager: Features > Curves
I
XYZ Points Menu: Insert, Curve, Curve Through XYZ Points
Do 158
> Curve Through
If you haven’t created a text file containing the locations beforehand, you can enter the X, Y, Z coordinates directly into the Curve File dialog. In addition, once you have done that, you can save the point list as a file for reuse. To do this, follow this procedure.
No
Entering Points “On the Fly”
The curve is created outside of a sketch. Therefore, the X, Y, and Z are interpreted with respect to the Front (XY) coordinate system.
Double-click in the upper-left cell (top row, under the heading Point) and the system will open a row for the first coordinate point using the default values of X=0.0, Y=0.0, and Z=0.0. Type in the appropriate values. Use the Tab key on the keyboard to move from one cell to another or just double-click each cell in turn.
SolidWorks 2012
Lesson 5 Working with Curves
Double-click in the next cell below Point #1 to add more rows. If you need to, you can insert a row in the middle of the list. Highlight the row by single-clicking the number in the point column and clicking the Insert button.
Reading Data From a File
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If you anticipate using this data set again, you can save it to a file using the Save button. If you are editing an existing file, Save will overwrite the original file; Save As will save a copy of it. Instead of entering the point data directly, you can browse for a file and read the data from it.
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The file must be an ASCII text file. You can use spaces or tabs between the columns of X, Y and Z coordinates. One method of creating the file is to use the Notepad accessory that comes with Windows. Another method is to use Excel and save the file as a *.txt file.
Remember: the X, Y, and Z are interpreted with respect to the Front, or model space coordinate system.
Editing the Curve
If you need to modify the data points associated with a curve created through a data point set, use Edit Feature, the same as you would for any feature. When editing the definition of the curve, you have several options: I I I
Special Considerations for Airfoil Data
Browse for and substitute a replacement file. Edit the existing point list. Edit the original file and read it in again.
Airfoil data only has X, and Y values. Z is assumed to be zero and is therefore omitted from the file. In order to use the data file in SolidWorks, you will have to add the Z coordinate values.
No
Airfoil data present some other special situations:
Do
I
I
I
The data is “unit” sized. That means the X coordinate goes from 1 to 0 and back to 0. In order to model an actual wing, the data has to be scaled to the chord length of the airfoil. In order to create the wing in its proper orientation with respect to the aircraft coordinate system, you will have to rearrange the X, Y, and Z values. For example, of you want the airfoil crated parallel to the Right reference plane, the X values in the original data must go in the Z column and the sign must be reversed. If you wanted to change the angle of attack of the airfoil, that is, rotate it, you would have to transform the values in the file. Not a trivial task.
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To work around these issues, we will pursue the following strategy: 1. 2. 3. 4. 5. 6.
Procedure
Create the curve in model space using the data “as is”. Open a sketch on the Front reference plane. Use Convert Entities to replicate the curve as sketch entities. Make a block of the active sketch. Create a new sketch on the appropriate reference plane. Insert the block, scale it, and position it where needed.
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Strategy: Use Sketch Blocks
Begin by opening a new part using the Part_IN template. 1
Change units.
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Change the units to feet & inches. We use feet and inches because the airfoil data is from a World War II-era Boeing B-17 and its specifications are all in those units.
2
Insert curve.
Click Curve Through XYZ Points
3
.
Select the file.
Click Browse and select the file NACA_0018.sldcrv from the Curve Data folder in the Case Study folder of this lesson.
The file contents are read into the dialog and separated into columns.
Note Note
The browser can be set to search for Curves (*.sldcrv) or Text Files (*.txt). NACA stands for National Advisory Committee for Aeronautics, the precursor to NASA.
Add the curve. Click OK to add the curve to the part. A smooth spline curve is created using the points contained in the file as shown below in a Front view. A feature named Curve1 appears in the FeatureManager design tree.
Do
No
4
5
New sketch.
Open a new sketch on the Front reference plane. 6
Convert Entities.
Use Convert Entities to copy the curve feature into the active sketch.
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7
Complete the sketch.
The trailing edges of the airfoil are not closed. Sketch a line connecting the two ends of the spline.
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Do not exit the sketch yet. Blocks are a way to save, edit, and reuse graphic information. Often people think of blocks in terms of elements in drawings, such as standard notes, symbols, and title blocks. However, blocks are also a way to reuse and manipulate sketch geometry.
Introducing: Sketch Blocks
You can create blocks from single or multiple sketch entities. Using blocks you can:
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Sketch Blocks
I
I I I
Create layout sketches using a minimum of dimensions and relations. For more information about creating layout sketches using blocks, please refer to the Assembly Modeling course. Freeze a subset of entities in a sketch to manipulate as a single entity. Manage complex sketches. Edit all instances of a block simultaneously.
To create a block you can either select entities in the graphics area, or save a sketch directly to a block file. Blocks are separate SolidWorks files with the file extension *.sldblk.
Where to Find It
I I
8
Menu: Tools, Blocks, Save Blocks Toolbar: Save Sketch as Block
Create block. Select the Origin. Click Tools, Blocks, Save.
In the Save As dialog box, browse to the Curve Data folder and save the block as NACA_0018.sldblk.
No
Click Save.
Selecting the Origin defines that location as the insertion point of the block. In other words, when you insert the block, this is the point that lines up with the cursor in the graphics window and determines the location of the block when you click.
Do
Why Select the Origin?
9
Repeat.
Repeat step 5 through step 8 this time using the curve file NACA_0010.sldcrv. Likewise, name the block NACA_0019.sldblk. 10 New part.
Change the units to feet & inches. Save the part and name it Wing.
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11 Reference plane.
Create a reference plane offset from the Right plane a Distance of 4 feet.
Name this plane Root. 12 New sketch. 13 Insert block. Click Tools, Blocks, Insert.
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Open a new sketch on the Root reference plane.
Browse to the Curve Data folder and select NACA_0018.sldblk. Under Parameters, set the Scale to 19.6.
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Since the airfoil sketch had a chord length of 1 unit, in this case 1 foot, a Scale of 19.6 scales the airfoil to 19.6 feet which is the length of the chord at the root of the wing. Click the Origin to insert the block. Click OK.
14 Offset plane.
Create a reference plane offset 45 feet from the Root reference plane. Name this plane Tip.
15 New sketch.
Open a new sketch on the Tip reference plane.
16 Define the insertion point.
As you can see from the drawing at the right, the cross section of the tip has to be positioned aft and up to accommodate the taper and dihedral angle of the wing.
Do
No
Insert a sketch point and dimension it as shown below.
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17 Insert block. Click Tools, Blocks, Insert.
Browse to the Curve Data folder and select NACA_0010.sldblk. Under Parameters, set the Scale to 7.25.
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This scales the airfoil to 7.25 feet which is the length of the chord at the tip of the wing. Click the sketch point to insert the block.
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Click OK.
Exit the sketch.
18 Loft.
Loft will be covered in detail in Lesson 7: Lofts. However, we are creating a simple loft here so we can see the finished wing. Click Features > Loft
.
Select the two sketches being careful to pick in roughly the same location on corresponding entities in each sketch.
Do
No
Click OK.
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19 Save and close the part.
Equation Driven Curves
Using equation driven curves you can create splines that are defined by equations.
Introducing: Equation Driven Curve
The equations for equation driven curves can be either Explicit where Y is a function of X, or Parametric where X, Y, and Z are functions of T. If you create a parametric equation driven curve in a 2D sketch, only X and Y can be defined. 3D sketches support parametric equations only.
No
You can use any functions that are supported in the Equations dialog box. For example: “D1@Sketch1”*sin(t).
. Enter the parametric equations shown at the right and click OK.
What do the Equations Mean?
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In a 3D sketch, Xt, Yt, and Zt are interpreted with respect to the model coordinate system. The equations for Xt and Zt together define a circle. The value 14 is the radius of that circle. The equation for Yt defines a cosine curve. (The only difference between a sine curve and a cosine curve is the phase — the cosine curves is shifted 90° out of phase compared to the sine curve as illustrated below.)
Cosine curve
Sine curve
No
In the equation for Yt, 1.25*cos(5*t), the value 1.25 is the amplitude of the curve. As written, the amplitude is centered with respect to Y=0. If you wanted to offset the amplitude you would add an offset value. For example, 1.25*cos(5*t)+2 would center the curve with respect to Y=2 causing it to oscillate between Y=0.75 and Y=3.25.
Do
The value 5 is the angular frequency. A sine curve is a periodic curve completing one oscillation in 2*π radians. The value 5 causes the curve to complete five oscillations in 2*π radians. The parameter t1 defines the start of the curve and t2 defines the end, in radians.
Create a second equation driven curve using the following equations:
Add a Fixed relation to this curve as well. Exit the sketch. 6
Profile sketch.
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Open a 2D sketch on the Right reference plane.
Sketch a rectangle and dimension it as shown.
Add Pierce relations between the midpoints of the two vertical lines and the equation driven curves. Exit the sketch.
7
Sweep.
Select the 2D sketch for the Profile.
Using the SelectionManager, select the inner curve for the Path and the outer curve for the Guide Curve.
For Orientation/twist type, select Follow path and 1st guide curve.
166
Orientation and twist options will be covered in more detail in Lesson 6: Advanced Sweeping.
No
Do
Note
Click OK.
SolidWorks 2012
Lesson 5 Working with Curves
8
Mirror.
Why didn’t we create the two equation driven curves through a full 360° (2*π radians)?
Question
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Mirror the body with respect to the Right reference plane to complete the part.
Because there is a limitation in equation driven curves that does not allow closed curves — curves where the starting and ending points are merged.
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We could have created a second set of equation driven curves but that would have been more work than simply mirroring the swept body. Save and close the part.
Do
No
9
167
Exercise 16
SolidWorks 2012
Worm Gear
Exercise 16: Worm Gear
Procedure
I
Creating a Helix on page 155.
I
Sketch Blocks on page 161.
I
Sweeping on page 100.
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This lab reinforces the following skills:
Open a new part using the Part_MM template and name it Worm Gear. Extrude a cylinder.
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1
The ends of the finished gear are symmetrical, so use the Midplane end condition.
2
Offset plane and sketch.
The plan is to make the helix longer than the final gear and then trim it to size. To accomplish that, create a plane offset from the end of the cylinder, open a sketch on it, and convert the edge of the cylinder into the sketch.
3
Create the helix.
Do
No
Be sure to use sufficient revolutions so the helix extends beyond the far end of the cylinder.
168
SolidWorks 2012
Exercise 16 Worm Gear
4
Gear tooth profile.
Insert the block Gear Tooth Profile.sldblk that is located in the Exercises folder of this lesson.
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Create a plane normal to the end of the helix and open a new sketch.
Add a Pierce relation between the helix and the sketch point in the block.
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Add a Perpendicular relation between the long construction line and the axis of the cylinder.
5
Sweep.
No
Sweep the gear tooth profile along the helix.
Do
6
Cut off the excess.
Sketch a rectangle. Make the two vertical sides Colinear with then ends of the basic cylinder. Make sure the two horizontal sides are outside and clear of the gear teeth. Extrude a Through All cut using the option Flip side to cut.
169
Exercise 16
SolidWorks 2012
Worm Gear
7
Extrude a boss.
Open a sketch on the cut end of the gear. Sketch a circle and make it Coradial with the edge of the cylinder.
8
Extrude another boss.
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This boss is concentric with the previous boss. Refer to the illustration for dimensions.
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Extrude a boss 3mm.
9
Mirror.
Mirror the bosses you created in the previous two steps.
Do
No
10 Save and close.
170
SolidWorks 2012
Exercise 17 D-cell Flashlight Spring
Exercise 17: D-cell Flashlight Spring
Using a helix with a variable pitch and diameter, create a spring for a Dcell flashlight.
Procedure
I
Creating a Helix on page 155.
I
Sweeping on page 100.
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This lab reinforces the following skills:
Open a new part using the Part_MM template and name it Flashlight_Spring. 1
Create the helix.
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Create a variable pitch helix defined by pitch and revolution. Pitch
2
Revolution
Diameter
0.5mm
0
40mm
2.0mm
1
40mm
5.0mm
2
35mm
5mm
4.5
22.5mm
0.001mm
6
15mm
Sweep the spring.
The wire diameter is 1.25mm. Save and close the part.
Do
No
3
171
Exercise 18
SolidWorks 2012
Water Bottle Cage
Exercise 18: Water Bottle Cage
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In this exercise you will model the wire portion of a water bottle cage for a bicycle. Although the illustration shows the mounting clips and a water bottle, those components are not relevant to the objectives of the lesson so you will not be modeling them. This lab reinforces the following skills: I
Sketching Splines on page 8.
I
Projected Curve on page 143.
I
Sweeping on page 100.
Procedure
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Units: millimeters
Open a new part using the Part_MM template and name it Water
Bottle Cage.
1
New sketch.
Open a new sketch on the Top reference plane.
Sketch and dimension a circle as shown. Note the location of the Origin. Use symmetry to maintain the orientation of the 40° angle.
The vertical centerline will be used in the next sketch.
2
Sketch the second profile. Open a new sketch on the Front
reference plane.
Do
No
The sketch consists of a short, horizontal line starting at the Origin, a tangent arc, and a spline.
172
Add a Pierce relation between the bottom end of the rightmost centerline and the vertical centerline in the previous sketch. Use curvature display and sketch relations to control the shape of the spline.
SolidWorks 2012
Exercise 18 Water Bottle Cage
3
Projected curve.
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Create a projected curve using the two sketches.
4
Sweep profile.
Sketch a circle on the Front reference plane.
Relate it to the projected curve with a Pierce relation and dimension it.
Sweep.
Do
No
5
6
Save and close the part.
173
Exercise 19
SolidWorks 2012
3D Sketching
Exercise 19: 3D Sketching
Create this by following the steps as shown.
Procedure
I
3D Sketching on page 136.
I
Sweeping on page 100.
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This lab reinforces the following skills:
Open a new part using the Part_MM template and name it 3D Sketching. New 3D sketch.
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1
Create a new 3D Sketch and change the view orientation to Isometric.
2
Sketch lines.
Click the Line tool and start the first line at the Origin. Sketch the line in the X direction of the Front reference plane.
3
Switch planes.
Begin dragging the second line to see the space handle. Press the Tab key to switch from the default Front plane to the other planes.
No
Switch to the Right plane orientation and sketch along the Z axis.
Do
4
174
Continue lines.
Continue sketching lines and switching planes so that you are always sketching on X, Y or Z in the appropriate direction.
SolidWorks 2012
Exercise 19 3D Sketching
5
Relation. Add a Coincident relation between
6
Dimensions.
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Dimension the true length of the lines as shown to fully define the sketch. Select the endpoints of the lines or the lines themselves.
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the endpoint and line shown at the right.
7
Fillets.
Add 20mm fillets at the vertex points.
8
9
Exit the 3D sketch.
Profile sketch.
No
Create a new plane normal to the 3D sketch and coincident to its endpoint.
Do
Sketch a circle of diameter 15mm.
175
Exercise 19
SolidWorks 2012
3D Sketching
10 Sweep.
Optional
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Sweep the circle section along the 3D path.
Edit the profile sketch of the sweep to create a thin wall. 11 Edit sketch.
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Edit the profile sketch and add a concentric circle, diameter 20mm. Exit the sketch.
12 Modified sweep.
The concentric circles form a thin wall in the sweep.
Do
No
13 Save and close the part.
176
SolidWorks 2012
Exercise 20 3D Sketching with Planes
Create this part by following the steps as shown. This lab reinforces the following skills: 3D Sketching on page 136.
I
Using Reference Planes on page 136.
I
Sweeping on page 100.
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I
No
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Exercise 20: 3D Sketching with Planes
Do
Planning Ahead
Procedure
Often times when 3D sketching you will need reference planes other than the three default ones. Whenever possible, it is a good idea to create these before you start 3D sketching. This usually requires some preplanning as well as some construction geometry. Open an existing part named 3DSketchAngle.
177
Exercise 20
SolidWorks 2012
3D Sketching with Planes
1
Reference plane.
Create a reference plane at a 15° angle to the Right reference plane, passing through the leftmost 100mm construction line as shown below.
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Name the plane Angle 15.
2
Second reference plane.
Create a second reference plane at a 60° angle to the Front reference plane, passing through the rearmost 150mm construction line as shown below.
Do
No
Name the plane Angle 60.
178
SolidWorks 2012
Exercise 20 3D Sketching with Planes
3 4
New 3D sketch. Create a new 3D Sketch and change the view orientation to Isometric. Sketching a line.
Drag the line using the Along X marker to keep it on the X axis of model space. End the line so it is Coincident with the end of
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the construction line.
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Click the Line tool and start sketching at the Origin of the sketch.
Switching Sketch Planes
To review switching sketch planes in 3D sketches, please see the topic Using Reference Planes on page 136.
5
Switch sketch planes. Press the Ctrl key and click the plane named Angle 15.
When you start sketching the next line, the space handle will be aligned with the reference plane named Angle 15. Drag the line using the Vertical marker to keep it on the Y axis of the active plane. Look at the cursor
The green square indicates that you have selected a plane for sketching. The On Surface symbol indicates you are capturing an On Surface relation between the line and the plane.
No
I
:
Do
I
179
Exercise 20
SolidWorks 2012
3D Sketching with Planes
6
Continue sketching.
to keep it on the X axis of
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Drag the line using the Horizontal marker the active plane.
7
Add relation. Deselect the Line tool.
Do
No
Add an On Plane relation between the end of the line and the Angle 60 reference plane.
180
SolidWorks 2012
Exercise 20 3D Sketching with Planes
8
Activate the Angle 60 plane. Double-click the Angle 60 reference plane. This becomes the active
sketch plane.
Then sketch a Vertical line as shown.
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Sketch a Horizontal line starting Coincident with the endpoint of the previous line. Drag this line beyond the Right reference plane. Horizontal and Vertical are interpreted with respect to the active sketch plane, not model space. The Angle 15 and Top reference planes
Note
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are hidden for clarity.
9
Add relations.
Deselect the Line tool. Add an On Plane relation between the end of the angled line and the Top reference plane. The two angled planes were hidden for illustration purposes.
Do
No
Note
181
Exercise 20
SolidWorks 2012
3D Sketching with Planes
10 Continue sketching. Deactivate the Angle 60 reference plane by double-clicking an empty
area of the graphics window.
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Starting at the end of the angled line, sketch along the model X axis ending the line so it is Coincident with the corner of the Setup sketch.
11 One more line. Press Ctrl and click the Right reference plane. Sketch the final line so it is approximately perpendicular to the Angle 60 plane.
Do
No
Add a Perpendicular relation between the line and the Angle 60 plane.
182
SolidWorks 2012
Exercise 20 3D Sketching with Planes
12 Add dimensions.
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Dimension the sketch as shown below. This fully defines the sketch.
13 Fillet. Add 30mm fillets to all six corners.
No
14 Sweep.
Do
Create a circle profile and use the sweep command to complete the exercise.
15 Save and close the part.
183
Exercise 21
SolidWorks 2012
Blower Housing
Exercise 21: Blower Housing
Create this by following the steps as shown. Helix and Spiral on page 142.
I
Sweep with Guide Curves on page 103.
I
Sweeping Along Model Edges on page 213.
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I
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This lab reinforces the following skills:
Getting Started
With some models, where you should start is not obvious. You may find it very tempting to start building your sweep by drawing the sweep profile first. It is best practice, however, to create the path and guide curves first so that the profile appears at the right point in history to apply Pierce relations to make the sweep work. This can present some difficulties because it is often helpful to use the profile to help build the path and guide curves. If you find that you must build the profile first and use it to construct the path and guide curves, you can copy the original profile to a new sketch which is driven by the path and guide curves.
In this part, the overall shape is a flat spiral, but the cross section of the involute shape changes in two directions as the sweep progresses. Making the profile grow taller around the sweep will mean that we use a spiral for the path and a spiral of a slightly larger pitch for the first guide curve. Making the sweep grow in width will be the work of a helix. Open a new part from the Part_IN template and name it Blower Housing.
No
Procedure
Do
1
Create the path.
The path should be the smallest spiral, since it is best practice to sweep to the outside of a curve when you can. Sweeping to the inside of a curve can create self-intersecting geometry if the curvature of the path is too small. Sketch a circle on the Front reference plane with a 4 inch diameter centered at the Origin, as shown.
184
SolidWorks 2012
Exercise 21 Blower Housing
I I I I
2
For Defined By click Spiral. For Pitch enter 0.750”. For Revolutions enter 1. For Start angle enter 0° and click Counterclockwise.
Create the first guide curve.
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Next use the Helix/Spiral tool with the sketched circle to create a spiral with the settings below:
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Draw a second circle again on the Front reference plane, this time with a 5 inch diameter centered at the Origin.
Use the settings below to create a second spiral which will function as a guide curve: I I I I
3
For Defined By click Spiral. For Pitch enter 1.500”. For Revolutions enter 1. For Start angle enter 0° and click Counterclockwise.
Create the second guide curve.
Create a new plane with an Offset Distance of 0.200” from the Front reference plane. Name it Helix_Plane.
Draw a third circle on Helix_Plane, with a 4.5” diameter, again centered at the Origin. This time create a helix with the settings shown.
I
For Defined By click Height and Revolution.
I
Constant pitch For Height enter 0.500”. For Revolutions enter 1. For Start angle enter 0° and click Counterclockwise.
No
I I
Do
I
You do not need to make a tapered helix to compensate for the increasing diameter. We will accommodate that in the profile sketch. You should now have two spirals and a helix.
185
Exercise 21
SolidWorks 2012
Blower Housing
4
Draw the profile.
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Open a sketch on the Top reference plane, and sketch a rectangle with two tangent arcs on the horizontal ends, turning two of the lines of the rectangle to construction geometry as shown.
To create involute shape, the spirals will drive the X dimension, so as the spirals get progressively further apart from one another, the X dimension of the sketch gets larger. The Y dimension will be driven by the helix.
5
Add sketch points to the profile sketch.
Add sketch points to the midpoints of the vertical lines. The points allow the spirals to drive the X dimension. The midpoint relations enable the Y dimension to be driven symmetrically.
Add Pierce relations to spirals. Next, add Pierce relations
No
6
between the sketch points and the spirals.
Do
Note
186
The helix has been hidden for clarity.
SolidWorks 2012
Exercise 21 Blower Housing
7
Add another sketch point to the profile.
Add a sketch point to the construction line as shown
8
Add Pierce relation to helix. Add a Pierce relation
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between the new sketch point and the helix. Make sure to select the helix in the graphics window near the end where you want the point to touch it. There are three locations on the plane where the pierce would be correct: either end and the midpoint of the helix.
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Do not place the point at the midpoint of the line, just on the line so that it only gets a Coincident relation. The point needs to be able to control the Y dimension and be able to slide back and forth, since the helix does not increase in diameter, but the spirals do.
Important!
9
Create the sweep.
Use the small spiral as the path, the large spiral as the first guide curve, and the helix as the second guide curve. Check the intermediate profiles to see how the profile sketch follows the guide curves parametrically.
Do
No
Also notice that the helix on one side drives the width of the involute symmetrically.
187
Exercise 21
SolidWorks 2012
Blower Housing
10 Extrude the outlet.
Open a sketch on the outlet end of the involute, select the end face, and click Convert Entities. Rename this feature Outlet.
11 Offset.
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Open a new sketch on the Front reference plane.
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Now extrude the sketch 2.25”.
Select the smaller spiral from the FeatureManager design tree, and create a sketch offset at 0.200”.
12 Complete the sketch.
Complete the sketch with horizontal and vertical lines as shown.
Trim the lines and the spline to create a closed profile.
Do
No
13 Create the body. Create a Mid-Plane extrusion with a Depth of 0.900”.
188
SolidWorks 2012
Exercise 21 Blower Housing
14 Draw outlet ring sweep profile.
Open a new sketch on the Front reference plane. Switch to Hidden Lines Removed to make the sketch more visible. Notice the sketch penetrates the solid body. In SolidWorks, sweeps are not always exact, so it is best practice to avoid creating lineon-line geometry. In this case, make the sweep interfere slightly with the main body to make sure that the new feature merges.
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Tip
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Create a Pierce relation between the endpoint of the arc and the edge of the Outlet. Edge of Outlet
15 Sweep the outlet ring.
Select the sketch from the previous step as the profile and the pierced edge as the path.
Use the option Tangent propagation so the sweep will
No
continue along the tangent edges, much like a fillet.
Do
The result of the sweep is shown in a different color for illustration purposes.
189
Exercise 21
SolidWorks 2012
Blower Housing
16 Create extrusion.
Open a sketch on the flat face as shown. Sketch a circle centered on the Origin with a diameter of 4.75”.
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Extrude the sketch a Depth of 0.550” with Draft of 5°.
17 Mirror the feature.
Mirror the extruded boss about the Front reference plane.
Splitting a Face
A split line is used to divide model faces into two. Split lines are created like any other sketched feature. They can be one or more connected sketch entities. They must be oriented so that they will pass through model faces when projected normal to the sketch plane.
Introducing: Split Line
Split Line uses one or more curves to split one model face into two.
Where to Find It
The curves are sketched on a plane and projected onto the faces to be split. I
Do
No
I
CommandManager: Features > Curves Menu: Insert, Curve, Split Line
190
> Split Line
SolidWorks 2012
Exercise 21 Blower Housing
18 Split line.
Open a sketch on the Front reference plane. Draw a circle centered on the Origin with a diameter of 3.25”. Create a Split Line feature splitting the two flat faces as shown.
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Make sure the Single Direction option is cleared.
19 Split the Outlet face.
Open a new sketch on the end face of the Outlet. Select the flat face, and offset the edges by 0.05” to the inside as shown.
Do
No
Create a Split Line feature on the face of the Outlet.
191
Exercise 21
SolidWorks 2012
Blower Housing
20 Add fillets.
Do
No
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Add fillets as shown.
192
SolidWorks 2012
Exercise 21 Blower Housing
21 Shell.
Shell the part using a Thickness of 0.050”.
Notice that at the transition from the involute scroll to the straight outlet, there is a bit of tangent discontinuity. To correct for this, try using a spline to flow smoothly between the spiral and the straight line. A similar technique was shown in the coil spring case study.
No
Tip
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For the Faces to Remove, select the three faces that were created by the split lines in step 18 and step 19.
Do
22 Save and close the part.
193
Exercise 21
SolidWorks 2012
Do
No
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Blower Housing
194
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Lesson 6 Advanced Sweeping
Upon successful completion of this lesson, you will be able to: Understand and apply orientation and twist control options to achieve the desired results when sweeping.
I
Understand and apply the path alignment options when sweeping.
I
Understand the role of guide curves in controlling twist.
Do
No
I
195
Lesson 6
SolidWorks 2012
Advanced Sweeping
When creating sweeps, controlling the orientation of the sketch profile is very important, and for certain types of sweeps it may seem difficult. To control the sweep, it is important to understand what sweeps are doing that effects twisting and orientation. One way to think of, and even better, to describe, is to put it in terms of degrees of freedom and the attitude of an airplane.
Yaw
Path
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Pitch and yaw are defined by the orientation of the profile’s sketch plane to the path. As the sweep progresses, it is the path that controls pitch and yaw.
Profile
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Orientation and Twist Control
Pitch Roll is the twisting or spinning of Roll the profile around the path. Generally the challenge is to either induce twist, or prevent it. This is done using options or guide curves.
Sweeps are created from a series of intermediate sections made by replicating the profile at various positions along the path. The intermediate sections are then blended together. In this sense, you can think of sweeps as an automated set-up for a loft. This is an oversimplification of what happens, and there are special cases where other types of functions are used, but it will do for the purposes of understanding how to set up a successful sweep. Intermediate sections are referred to several times in this section in situations where SolidWorks does not actually display them. Intermediate sections can only be displayed for sweeps with guide curves. However, visualizing the intermediate sections is a good way to understand the final geometry and reasons for why a sweep might fail, such as self-intersection.
Do
No
Intermediate Sections
196
SolidWorks 2012
Lesson 6 Advanced Sweeping
Follow Path
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Intermediate sections for sweeps using a planar path maintain the relation of the initial profile to the path throughout the sweep. If the profile sketch is perpendicular to the beginning of the sweep path, then the rest of the intermediate sections are also perpendicular to the sweep path. If the profile is at an angle, so are the intermediate sections.
The Keep Normal Constant option keeps the intermediate sections parallel to the original profile.
Do
No
Keep Normal Constant
197
Lesson 6
SolidWorks 2012
Advanced Sweeping
The default Orientation/twist type is Follow Path. This is appropriate and good for many sweeps, especially simple ones. For example, consider sweeping a simple tube. As you can see in the illustration below, the circular profile stays normal to the centerline (path) of the tube.
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Which to Use?
Do
No
However, when the Orientation/twist type is set to Keep Normal Constant, the tube is distorted. Clearly this is not appropriate for this type of sweep.
198
SolidWorks 2012
Lesson 6 Advanced Sweeping
One situation where Keep Normal Constant is the correct choice is when sweeping a rib. Consider this example: the entire part – base, bosses, and rib – requires 5° of draft.
Procedure
Open the part Keep Normal Constant.
Edit feature. Edit the Sweep1 feature. The Orientation/twist type is set to Follow Path.
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1
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When to Use Keep Normal Constant
Click Cancel.
2
Edit Sketch6. This sketch was created using the Intersection Curves command to find the intersection between the Right reference plane and two faces in the part. The angle dimension was created by selecting the two ends and the corner of the intersection curves.
Notice that even though the profile had the proper amount of draft built into it, the side of the rib has less than the required 5° of draft. This is because as the profile rotates to stay normal to the path, it has the effect of foreshortening the draft angle. Exit the sketch.
3
Edit feature. Edit the Sweep1 feature.
No
Set the Orientation/twist type to Keep Normal Constant. Click OK to rebuild the feature.
Do
4
Edit Sketch6. Notice that the draft angle is now correct.
199
Lesson 6
SolidWorks 2012
Advanced Sweeping
Controlling Twist
The concepts of Follow Path and Keep Normal Constant also hold true for sweeps with 3D paths. However, with a 3D path, there is an additional degree of freedom – how the intermediate sections rotate or spin around the path.
Do
No
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In other terms, pitch and yaw are controlled by the profile’s relationship to the path, but roll is not.
200
SolidWorks 2012
Lesson 6 Advanced Sweeping
1
Open the part Twist.
Notice how the sweep twists. If the profile had been circular, this may not have been noticeable.
Do
No
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The goal is to make the rectangular profile remain aligned with Axis1, such that the faces on the inside and outside of the ring are normal to the Front reference plane.
201
Lesson 6
SolidWorks 2012
Advanced Sweeping
2
Predicting twist.
The twist of this part may not be intuitively clear, but it can be predicted by looking at the curvature comb for the path. Show the path sketch and the profile sketch. Show curvature comb for the path spline.
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Notice that the relationship between the curvature comb and the profile remains approximately constant throughout the sweep.
Turn off the curvature comb display and hide the two sketches.
3
Minimize twist.
Do
No
Edit the sweep feature, and set the Path alignment type to Minimum Twist.
202
Section View
Compared to the default setting, Minimum Twist is an improvement, but not enough. The edges of the cross section should be square to the display. The profile still does not have an external reference to control its rotation about the path.
SolidWorks 2012
Lesson 6 Advanced Sweeping
Since we know that a sweep with a planar path does not twist, we can use that to prevent the section from spinning.
Using a Planar Path and Guide Curve to Control Twist
4
Create a planar curve for the path.
ibu te
To do this while still keeping the 3D shape of the sweep, we will use the 3D spline as a guide curve, and a projection of the 3D spline onto the Front reference plane as the path. Expand the sweep feature. Show the path sketch, 3DSketch1.
Drag the rollback bar just after the sweep feature and before Sketch1.
You may receive a message telling you the sketches will be temporarily unabsorbed for editing purposes. If so, click OK. Open a new sketch on the Front reference plane.
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Use Convert Entities to project the 3D spline onto the sketch plane.
No
Exit the sketch.
Do
5
Modify the profile sketch.
Drag the rollback bar down between Sketch1 and the sweep feature. Edit Sketch1.
203
Lesson 6
SolidWorks 2012
Advanced Sweeping
6
3D sketch
Edit the sweep feature.
2D sketch
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Keep the same sketch selection for the Profile. Select the new 2D sketch for the Path. Select the 3D sketch for the Guide Curve.
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Draw a new construction line which is collinear with the existing construction line and that extends to the 2D sketch. Add a Pierce relation between the end of the new construction line and the 2D sketch. In this way, as the profile is moved around the path, the construction line will remain parallel to Axis1. Exit the sketch.
7
Examine the resulting sweep.
Do
No
Create various section views and vary the offset distance to see how the side faces of the part are oriented. Also, edit the sweep and show the intermediate sections. Examine how they are oriented with respect to the path and guide curves.
8
204
Save and close the part.
SolidWorks 2012
Lesson 6 Advanced Sweeping
Control Twist with Guide Curves
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Above we have seen eliminating twist using guide curves and settings. Next we explore inducing controlled twist and other uses for guide curves.
When creating a profile sketch for a sweep that you know is going to have a tendency to twist, it is a good idea to avoid Horizontal, Vertical and any external sketch relations other than Pierce. This is especially true for lines that go between the path and guide curves. When a sweep section twists, horizontal and vertical relations may cause the sketch to fail because they can not be solved in one or more of the intermediate positions.
Sketch Relations
But if relations like Parallel and Perpendicular are used, the sketch is allowed to move and rotate independently from the sketch plane itself. This often makes the difference between a sweep that works and one that does not.
1
Open the part Guide_Curves. In the part are a profile sketch and three curves.
Do
No
Second guide curve
Profile
First guide curve
Path
205
Lesson 6
SolidWorks 2012
Advanced Sweeping
2
Predicting twist.
We can predict twist by showing the curvature combs of the path. However, Show Curvature Combs does not work on a projected curve, which is what the path is. So we need to make a copy of it as a spline.
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Open a 3D sketch. Select the path, Curve2, and click Convert Entities. This creates a copy of the curve as a spline. Right-click the spline and click Show Curvature Combs.
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This graphically shows how the path twists which in turn will cause the profile to twist as it is swept.
Do
No
Exit the sketch discarding the changes.
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SolidWorks 2012
Lesson 6 Advanced Sweeping
3
Start the Sweep feature. Select Profile to be used as the sweep profile.
Select Curve2 for the path.
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The sweep follows the path, but it also twists in a way that for this part, is not useful.
4
Path alignment.
Expand Options and set the Path alignment type to Minimum twist.
This eliminates some of the twist but the result is still not acceptable. Select the first guide curve. Select Curve1 as the first guide curve.
Do
No
5
Notice how the end of the sweep is distorted. This is because of Horizontal and Vertical sketch relations in the profile.
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Lesson 6
SolidWorks 2012
Advanced Sweeping
There are two ways to fix this problem: I I
Change the Orientation/twist type option. Expand Options and under Orientation/twist type, click Follow path and 1st guide curve.
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6
Change the Orientation/twist type option. Edit the profile sketch and remove the problematic horizontal and/ or vertical relations, replacing them with parallel or perpendicular.
This straightens out the sweep because the intermediate sections are no longer relying on just the path to determine their orientation. Using the Follow path and 1st guide curve option, the twist orientation of each intermediate section is determined by a vector between the path and the first guide curve.
No
Vector that controls orientation
Do
The option Follow 1st and 2nd guide curves uses the same concept, except that the alignment is defined by a vector between two guide curves instead of between the path and first guide curve.
208
7
Add a second guide curve. Add Curve3 as the second guide curve. The order
of the curves listed in the list box is important, especially if using one of the Orientation/Twist type options that uses guide curves. The order can be changed by using the arrows on the left side of the selection list.
SolidWorks 2012
Lesson 6 Advanced Sweeping
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This curve controls the height of the sweep as it moves along the path. In this example, the height of the section affects the radius of the arcs on the top of the profile sketch. This is done with construction geometry and an Equal relation.
Click OK.
8
An alternate method for straightening out the sweep is to edit the Profile sketch, remove the problematic Horizontal and Vertical sketch relations, and replace them with Parallel and Perpendicular as appropriate.
Do
No
Alternative Method
Results.
With this approach you would not use the Follow path and 1st guide curve option but you would still use the guide curves.
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Lesson 6
SolidWorks 2012
Advanced Sweeping
9
Edit the Profile sketch.
View the sketch relations.
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Select the two Vertical relations and delete them.
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Delete these relations
10 Add relations.
Select the construction line and the long sketch line as shown in the illustration at the right.
Add a Perpendicular relation.
Select these lines
11 Add relations.
Select the two construction lines as shown. Add a Parallel relation.
12 Exit the sketch.
Do
No
13 Edit the Sweep1 feature. Change the Orientation/twist type to Follow Path and the Path alignment type to Minimum twist.
210
Select these lines
SolidWorks 2012
Lesson 6 Advanced Sweeping
Neither technique is really better than the other. Best practice is to avoid using Horizontal and Vertical relations in the profile sketch, using Parallel and Perpendicular instead. That’s good sketching technique for sweeps that follow 3D paths. And, use guide curves together with the Orientation/twist type options to control twist – either to induce it or to eliminate it. To really master sweeping along 3D paths, you need to be comfortable employing both techniques.
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Best Practice
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14 Add shell and fillet features to complete the part. I Fillet radius = 0.150” I Wall thickness = 0.150”
15 Save and exit the part.
Twist along Path
Use the Twist along Path option to twist any sweep. It can also be used to prevent sweeps from twisting, by setting the amount of twist to zero.
No
Twist along Path can be used on
Do
complex 3D spline paths (far right image) as well as on straight line paths (near right).
211
Lesson 6
SolidWorks 2012
Advanced Sweeping
The twist can be defined by a value of Degrees, Radians or Turns along the entire length of the path.
Defining Twist
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Path
Profile
Open the part Twisted Ring. It contains two sketches:
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1
I I
2
Sketch2 is the Profile Sketch3 is the Path
Sweep. Click Cut Sweep
and create a simple cut sweep using the default Follow Path option.
3
Edit Cut-Sweep1 feature. Edit the Cut-Sweep1
No
feature and set the
Orientation/twist type to Twist Along Path.
Do
Use Define by: Turns and 15 turns.
212
Click OK.
SolidWorks 2012
Lesson 6 Advanced Sweeping
4
Completed.
You are probably wondering what the option Align with End Faces is used for. Consider this simple example. Suppose you wanted to create a cut by sweeping a profile along the edge of a model as illustrated at the right.
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Align with End Faces
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Complete the model by adding a R0.013”fillet to the edges of the cut feature.
If you use Align with End Faces, the cut continues all the way through to the end face of the model. This is similar to the Through All end condition used in extruded features. This is usually desirable and is why this option is selected by default – when you are sweeping a cut.
No
If you do not use Align with End Faces, the cut terminates when the profile reaches the end of the path, leaving a small lip of uncut material.
Do
The reason we did not use Align with End Faces when sweeping the threads is there
Sweeping Along Model Edges
were no end faces for the boss to align with. Using it in that case could have forced the system to give an incorrect result. Fortunately, Align with End Faces is deselected by default when sweeping a boss. There is something else this example shows: model edges are valid entities for a sweep path. They can be selected directly, without copying them into a sketch.
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Lesson 6
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Advanced Sweeping
When you select a model edge as a sweep path, an additional option becomes available in the Sweep dialog. This option is Tangent propagation and it serves the same function as the similar option in filleting. If you select a single segment of the edge, this option causes the sweep to continue along the adjacent, tangent edges.
What if the Edges Aren’t Tangent?
Consider a situation where you want to run a swept feature around a number of edges, not all of which are tangent. The Sweep Path selection list only accepts one selection if you use the conventional method of selecting it in the graphics window. Use the SelectionManager to select all the edges as a closed loop.
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Propagate Along Tangent Edges
1
2
Open the part align end faces.
Sweep the cut.
Click Swept Cut Cut, Sweep.
or click Insert,
Select the circle as the Profile.
3
SelectionManager.
Do
No
Right-click in the graphics area and click SelectionManager from the shortcut menu.
214
Click Select Group and select the uppermost edge that coincides with the center of the profile circle. Click the Tangent icon
.
The system selects the tangent chain of edges.
SolidWorks 2012
Lesson 6 Advanced Sweeping
4
Remaining edges.
Next select the remaining edges to complete the path.
This completes the definition of the group.
Preview and results.
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5
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Click OK using the right mouse on the button , or click OK SelectionManager.
Click OK.
Save and exit the part.
No
6
Sweeping a Tool Body
You can sweep a solid tool body along a path to make a swept cut using the Solid sweep option. One common application is creating cuts around cylindrical bodies such as on a drill bit.
Do
The Solid sweep option has some specific requirements: 1. It is only available for swept cuts. 2. The tool body must: I Be a revolved feature. I Contain only analytical geometry (lines and arcs). I Not be merged with the model. 3. The path must be tangent within itself (no sharp corners) and must begin at a point on or within the tool body’s profile.
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Lesson 6
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Advanced Sweeping
Open the part Drill_Bit.
The part consists of two disjoint solid bodies: I I
2
Tool body
One representing the body of the drill bit. One representing the tool that will cut the flutes.
Examine the geometry.
Drill body
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The path is a helix defined by a circle that was sketched on a plane that is parallel to the Front reference plane and coincident with the vertex at the tip of the drill body.
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1
The sketch for the revolved tool body is on a plane that is normal to the path and coincident with the end of the path. There are two relations on the lowermost end of the construction line:
I I
Coincident to the arc Pierce to the path
Do
No
The angle of the sketch is controlled by the 1mm dimension between the construction line and the vertex of the drill body.
216
Path
SolidWorks 2012
Lesson 6 Advanced Sweeping
3
Sweep the cut. Click Swept Cut
or click Insert, Cut, Sweep.
Under Profile and Path, click Solid sweep. Select the tool body as the Profile.
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Select the helix as the Path.
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Under Options you can click Show preview, although it is off by default because generating the preview is fairly time consuming.
Click OK.
4
Results.
The results of the sweep are shown at the right. The tool body is absorbed into the resulting sweep feature.
5
Circular pattern.
Make a circular pattern of the cut sweep feature. Use the cylindrical face of the drill bit body as the Pattern axis.
No
Use two instances evenly spaced through 360°.
Do
The results are shown below using RealView graphics.
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Lesson 6
SolidWorks 2012
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Advanced Sweeping
Save and close the part.
Do
No
6
218
SolidWorks 2012
Exercise 22 Makeup Case
Exercise 22: Makeup Case
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This is a concept model for a cosmetics case such as one that powder or rouge would be packaged in. As such, it is a single, monolithic solid with no internal components or details, much like the USB flash drive you worked on in Exercise 10: Split Part on page 96.
Thanks to Keith Pedersen at Computer-Aided Products, Inc. for submitting this example.
This lab reinforces the following skills: I
Split Line on page 190.
I
Sketch Blocks on page 161.
I
Orientation and Twist Control on page 196.
Units: millimeters
Procedure
Use the following procedure:
Open the part Makeup Case. This part represents the conceptual design of the product.
No
1
Do
2
Edit sketch.
Edit the Groove Path sketch. Use Fit Spline to convert the two lines and the arc to a spline.
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Exercise 22
SolidWorks 2012
Makeup Case
3
Split line.
Use the active sketch to spit the uppermost face of the solid.
The challenge is to sweep the profile and maintain the correct orientation with respect to the uppermost face of the part. 4
Reference plane and sketch.
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Create a reference plane normal to the end of the split line.
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This edge will be the sweep path for the groove.
Open a sketch and insert the block named Groove Profile located in the Exercises folder of this lesson.
5
Add relation. Add a Pierce relation between the split
line and the sketch point in the block.
6
View normal to.
Change the view so it is normal to the sketch and zoom in on the sketch block.
No
Drag the block. See how it is free to rotate with respect to the split line (the sweep path)? This is the degree of freedom you must control in order to successfully sweep the profile.
Do
7
220
Add relation.
Add a Coincident relation between the split line and the end of the construction line (center of the arc). Exit the sketch.
SolidWorks 2012
Exercise 22 Makeup Case
8
Sweep a cut.
Sweep a cut using the default settings: I I
View the results.
The results are not good. The profile twists as it moves along the path, distorting the shape of the groove. 10 Edit feature.
Edit the sweep feature and change the Path alignment type to All Faces.
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This causes the profile to maintain the proper orientation along the path.
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9
Orientation/twist = Follow Path Path alignment type = None
11 Mirror.
No
Mirror the swept cut with respect to the Front reference plane.
Do
12 Save and close the part.
221
Exercise 23
SolidWorks 2012
Mouse
Exercise 23: Mouse
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This is a concept model for a computer mouse. As such, it is a single, monolithic solid with no internal components or details. The task is to create a reveal using a swept cut feature.
This lab reinforces the following skills: I
Orientation and Twist Control on page 196.
I
Control Twist with Guide Curves on page 205.
I
Sketch Relations on page 205.
Units: millimeters
Procedure
Use the following procedure:
1 2
Open the part Imported Mouse. This part represents the conceptual design of the product. Sweep the cut.
Do
No
Sweep a 0.5mm square profile along the edge of the model to create the reveal, shown in orange below. Try to complete this exercise without referring to the answer on the following pages.
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SolidWorks 2012
Exercise 23 Mouse
Answer
If you were not able to control the twisting of the profile to create a satisfactory sweep, follow the steps below. 1
Composite curve.
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Create a composite curve using the edges of the mouse. This will be the guide curve.
Because of the shape of the path, you can anticipate that the profile will tend to twist when it is swept. This means two things: I I
2
Avoid horizontal and vertical relations in the profile sketch Use a guide curve
Create the guide curve.
The guide curve has to be created before the sweep profile so you can relate the profile to it. Open a sketch on the Top reference plane.
Do
No
Use Convert Entities to copy the edges of the mouse into the sketch.
223
Exercise 23
SolidWorks 2012
Mouse
3
Sketch the sweep profile. Open a sketch on the Right
Sketch a 3 Point Corner Rectangle and make it a square by adding an Equal relation between two adjacent sides. This is an easy way to avoid unwanted horizontal and vertical relations. 4
Pierce relations.
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Sketch a centerline and add a Colinear relation between it and the side of the square.
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reference plane.
Add Pierce relations between the corner of the square and the composite curve, and between the bottom end of the centerline and the guide curve.
5
Dimension. Add a 0.5mm dimension to one
side of the square.
Sweep the cut using the guide curve.
Do
No
6
7
224
Save and close the part.
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Lesson 7 Lofts
Upon successful completion of this lesson, you will be able to: Create a boss by lofting between profile sketches.
I
Model complex shapes using advanced lofting techniques.
I
Use Split Entities to divide a sketch curve.
I
Use the Deviation Analysis tool to compare faces along edges.
Do
No
I
225
Lesson 7
SolidWorks 2012
Lofts
Both sweeping and lofting are capable of creating complex shapes. Which tool you use to build a particular part depends primarily on what design information you have to work with. There are also some general differences between sweeping and lofting that will influence which method to use. In essence: I I
Sweeping uses a single profile sketch. Lofting uses multiple profile sketches.
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Lofting and Sweeping: What’s the Difference?
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Consider the first feature of a plastic bottle such as the one we worked on in Lesson 4: Introduction to Sweeping. If the design data you are working with consists of the two curves that describe the outline of the bottle as seen from the front and side, and the cross section is similar throughout the shape, you can create the feature using sweep, with guide curves controlling the major and minor axes of the elliptical section.
If the design data you are working with consists of a set of cross sections, you can use loft to build the part. This is especially useful when the cross sections are dissimilar, although that is not the case in this example.
Do
No
Starting with this? Use Sweep.
226
Starting with this? Use Loft.
SolidWorks 2012
Lesson 7 Lofts
It may be helpful to think of extrudes and revolves as being analogous to lines and arcs, and lofts being analogous to splines. In the same way that splines interpolate curves between points, lofts interpolate surfaces between profiles.
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How Lofting Works
Spline interpolated through points
Surface lofted through profiles
This explains why if you start with four profiles like this:
No
You end up with this:
Do
Instead of this:
227
Lesson 7
SolidWorks 2012
Lofts
Lofting enables you to create features that are defined by multiple crosssectional profiles. The system constructs the feature – a boss, a cut or a surface feature– by building the feature between the sketches. Lofts and sweeps are often referred to as interpolating features because they interpolate face geometry between the profiles.
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Basic Lofting
Do
No
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We are given the dimensions of the bottom, top, and an intermediate section of this part, as well as its height. This sort of problem lends itself very well to lofting.
228
SolidWorks 2012
Lesson 7 Lofts
Stages in the Process
The major steps in this operation are: I
Create the profiles.
I
Optionally create guide curves.
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Loft profiles may be made from 2D or 3D sketches, edges, curve features or faces. For best results the profiles should be made up of the same number of entities and you should give some thought to how the entities will map one to the other during the loft. To save time, the sketches have already been created for this example. Guide curves can optionally be used with lofting to give more control over the transitions between the profiles. I
Insert loft between profiles.
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Where you select each profile and the order in which you select them is important.
Introducing: Loft
Inserting a Loft creates a boss, cut or surface using profiles and optionally, guide curves. The loft is first created between the profiles and optional guides provide additional control over how the shape in between the profiles is generated.
Where to Find It
I I I I
Procedure
CommandManager: Features > Lofted Boss/Base CommandManager: Features > Lofted Cut Menu: Insert, Boss/Base, Loft Menu: Insert, Cut, Loft
Consider the following procedure:
1
Open the part Defroster Vent.
Do
No
It contains three profile sketches as shown.
2
Insert a loft.
Click Lofted Boss/Base
.
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Lesson 7
SolidWorks 2012
Lofts
3
Loft PropertyManager. Click in the Profiles list and select the three
sketches in the graphics window. You should pick in roughly the same location on corresponding entities in each sketch. When lofting three or more sketches they have to be in the proper sequence. If the profiles are not in the correct order in the list, you can reposition them using the Up and Down buttons.
Tip
Although Show preview improves visualization as you select the profiles, with complex shapes, the preview tends to slow the system response. Loft connectors.
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4
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Note
As you select the sketches, the system generates a connector showing which vertices on the sketches will be connected during the loft. Pay close attention to this connector because it will show you if the loft is going to twist, and it will enable you to correct twists or selection errors just by dragging the dot. A callout also appears to identify the profiles.
Click Thin Feature.
No
5
Do
Set the Thickness to 0.090 inches. Make sure the thickness is added to the outside of the profiles.
230
Under Options, click Merge tangent faces. Click OK to create the feature.
SolidWorks 2012
Lesson 7 Lofts
Merge Tangent Faces
6
Edit the feature.
Edit the definition of the loft feature. Under Options, clear the Merge tangent faces
option and click OK.
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Notice that the edges that corresponded to the ends of the lines and arcs in the profiles are now visible. Compare this to the results in step 5.
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The Merge tangent faces option causes the surfaces in the loft feature to be tangent if the corresponding segments in the profiles are tangent. Faces that can be represented as planes, cylinders, or cones are maintained. Other adjacent faces are merged, and the sections are approximated. Sketch arcs may be converted to splines.
7
Start and End Constraints
Turn Merge tangent faces back on.
When lofting, you can control the shape at the ends of the loft by using options that influence the direction of the loft at the beginning and ending profiles. You can also control the length and direction of the influence at each end.
8
Edit the feature.
Edit the definition of the loft feature. Expand the Start/End Constraints group box.
Do
No
The Default tangency condition approximates a parabola scribed between the first and last profiles. The tangency from this parabola drives the loft surface, which results in a more predictable and natural loft surface when matching conditions are not specified.
Start/End Constraints = Default
Start/End Constraints = None
231
Lesson 7
SolidWorks 2012
Lofts
9
Normal to Profile. Select the options Normal to Profile for both the start and end of the
loft. The tangent vector arrows should point in the directions shown. If they do not, click Reverse Direction
to reverse the direction.
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Leave the start and end tangent length values at the default 1. Changing the tangent length changes the influence on the shape of the loft.
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You can change all the Tangent Length values by typing a value and clicking Apply to all. Individually, a single tangent vector arrow can be dragged.
Do
No
Pay attention to the preview. If the tangent arrows are in the incorrect direction, the preview will look something like the illustration below.
232
Click OK.
SolidWorks 2012
Lesson 7 Lofts
The result is that the shape of the loft is altered so that the faces of the feature start and end normal (perpendicular) to the plane of the profile sketches. The Draft Angle option with
Note
Normal to Profile
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10 Results.
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applies draft with respect to the planes of the profiles. If it is used with the Direction Vector option, the draft is applied with respect to the direction vector.
11 Save and close the part.
Instead of several 2D sketches, one for each section of the loft, you can create everything in a single 3D sketch. Use the SelectionManager to select each loft section within the 3D sketch. Since a solid model requires closed loft sections, you should use Select Closed Loop .
Do
No
Lofting Using a 3D Sketch
Examine the part Defroster Vent - 3D Sketch to see an example of lofting using a 3D sketch.
233
Lesson 7
SolidWorks 2012
Lofts
Merging a Multibody with Loft
The Merge result check box can be used on any boss feature aside from the first feature. In this example, we will create the transitional feature from the head of a golf club into the shaft using a multibody. Open the part Lofted Merge. It contains two solid bodies that cannot be merged.
2
Insert a loft feature.
Insert a loft feature between the planar faces of the two bodies.
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Select the faces in similar areas.
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1
3
Start/End constraints.
Change the two tangency options to Tangency To Face for the selection on the head and Normal to Profile for the selection on the shaft. The Next Face button is used to resolve any ambiguity as to which set of faces is used.
Merge result must also be
checked.
Note
The option Curvature To Face could be used in place of Tangency To Face to make the faces match in curvature.
4
Merged feature.
Do
No
Once the feature is added, the part contains only one solid.
234
SolidWorks 2012
Lesson 7 Lofts
Using Derived and Copied Sketches
Lofted features may have many sketches to describe the Profiles, Guide Curves or Centerlines. Many of the sketches may be similar or exactly the same. Derived and copied sketches can help reduce the amount of sketching required. exact duplicates of the original sketch and retain the link from the original to the derived. They can only be placed, not changed. Copied Sketches are also duplicates of the original sketch but can be changed in any way. There is no link back to the original.
Original Sketch Copied Sketch
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I
Derived Sketches are
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I
Consider a decorative shape Derived Sketch like the one shown in the illustration. Two sketches of the loft are the same (the original sketch and derived sketch) while the third is similar, but not identical.
1
Open the part Derive&Copy.
It contains a single sketch named Source.
To create another profile of similar shape, copy and paste the existing sketch onto the desired sketch plane. Copied sketches can be edited in any way and are not linked back to the original. In this example, the sketch Source will be copied onto the plane Right and edited.
No
Copying a Sketch
Do
2
Select sketch.
Select the sketch Source. The sketch geometry will highlight on the screen.
3
Copy sketch.
Using Ctrl+C, or Edit, Copy, copy the sketch to the clipboard.
235
Lesson 7
SolidWorks 2012
Lofts
Select plane and paste. Select the Right plane from the
FeatureManager design tree and press Ctrl+V, or click Edit, Paste. The sketch will be pasted from the clipboard to the selected plane. It will appear on the screen in the plane’s orientation.
5
Edit sketch.
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4
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Select the new sketch and click Edit Sketch. Use Tools, Sketch Tools, Modify to rotate and move the sketch geometry. Relations and dimensions will be needed to fully define the sketch.
6
Add relations.
No
Add relations between the profiles to fully define the sketch.
Do
7
Make changes.
Make some changes to the dimensions in the sketch. Change the bold, red, underlined dimensions as shown. Note that two of them are also changed from Diameter dimensions. Exit the sketch and rename it Copied.
236
SolidWorks 2012
Lesson 7 Lofts
Derived Sketches
A Derived Sketch is used to create a copy of the Source sketch on a different plane and location. The derived sketch will be a child of the original sketch.
Introducing: Insert Derived Sketch
Insert Derived Sketch is also used to create a copy of a sketch.
Where to Find It
I
Creating a Derived Sketch
Create the derived sketch on the plane Top. Once copied, the sketch can be rotated and repositioned if it is at the wrong orientation.
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Menu: Insert, Derived Sketch
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Derived sketches are dependent on the original for size and shape but not location and usage. You cannot edit the geometry or dimensions of a derived sketch. You can only locate it with respect to the model. Changes to the original sketch propagate to the derived copies.
8
Select sketch and plane.
Hold down Ctrl and select the sketch Source and the plane you want it copied to (Top). The sketch will be copied to the selected plane in the next step.
9
Insert a derived sketch.
Click Insert, Derived Sketch. The sketch is inserted onto the selected plane, but it is under defined. Unlike Copy and Paste, the system automatically puts you into the Edit Sketch mode. Also, notice that derived sketches are identified as such by the derived suffix appended to their names in the FeatureManager design tree.
Locating the Derived Sketch
Derived Sketches are inserted under constrained and often out of
orientation.
10 Modify the sketch. Click Modify Sketch
No
. Position the cursor over the black origin symbol as indicated.
Before
Do
Click the right-mouse button to mirror the sketch.
After
237
Lesson 7
SolidWorks 2012
Lofts
11 Drag.
12 Fully define.
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Add relations between the profiles to fully define the sketch.
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Move the sketch to the right and close the Modify Sketch dialog.
13 Insert a loft. Click Loft Boss/Base
. Click Merge tangent faces.
Do
No
Loft the three profiles without using guide curves or centerlines. Select the profiles near a common vertex.
238
SolidWorks 2012
Lesson 7 Lofts
Loft Viewing Options
When you are creating or editing a loft feature, you can enhance the preview by displaying Connectors, Mesh, or Zebra Stripes.
Where to Find It
I
Faces I
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I
Shortcut Menu: Right-click in the graphics window and click Show All Connectors or Hide All Connectors Shortcut Menu: Right-click in the graphics window and click Mesh Preview, Mesh All Faces or Mesh Preview, Clear All Meshed Shortcut Menu: Right-click in the graphics window and click Zebra Stripes Preview
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14 Show All Connectors. Right-click Show All Connectors to view
connections between all the profile endpoints.
Right-click Hide All Connectors.
15 Mesh Preview. Right-click Mesh Preview, Mesh All Faces. A surface
mesh overlays the shaded preview.
Right-click Mesh Preview, Clear All Meshed Faces. Click OK.
Do
No
16 Save and close the part.
239
Lesson 7
SolidWorks 2012
Lofts
Centerline Lofting
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The part shown at the right is a heat shield that goes over a hot gas manifold. It consists of several shapes – a semi-circle, a rectangle, a half ellipse – all of which must be smoothly blended together. Since the basic shapes are the result of blending two or more profiles, lofting is the approach of choice.
Open the part Heat Shield. To save time, we will start with this part that already has the basic geometry defined.
Do
No
1
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SolidWorks 2012
Lesson 7 Lofts
Preparation of the Profiles
When lofting, you have to give special consideration to the way you sketch the profiles, and how you subsequently select them in the Loft command. In general, there are two rules you should follow for good results: I
Pick the same corresponding spot on each profile.
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The system connects to points you pick. If you are careless, the resulting feature will twist.
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If the profiles are circles there are no ends to pick such as there are on rectangles. That makes picking corresponding spots tricky at best. In this situation, put a sketch point on each circle and pick them when you select the profiles.
I
Each profile should have the same number of segments.
In the example at the right, a closed semicircle (2 segments) was lofted to a rectangle (4 segments). As you can see, the system blended one side of the rectangle into part of the arc, another side into the remainder of the arc, and so on. This does not give a good result. You have two options: I I
Insert a loft. Click Loft Boss/Base
, or click Insert, Base, Loft.
Do
No
2
Interactively add or move connector points during the Loft command. Subdivide the arc manually so you can control exactly which portion of the arc corresponds to each side of the rectangle.
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3
Preview. Select Sketch6 and then Sketch4. Notice the
preview. Be careful to pick the same relative corner of each profile.
4
Centerline.
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Expand the Centerline Parameters group box.
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Because of the importance of where you pick the profiles, it is usually not a good idea to select them from the FeatureManager design tree.
Tip
Select the centerline (Sketch3).
Use Normal to Profile for both the start and end constraints. Click OK to create the feature. Results.
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No
5
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Sharing Sketches
Sketches that have been absorbed when used to create extrudes, revolves, sweeps and lofts can be used again to create additional features. They can simply be selected from the FeatureManager to become part of the new feature. Insert another loft.
Show Sketch4. (It is absorbed into the loft feature.) Loft between Sketch5 and Sketch4. Use Sketch2 as the Centerline.
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Use Normal to Profile for both the start and end constraints.
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6
7
Shared sketch. Sketch4 is shared by both
loft features, as indicated by the name and the symbol. Editing the sketch would change both features. Unfortunately the loft shape, although valid, is not desirable. The fact that the profiles have different numbers of edges adversely influences the shape of the feature.
Show Connectors. Right-click the Loft2 feature and click Edit Feature. Right-
click in the graphics area and click Show All Connectors. Colored circles appear at the endpoints of the segments of the profiles. Notice that a connector has been added to the semicircular profile. This is because both profiles must have the same number of segments. If you did not sketch them that way, the system breaks them for you.
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8
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9
Synchronize the profiles.
Drag the connectors to improve how the rectangular profile maps to the semicircular profile.
10 Results.
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Although dragging the connectors is very interactive, it may not be precise enough for some applications. If precise control is needed over how the profiles map to each other, you should manually subdivide the profile.
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Click OK to rebuild the feature.
11 Delete.
Delete the Loft2 feature and use a modified sketch with an equal number of segments.
12 Recreate the sketch. Select Plane4 and open a
sketch.
No
Select Sketch4 and click Convert Entities to create copies of the arc and line in the sketch.
Split Entities breaks a single sketch curve into multiple pieces at
Where to Find It
I
Do
Introducing: Split Entities
244
selected locations.
I
Menu: Tools, Sketch Tools, Split Entities Shortcut Menu: Right-click a sketch segment and click Split Entities
SolidWorks 2012
Lesson 7 Lofts
13 Split entities.
Divide the arc into three pieces by using Split Entities at two locations along its length.
Split Points
All three arcs are coradial but their arc angles are under defined. 14 Angular dimensions. Dimension the arcs at 35°
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using 3 point angular dimensions. If you want, you can make the values of the angles equal using a global variable. This way, when you change one, they both change.
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Position the breaks on either side of the center.
15 Exit the sketch. 16 New Loft.
Create a second centerline loft between Sketch5 and the new four-sided sketch using the centerline curve.
Use Normal to Profile for both the start and end constraints.
Right-click Show All Connectors to display the matching endpoints.
No
17 Results.
Do
The second loft merges into the first, forming a single solid.
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Lofts
Sometimes with sweeping and lofting the model ends up with unwanted artifacts – faces from one feature that protrude through another feature. Generally these artifacts should be removed. One way to make it easier to spot these artifacts is to make the features contrasting colors.
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Cleaning Up a Model
Artifact
Changing the display to Shaded With Edges also helps make artifacts more visible.
The Delete Face tool removes one or more faces from the model, allowing it to be replaced by extending the boundaries of adjacent faces or by filling in the gap with a completely new surface. Delete Face can also turn a solid body into a surface body by simply removing the face and not replacing it with anything.
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Introducing: Delete Face
Where to Find It
I I
CommandManager: Surfaces > Delete Face Menu: Insert, Face, Delete Face
18 Change colors.
Change the appearance of the two loft features, making them contrasting colors.
Tip
Increase the image quality to make it easier to see the artifacts.
19 Delete face. Click Delete Face
.
Click Delete and Patch.
No
Zoom in on the edge of the flat face where the two loft features meet.
Do
Select the artifact faces. Some are very tiny, sliver faces.
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Artifact faces
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Lofts
Click OK.
20 Remove color.
Remove the colors you assigned in step 18.
Introducing: Deviation Analysis
The Deviation Analysis tool can be used to determine the angular difference between faces along common edges. A 90° value indicates perpendicular faces, 0° indicates tangency.
and select the model edge shown. Set the number of sample points slider control to halfway.
Do
No
Click Calculate.
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22 Deviation Analysis graphics.
The results of the deviation analysis appear as pairs of 3D arrows on the edge. They are color coded to show the change in angle between the faces along the common edge.
A Face Fillet is created between selected faces, instead of on selected edges as with the default fillet type. Face fillets are generally used when the edge between two faces is not as perfect as you would like it to be. As we saw with the deviation analysis, the angle between the faces joined by the edge highlighted in the illustration at the right transitions from 90° to 0°. This is sometimes called a degenerate edge and they can be problematic when it comes to filleting. This is because of very slight irregularities caused by the interpolation of the lofted faces. The best approach for filleting this type of edge is to use a face fillet.
Do
No
Face Fillets
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The color settings used for the arrows can be changed.
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23 Face fillet. Click Fillet
.
Click Face fillet. Click in the Face Set 1 selection list to activate it. Select the face on the top of the Loft2 feature. Click in the Face Set 2 selection list to activate it.
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Select the face on the side of the Loft2 feature.
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Set the Radius to 25mm.
Click OK.
24 Second face fillet.
You cannot fillet disconnected edges using a face fillet. Therefore a second face fillet is required on the degenerate edge on the opposite side of the Loft2 feature.
25 Remaining fillets.
You can use a multiple radius fillet if you wish, or create two separate fillets.
No
Run a 25mm fillet down the remaining sharp edge of the Loft2 feature. This can be a regular edge fillet; it does not have to be a face fillet.
Run a 55mm radius fillet up the edge between the two lofts.
Do
Note Tip
Fillets shown in color for clarity. If you have difficulty creating the 55mm fillet, edit the first loft feature and under Centerline Parameters, increase the Number of sections by dragging the slider slightly to the right.
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26 Create an offset plane. Create a plane offset 100mm from the Top reference plane.
27 Sketch profile.
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Sketch a rectangular profile as shown.
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This will be used to sketch the profile of the rectangular inlet tube.
Fillet the corners with sketch fillets.
The profile is centered left-toright with respect to the Origin.
28 Extrude.
Extrude a boss using the end condition Up to Next, and 5° of Outward Draft.
29 Add fillet. Run a 12.5mm radius fillet around
Do
No
the base of the boss.
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30 Shell part.
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Shell the part towards the inside using a wall thickness of 1.5mm.
31 Save and close the part.
Advanced Lofting
Many shapes found in industrial products fall into the complex shapes category. This lifting hook is one of them. There are no flat surfaces, and the only identifiable feature is the revolved loop on top. To help determine where to start building, make a list of the information you have: I I
No
I
Design requirements Sizes Materials Manufacturing processes The application in which it will be used
I
Do
I
This may not answer all the questions for you, but it will give you a start.
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Lofts
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In this case, we have a picture of a similar part we are to design around, and know that the inside diameter of the top loop is 1.25” and the cross section of the loop has a diameter of 0.750”.
Planning a Modeling Strategy
Before tackling a part like this, it is a good idea to plan out the task. Placement of the origin is one of the first things that should be considered, since it can be important to downstream tasks such as mating in an assembly. In this case, the origin could go at the center of the top loop or at the center of the hook throat. There may be other valid locations but these are two examples. Next you should try to identify functional shapes on the part. For example: I I I I
The loop The hook The transition between the hook and the loop The tip on the end of the hook
Loop
Transition Tip
Each one of these functional shapes will present its own modeling challenge.
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No
Hook Once you have identified the functional shapes, it may become easier to assign features to make each shape. The loop is most easily created as a revolve. A transition from one shape to another is a good description of a loft, so we will use a loft for the transition area. The hook could be created with either a loft or a sweep, but a loft will be easier to set up to get the desired shape. Again, there are several ways to make the tip, but here we will create it with a loft.
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Lesson 7 Lofts
Layout sketches are frequently used when creating complex models. A layout sketch is a regular 2D or 3D sketch used as either a visual reference or as a parametric reference for the rest of the model.
Procedure
To simplify matters somewhat, this part has been partially set up for you. 1
Open the part Hook. It contains the following:
Hook Layout Sketch. The Hook Layout Sketch has been partially created for you. You will finish it. Sketch Picture. The Hook Layout Sketch has a sketch picture in it for you to trace around and to help align sketches and features. Loft Profile Sketch. This is a sample sketch to get you started. Loft Profile Planes. Several loft profile planes have been created for you.
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Layout Sketches
I
I
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Now you are ready to use a spline to trace the back side of the hook. Edit Hook Layout Sketch. Create a second spline around the outside curve of the main hook body. It will take some adjustment to get it close to the sketch picture image. The purpose of this spline is to help you set up the loft which will form the main part of the hook body.
First Profile Plane
Do
No
2
Overbuild the spline by one or two spline points on both ends, and do not be concerned about the transition to the loop or the tip. Overbuilding and trimming back will help us get the correct curvature at the end of the shape. The new spline should extend past the First Profile Plane.
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3 4
Exit the sketch. Open a new sketch.
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Open a new sketch on the First Profile Plane. This will help the loft begin the transition shape even though at this point we aren’t yet starting to build the transition feature.
Sketch an ellipse whose major axis is pierced on both ends by the splines of the layout sketch, and whose minor axis is 1” wide. 5
Exit and rename the sketch.
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Name the sketch First Profile.
6
Suppress the sketch picture.
Expand the Hook Layout Sketch in the Feature Manager design tree.
Right click Sketch Picture1 and click Suppress from the shortcut menu.
7
Edit the Second Profile sketch.
Constrain the two points of the proportional spline which lie on the axis of symmetry to the layout sketch splines using the Pierce relation.
Note
This sketch was created by mirroring a proportional spline and using Fit Spline to join the original and the mirrored copy.
8 9
Exit the sketch.
Copy and paste the profile.
Do
No
We are going to use this same profile for several of the loft sections. Because it is a proportional spline and the distance between the guide curves changes, the sketch will stretch to fit between the curves. Select the Second Profile sketch from the FeatureManager design tree and press Ctrl+C. Select the Third Profile Plane, and press Ctrl+V. Repeat this for all the remaining planes except Seventh Profile Plane. Notice that the last sketch that was pasted is not where it belongs. We will fix this as we edit each profile.
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10 Edit the copied sketches. Edit Sketch2.
Constrain the same points in the same way as in step 7, using the Pierce relation.
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Do this for all of the remaining sketches except the last copy.
Notice that the sketches grow in width as they grow in length. Also notice that the fit spline looks black on top of a blue proportional spline. The sketch is still under defined until both Pierce relations are applied.
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11 Reposition the sixth profile sketch. Edit the sketch. Notice that Sixth Profile Plane
crosses both guide curves twice. If you apply a
Pierce relation, between a sketch and a guide
curve, it may go to the correct location and it may not, depending on which is closer. To make sure the Pierce relation snaps to the correct location, move the point you want to pierce so it is close to the location you want it to snap to. Use the same technique for both ends.
Tip
Add the Pierce relation at the end that is already in the correct position. Then, drag the other end of the centerline (the axis of symmetry) to rotate the profile into position. Now add the second Pierce relation.
12 Create the last profile sketch. The last profile sketch is on Seventh Profile Plane, and is again an ellipse, with a width of 0.6”.
Do
No
At this point, the sketching for the main hook body loft is complete.
Because portions of this example have been set up ahead of time, the construction of the rest was relatively easy. In real projects you should expect this process to take more time. As you gain experience with the techniques, your speed to model complex shapes will increase.
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Lofts
13 Create the loft feature.
We are using closed loop splines and ellipses, so each profile only has a single entity. Still, it is best practice to select each profile in approximately the same location.
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First, select all the profiles, and make sure the preview is showing you approximately what you expected to see.
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Also, on models that turn through a large angle such as this one, sometimes SolidWorks will automatically reorder the loft profiles. If the profiles are lofted in a different order, the feature will likely fail. One way to see this quickly is if you notice the connector lines showing in a way that doesn’t match your intent. Notice that the loft preview doesn’t quite match the guide curve sketches at this point. This is an important thing to observe when setting up a loft. If you try to modify a loft too much with a guide curve, the loft may fail. In this case, the natural loft is reasonably close to what we want the end shape to be, so it is likely to work. Do not click OK.
14 Select the guide curves.
Select the spline to the outside of the hook, the one that you have drawn, as the first guide curve.
Do
No
When you begin to select the guide curves for the loft, the SelectionManager will appear on the screen.
In the SelectionManager, click Select Open Loop , and click the right mouse button OK , or, click OK on the SelectionManager. Select the inner guide curve in the same manner. Notice now that the loft fits the guide curves well.
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15 Evaluate the loft preview. Before clicking OK to create the loft, take a look at the mesh lines. The
16 Create the top loop. On the Front reference plane,
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create the sketch as shown. The bottom of the 0.750” diameter circle should just touch the circle from the layout sketch.
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mesh lines are the thin black lines on the loft preview. In this case, the mesh looks clean, and the lines don’t bunch together, twist or kink. In some lofts, the mesh will preview areas which appear rippled, kinked, or twisted. This is usually an indication that there are problems with the loft or that there will be problems later with features such as shell, offset or fillet.
Revolve the sketch about the centerline.
Do not merge the revolved body with the lofted body.
17 Trim the loft feature.
Before adding the top loop, it was difficult to tell where the top of the lofted feature should be. This is the reason why we overbuilt the loft. Now that we can see the relationship between the shapes, we can trim back the loft to the appropriate length.
Also, because the loft has to transition to a round shape, it makes sense to have the loft end at a curved edge rather than a flat one.
No
On the Right reference plane, draw a circle concentric with the top loop with a diameter of 3.7”.
Do
Extrude a Through All cut in both directions. Use the Feature Scope so that it only cuts the lofted body.
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Lofts
18 Trim the top loop.
To transition from the hook loft to the loop, we need a place on the loop to transition to. Again on the Right reference plane, draw a circle dimensioned as shown.
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Be sure to use Flip side to cut.
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Extrude a Through All cut in both directions. Use the Feature Scope so that it only cuts the revolved body.
19 Make the transition loft.
Now that we have a cut surface on the loft and one on the loop, we can join the two shapes together.
Do
No
Create a loft feature by selecting the two faces created by the cuts made in previous steps. Select the faces at approximately corresponding locations. It will also work if you select the edge around the cut face instead of the cut face itself, but in general, it is better practice to loft between faces than edges when creating solid lofts. This is because SolidWorks will use the edge to create a new face which could introduce small errors. Use Tangency to Face end condition for both profiles. Use a value of 0.5 for the Start Tangent Length and End Tangent Length.
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If the loft bulges out, it may be because the tangency is going to the wrong face. If this is the case, you will have to use the Next Face button to get it to select the correct face to be tangent to.
20 Sketch a point.
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Also notice the connectors. Depending on your selection, you may have to move them. The best place for them is as shown, along the plane of symmetry of the part Create a plane with an Offset Distance of 0.5” from the small end of the hook loft.
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Create a sketch on the new plane and sketch a point as shown. The point should be constrained Vertical from the Origin or Coincident to the Right reference plane. Exit the sketch.
21 Loft the tip.
Create a loft from the flat face of the end of the hook loft to the sketch point. Lofting to a point is a useful technique for capping the ends of parts.
Do
No
Start/End Constraints should be set Tangency To Face for the face profile.
Use Normal to Profile for the point profile, with the End Tangent Length set to 2.2 to give the tip of the hook some breadth. Click OK.
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22 Results.
Boundary Feature
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23 Save and close the part.
The Boundary feature (boss, cut, surface) is much like Loft with some exceptions. The best way to understand the Boundary feature is to compare it with Loft and illustrate the differences. This will help you decide which tool to use in different modeling situations.
Do
No
When a feature is made up of only profiles, such as the Defroster Vent, there is very little difference between the results you get with Loft and those you get with Boundary. The most noticeable difference is the start and end tangent conditions seem to have more influence in the Loft feature. However, you can adjust this in the Boundary feature by lengthening the tangent vectors.
260
Loft
Boundary
Which result is correct? They both are. When you are modeling features that are not analytic, such as extrudes and revolves are, but rather are created by interpolating between cross sections, there is virtually an unlimited number of correct answers.
SolidWorks 2012
Lesson 7 Lofts
When a feature is made up of two sets of curves, profiles and guides in the case of Loft, the difference between Loft and Boundary is more pronounced. An example of this type of part would be the Hook.
Do
No
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In the Loft feature, the profiles have more influence over the resulting shape than do the guides. In the Boundary feature, both sets of curves (called Direction 1 and Direction 2) have the same weight or influence over the shape of the result.
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Lofts
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This difference between Boundary and Loft really becomes apparent in surface modeling. Because both sets of Boundary curves have equal weight, C2 matching can be applied to all four sides of the surface patch. With a lofted surface, C2 matching can only be applied to the profiles, not the guides.
For a more complete treatment of the Boundary feature, please refer to the Surface Modeling course.
Optional
Explore the Boundary feature by redoing any of these case studies using Boundary instead of Loft: Defroster Vent
No
Lofted Merge
Do
Hook
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SolidWorks 2012
Exercise 24 Funnel
Exercise 24: Funnel
Create this part using the information and dimensions provided.
Loft on page 229.
I
Sweeping Along Model Edges on page 213.
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Procedure
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This lab reinforces the following skills:
Open a new part using the Part_MM template and name it Funnel.
1
Sketch the first profile.
Open a new sketch on the Top reference plane.
Use ellipses, lines and arcs to create this profile.
2
Second profile.
No
Create a new plane that is parallel to the Top reference plane 82.5mm below it.
Do
Sketch a circle lined up with the Origin. This circle will be used as the second profile in a loft, after it is divided up into sections that match the first profiles endpoints. If the circle is not broken up, the loft will decide what the breakup of the circle should be.
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SolidWorks 2012
Funnel
3
Breakup.
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Add centerlines radially from the circle’s center to the endpoints of the first profile. This geometry will cross the circle’s circumference at several places.
4
Divide the circle.
Using the Split Entities command, add six split points, breaking the arc into pieces. Make each split point coincident with a centerline. You can add Coincident relations or you can drag and drop them onto the centerlines.
First loft.
Exit the sketch and loft between the two profiles. Select two endpoints that will match position, one from each sketch. This will ensure that the “start point” of the loft will be positioned correctly.
Do
No
5
Important!
The option Merge Tangent Faces should be used.
Note
An extra callout was added to the illustration for clarity.
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Exercise 24 Funnel
6
Resulting loft.
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The loft solid should look like this when completed.
7
Initial neck sketch.
The funnel neck is formed by another loft, this time using two sketched circles. Flip the model over and sketch a circle on the end face, making it Coradial with the circular, outer edge.
Circular Edge
Add a point on the circle. Relate the point to the Origin with a Vertical relation. Neck end sketch.
Create a new reference plane offset from the circular face by 50mm. Sketch a circle that is lined up with the Origin. Add a point on the circumference of the circle that is related to the Origin with a Vertical relation. The points are used to “line up” the profiles just as the centerlines were used in the first loft.
Do
No
8
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Exercise 24
SolidWorks 2012
Funnel
9
Neck loft.
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Select the sketches in the FeatureManager design tree and loft between the profiles.
10 Shell the funnel.
The dimensions are given for the inside of the funnel.
Do
No
Create a thin walled part by shelling to the outside, a thickness of 1.50mm.
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Exercise 24 Funnel
11 Build the rim.
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Sketch the outline of the rim using the dimensions given. Use Convert Entities to create the inner outline. Extrude the rim to a depth of 1.50mm. Make the two thickness values equal using a global variable.
12 Sweep a lip on the underside of the rim.
The cross-section of the lip is a semi-circle, 1.50mm in diameter. Use the model edge of the rim as the sweep path. To review selecting model edges as a sweep path, see Propagate Along Tangent Edges on page 214.
Do
No
Tip
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Exercise 24
SolidWorks 2012
Funnel
13 Make a rib on the neck of the funnel.
Profile
Sweep Path
Sweep the section along a curve that lies on the inner face of the funnel neck.
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An easy way to construct this curve is to sketch a line and constrain it with Pierce relations to model edges at the opening and where the inside of the neck meets the main body. 14 Pattern the rib.
Make a total of three ribs, equally spaced, using a circular pattern.
15 Problem.
Do
No
Because of the shape of the sides of the funnel, the two copies of the rib do not merge completely with the body.
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Exercise 24 Funnel
16 One solution.
Edit the sketch for the path of the rib and make the path longer by a adding a short, colinear line. Make the line about 1mm long. If you make the path too long, the rib will protrude into the inside of the funnel.
Note
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17 A hole in the rim.
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Using the dimensions provided, sketch a profile to cut through the rim so the funnel can be hung on a hook. Notice the use of an angular dimension on an arc. This can be created by picking the arc’s centerpoint and its two ends.
Do
No
Detail of the hole.
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Exercise 24
SolidWorks 2012
Funnel
Do
No
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18 Save and close the part.
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SolidWorks 2012
Exercise 25 Rocker Arm
Exercise 25: Rocker Arm
This lab reinforces the following skills: Layout Sketches on page 253.
I
Sketching Splines on page 8.
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Derived Sketches on page 237.
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Loft on page 229.
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Create this part using the dimensions provided. Use sketch relations and dimensions to maintain the design intent.
Design Intent
The design intent for this part is as follows:
1. The part is symmetrical. 2. The main body of the arm must smoothly connect the three pivot points. Units: millimeters
Procedure
Open a new part using the Part_MM template and name it Rocker Arm.
1
Draw the layout sketch.
No
Use the dimensions shown to draw the layout sketch on the Front reference plane. This will place all of the functional features on this part. Note the symmetry. Exit the sketch.
Do
Name the sketch Layout Sketch.
2
New sketch.
Open a new sketch on the Front reference plane. Name the sketch Guides.
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Rocker Arm
Draw guide curves.
Draw both guide curves in the same sketch. The lower guide curve is two lines and an arc, and the upper one is a single three-point spline. The spline is perpendicular to the two short centerlines that pass through the centers of the small circles. Create three new planes.
Plane2
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4
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3
Create two new planes perpendicular to the centerlines at the centers of the small circles.
Create a third plane at 90 degrees from the Front reference plane through the short centerline.
5
Draw profile sketch.
On Plane1, sketch an ellipse.
No
Constrain it to the guide curves and dimension it as shown.
6
Derived sketch.
Do
Using the sketch from step 5, create a derived sketch on Plane2.
272
Constrain it to the layout sketch and guide curves to fully define it.
Plane3
Plane1
SolidWorks 2012
Exercise 25 Rocker Arm
7
Draw third profile sketch. On Plane3, draw an ellipse
dimensioned as shown.
Begin loft.
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8
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Use Pierce relations to constrain the ends of the major axis to the two guide curves.
Click Loft, and select the three ellipses.
9
Select guide curves.
Select the spline as the first curve.
Select the two lines and the tangent arc as the second guide curve.
Since both of the guide curves are in the same sketch, you will have to use the SelectionManager.
Do
No
Click OK.
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Exercise 25
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Rocker Arm
10 Extrude the pivot bosses. On the Front reference plane
Set the three offset values equal to each other using a global variable.
Optional
Extrude the sketch: I I
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I
End Condition: Mid Plane Distance: 65mm Draft: 5°
11 Cut holes.
Open another new sketch on the Front reference plane.
Convert the circles from the layout sketch and create a cut that goes Through All in both directions.
12 Add fillets. Add 10mm fillets around the
bosses.
Select the lofted body rather than the edges.
Do
No
Tip
274
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open a new sketch and offset each of the three circles from the layout sketch by 10mm.
13 Save and close the part.
SolidWorks 2012
Exercise 26 Boat Hull
Exercise 26: Boat Hull
Create this part using the dimensions provided. Use relations and equations where applicable to maintain the design intent.
Layout Sketches on page 253.
I
Fit Spline on page 147.
I
Projected Curve on page 143.
I
Loft on page 229.
I
Loft connectors. on page 230.
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I
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This lab reinforces the following skills:
Units: MKS (meter, kilogram, second)
Design Intent
The design intent for this part is as follows: 1. 2. 3. 4.
Procedure
1
Bow (front of hull) comes to a point Transom (rear of hull) is a single smooth spline Intermediate sections consist of four symmetrical lines Hull transitions from sharp corners to a continuous smooth surface
New part.
Open a new part using the Part_MM template.
Change the units to MKS (meter, kilogram, second) with 3 decimal places. Save the part naming it Boat Hull.
2
Draw a scale reference layout sketch.
Sometimes it is helpful to have a reference sketch just to indicate the overall size of the part.
No
On the Right reference plane, sketch a rectangle 9m long by 2.2m high.
Do
Change the rectangle to construction lines.
3
Insert sketch picture.
A sketch picture has been provided in the Exercises folder of this lesson. It is named Boat Hull Side Elevation. Insert the sketch picture and scale and position it using the sketched rectangle as a guide. 4
Exit the sketch.
Rename it to Scale_Reference.
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Exercise 26
SolidWorks 2012
Boat Hull
5
Draw a layout sketch. On the Right reference plane, sketch two splines – one for the keel and
one for the sheer. Use the sketch picture as a guide. Definition
Sheer is a boat building term meaning the fore-and-aft curvature from bow to stern of a boat’s deck as shown in side elevation.
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One end of each spline is Coincident with the Origin.
The other end of each spline is Coincident with the rightmost vertical construction line in the Scale_Reference sketch.
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Sheer
Keel
Keel
On this part, especially on the keel, you want to create a spline that does not change convexity. The best way to find a convexity change is to right-click the spline and click Show Inflection Points.
Inflection Point
Do
No
Tip
Remember the relationship between splines and lofts: loft sections are analogous to spline points. When using a spline to lay out the keel, it is a good idea to make the spline points and the loft sections coincide. Later we will create the profile planes at the spline points of the keel.
The curvature comb and the control polygon can also show an inflection point where they cross the spline. 6
Exit the sketch.
Rename it Layout_Sketch.
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SolidWorks 2012
Exercise 26 Boat Hull
7
Second reference sketch.
Open a new sketch on the Top reference plane.
The width is 4.5 m. Note particularly the Midpoint and Coincident relations.
8
Sketch picture.
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Sketch a rectangle of construction lines as shown.
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Switch to a Top view and insert the sketch picture named Boat Hull Plan View.
Scale and position the picture so it lines up with the sketched rectangle.
9
Sketch a spline.
Use a spline to sketch half of the top outline of the boat, tracing the sketch picture.
No
Make sure the spline is as long or longer than the rest of the sketches. If it is too short, it will not work as a guide curve.
Do
Use Coincident relations to connect the ends to the sketched rectangle.
10 Exit the sketch. Rename it Top_Outline. 11 Copy the sheer. On the Right reference plane, open a new sketch and use Convert Entities to copy the sheer from the Layout_Sketch. 12 Exit the sketch.
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Exercise 26
SolidWorks 2012
Boat Hull
13 Hide the Layout_Sketch. 14 Create a projected curve. Use Project Curve to create the 3D curve
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from two 2D sketches.
15 Create mirrored curve.
You cannot mirror a curve directly. To create a mirrored curve, use a Derived Sketch and a shared sketch to create another projected curve.
Insert a derived sketch of Top_Outline on the Top plane, and use Modify Sketch to mirror it about the Origin.
Use Project Curve
to create the 3D curve from two 2D sketches.
16 Autosize the standard planes.
Do
No
When making a part much larger than most of the other parts you have worked on, the default display size of the reference planes may be too small.
278
Right-click the Front reference plane in the FeatureManager and click Autosize. You can do this for the rest of the standard planes as well as any newly created plane features.
SolidWorks 2012
Exercise 26 Boat Hull
17 Create profile planes. Show the Layout_Sketch.
Create new planes in the order shown parallel to the Front reference plane and at each of the keel spline points and at the end of the keel using the Parallel to Plane at Point plane type. Plane3
Plane4
Plane5
After you create the first plane, select the Front reference plane and the next spline point. Then press Enter. This repeats the previous command. Now press Enter again to create the next plane.
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Tip
Plane2
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Plane1
18 Create first profile.
The first profile will be the point at the bow of the boat. On the Front reference plane, place a sketch point
at the Origin.
Exit the sketch and rename it Bow_Point.
19 Create the second profile. On Plane1, create a sketch of five
lines as shown, with symmetry. Add a Pierce relation between the sketch and the keel spline and one of the projected curves. Because of the symmetry, if you pierce both projected curves, the sketch will become over defined. Exit the sketch and rename it Second_Profile.
No
20 Copy the profile. Select the Second_Profile sketch in the FeatureManager and press Ctrl+C.
Do
Select Plane2 and press Ctrl+V. Do the same for Plane3 and Plane4, but not Plane5. Plane5 will get its own sketch.
279
Exercise 26
SolidWorks 2012
Boat Hull
21 Constrain the copied profiles. Add the Pierce relations to the copied sketches and change the
dimensions as shown.
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Name the sketches Third_Profile, Fourth_Profile, and Fifth_Profile respectively.
Third_Profile
Fourth_Profile
Fifth_Profile
No
The Fifth_Profile will get some additional attention in the next step.
22 Fit spline. Edit Fifth_Profile.
Do
Select the lower four sketch lines and fit a spline to them as follows:
280
I
Clear the Closed spline check box
I
Constrained Tolerance = 0.05 m
I
Transitioning from a profile with sharp corners to a profile rounded by a spline will enable you to create a transition which gradually blends into a smooth surface.
SolidWorks 2012
Exercise 26 Boat Hull
23 Adjust the sketch.
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In the previous step, the Tolerance was set to 0.05 m. This means the spline can be as far as that distance away from the original lines. Because loft guide curves have to contact the profiles, we need to adjust the sketch to compensate for this.
Fit Spline Considerations
You cannot add relations to a fit spline. This poses a challenge when trying to “attach” the fit spline to the guide curve. Normally we would insert a sketch point and constrain it to the intersection of the construction line and the fit spline. We then could add a Pierce relation between the point and the guide curve. However, since we cannot add relations to a fit spline, that technique won’t work.
24 Trim the construction line.
Under defined
The system trims the construction line to its intersection with the fit spline.
Notice the end is blue indicating it is under defined. That is because there is no Coincident relation between it and the fit spline.
25 Dimension the construction line.
Do not change the length. Accept the value as it is. This will fully define the construction line.
Do
No
Notice the length is slightly less then the Tolerance of 0.05m used in the Fit Spline command. This is because the Tolerance is the maximum distance the spline can deviate from the source geometry.
26 Remove relation. Delete the Pierce relation between the
original lines and the keel.
Delete
281
Exercise 26
SolidWorks 2012
Boat Hull
27 Add relation. Add a Pierce relation between the end of
the construction line and the keel. This pulls the profile down so it intersects the keel.
29 Transom sketch. On Plane5, draw several
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construction lines using symmetry and then sketch a single spline as shown to create a symmetrical spline.
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28 Exit the sketch.
Exit the sketch and rename it Transom.
30 Hide the Layout_Sketch.
31 Keel guide curve. On the Right reference plane, open a new sketch and draw a spline whose spline points are Coincident with each profile except for the Fifth_Profile.
The Fifth_Profile, the fit spline, has no point on the Right reference plane and the guide curve has to be related to the profile geometry.
No
Add a Pierce relation between the spline point and the fit spline in the Fifth_Profile.
Do
32 Exit the sketch. Rename it Keel_Guide.
282
SolidWorks 2012
Exercise 26 Boat Hull
33 Start the loft. The Bow_Point sketch is the first
profile. Select the profiles in order and in approximately the same location. At first the loft may appear misshapen.
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34 Select the guide curves. Click in the Guide Curves selection
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It is easy to see the effect of having a different number of sketch segments in the profiles. Some faces may appear twisted or like they are joining the wrong corresponding faces. This will be fixed by using the loft connectors.
list and select both projected curves and the Keel_Guide sketch.
The loft should straighten out at this point.
35 Show connectors.
Right-click in the graphics window and click Show All Connectors.
36 Adjust connectors.
No
We want the sharp corner to transition at the middle of the bend in the spline.
Do
Adjust the connectors for the corner transition.
Adjust
283
Exercise 26
SolidWorks 2012
Boat Hull
Before Adjustment
38 Finish the loft. Click OK to create the loft.
After Adjustment
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39 Shell.
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37 Adjustment.
Optionally you can shell the boat, removing the top face. Shell with a Thickness of 0.006 m (6.0mm).
Do
No
40 Results.
284
SolidWorks 2012
Exercise 27 Light Cover
Exercise 27: Light Cover
Create this part using the dimensions provided. Use relations and equations where applicable to maintain the design intent. Closed loop loft
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I
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This lab reinforces the following skills:
Design Intent
The design intent for this part is as follows: 1. Part is symmetrical. 2. The surface is smooth. 3. The shell is 1.25mm thick. Units: millimeters
Procedure
Open a new part using the Part_MM template and name it Light Cover.
1
Create the setup curve.
This part uses a projected curve to set up the loft, but does not use the curve as a guide curve or a centerline. I I
Do
No
I
On the Front reference plane, draw an ellipse. On the Right reference plane, draw an arc. Create a projected curve.
285
Exercise 27
SolidWorks 2012
Light Cover
2
Create multiple profile sketches. On the Top reference plane, create
Second sketch.
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3
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two semi-circles centered on the projected curve with dimensions as shown.
On the Right reference plane, create two half ellipses centered on the projected curve with dimensions as shown.
4
Start the loft.
When you select one of the profiles, the SelectionManager will appear. Use the Closed Loop option and click OK.
No
Do this for all four profiles.
5
Adjust the connectors.
Do
You may need to adjust the connectors to get the loft to work properly.
286
If the connectors will not move, right-click and click Reset Connectors.
SolidWorks 2012
Exercise 27 Light Cover
6
Close the loft.
7
Shell the part.
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To make the loft create a closed loop, click the Close loft option in the Options area.
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Use a Thickness of 1.25mm and remove the back face created by the straight lines.
Save and close the part.
Do
No
8
287
Exercise 27
SolidWorks 2012
Do
No
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Light Cover
288
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Lesson 8 Other Advanced Tools
Upon successful completion of this lesson, you will be able to: Understand the options available with default, constant radius fillets.
I
Apply advanced fillet types.
I
Analyze geometry for curvature, minimum radius and inflection points.
I
Analyze surfaces with zebra stripes.
I
Use the Wrap feature.
I
Use the Deform feature.
No
I
Use the Move Face command.
I
Use the Delete Face command.
Do
I
289
Lesson 8
SolidWorks 2012
Other Advanced Tools
Advanced Fillets
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Fillets do not take the place of advanced modeling techniques such as loft and sweep. In general they are used to break sharp edges. This is mostly a best practice suggestion which will depend on the type or level of work you are doing. Highly stylized consumer products will use fillets mainly in the final stages to break hard edges. On the other hand, when working with rough conceptual models, it may be acceptable to use fillets to round out a part or create an overall shape.
There are many filleting functions beyond the most commonly used default constant radius fillet. Advanced fillets can be powerful tools to help you achieve your design goals. This lesson will help you explore these. Advanced fillet types include: I
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I
Variable radius Setback fillet Face fillet
I
There are also various options which affect the finished fillet: I I I I I I I
Keep Features
Multiple radius Overflow type (Keep edge, Keep surface) Round corners Curvature continuous Constant width Smooth or straight transition for variable radius fillet Using hold lines
The Keep features option controls the behavior of fillets when they fully surround an existing feature.
1
2
Open the part Keep_Features.
Click Fillet
.
Apply a constant radius fillet to the edges shown using a Radius of 5mm.
Do
No
Expand the Fillet Options group box and look at the Keep features option. By default it is selected.
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SolidWorks 2012
Lesson 8 Other Advanced Tools
3
Click OK.
Change the fillet radius value. Change the radius value to 9mm.
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4
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Notice that both the hole and the boss are affected by the fillet and are either trimmed or extended to adjust for it.
Rebuild the model to reflect the new value.
Notice that the fillet completely surrounds the boss but not the hole. Both features are still extended or trimmed back to compensate.
5
Change the Keep Features setting. Edit the fillet feature and clear the Keep features check box.
Click OK.
Do
No
Notice that the boss disappears but the hole remains.
291
Lesson 8
SolidWorks 2012
Other Advanced Tools
6
Change the fillet radius value. Change the radius value to 12mm.
Rebuild the model to reflect the new value. 7
Keep Edge and Keep Surface
Save and close the part.
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The hole disappears.
Under Fillet Options for constant as well as variable radius fillets, there are two Overflow type options: Keep edge Keep surface
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I I
These options enable you to specify how fillets will act when they are larger than the space available for them.
1
Open the part Keep_Edge.
Notice that the edges of the middle layer are not parallel to the sides of the bottom layer. This will help illustrate the differences between the Keep edge and Keep surface Options.
2
Click Fillet
.
Select the edge as shown. Set the Radius to 5mm.
Do
No
Make sure Tangent propagation is selected.
292
SolidWorks 2012
Lesson 8 Other Advanced Tools
3
Keep Surface setting. Expand the Fillet Options group box and click Keep surface.
The surface that is being “kept” is the surface of the fillet itself. Notice that the edges of the outer faces have changed – they are no longer straight. However, the faces of the fillet are unbroken. 4
Keep Edge setting.
Face is unbroken Edges have changed
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Edit the fillet and change the option to Keep edge.
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Click OK.
Now notice that the boundary of the outer face is now straight – as it was before the fillet. However, the face of the fillet has been broken up.
The Default setting in this case Face is broken would be the same as Keep edge, Edges are straight but in general, this is an automatic setting which allows SolidWorks to choose the overflow type for you based on geometry conditions.
5
The Round corners setting determines the behavior of fillets at non-tangent corners. With Round corners selected, the fillet will roll around the sharp corner like a marble. With the option cleared, the fillet will miter like a picture frame.
Do
No
Round Corners
Save and exit the part.
Round corners selected
Round corners cleared
293
Lesson 8
SolidWorks 2012
Other Advanced Tools
When filleting you often have to select edges that are hidden behind faces of the model. Under Fillet Options there is an option Select through faces which allows you to select hidden edges. This option is enabled by default and works independently of the similar option in Tools, Options, System Options, Display/Selection.
Variable Radius Fillets
As the name suggests, the Variable Radius fillet feature creates a fillet or round which can change radius along an edge.
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Select Through Faces
1
Open the part Variable_Radius.
2
Click Fillet
.
Select the curved edge of the part.
Click Variable radius as the Fillet Type.
Note
The fillet type cannot be edited after the feature is initially created. You cannot change a constant radius into a variable radius fillet or vice versa.
3
Enter radius values.
Do
No
The radius values can be added either using the on-screen callouts or in the PropertyManager. The callouts are generally easier to use because they graphically show where the radius value will be applied.
294
Assign a value of 30mm to the inner callout and 10mm to the outer callout as shown.
SolidWorks 2012
Lesson 8 Other Advanced Tools
Variable radius control points operate as follows: I
I
I
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I
The system defaults to three control points, located at equidistant increments of 25%, 50%, and 75% along the edge between the vertices. You can increase or decrease the number of control points. You can change the position of any control point by changing the percentage assigned to that control point. You can also drag any control point, and its assigned percentage will update accordingly. If all the default control points have been assigned and you still need to assign more, select a control point, press Ctrl, and drag the control point to create another. Although there is a visual display of the control points, they are only active if you select them and assign a radius value. Inactive control points are orange. Active control points are gray, and have a callout attached to them indicating the assigned radius and percentage values.
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Control Points
I
4
Add a control point.
By default, callouts only appear at the endpoints of selected edges. To assign another radius value at an intermediate point, select one of the orange control points and add a value to the callout.
Select the orange control point nearest to the 30mm value and assign 30mm.
5
Click OK.
The finished variable radius fillet is smooth. Save and exit the part.
Do
No
6
295
Lesson 8
SolidWorks 2012
Other Advanced Tools
Straight and Smooth Transitions
Variable radius fillets can transition between values at control points in two ways, straight or smooth. To access the setting, use the Variable Radius Parameters area in the PropertyManager.
Smooth Transition
Zero Radius Values
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Straight Transition
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The variable radius fillet is one of the few features in SolidWorks which can accept a value of zero. 1
Open the part Zero_Radius.
Notice that the edges on either side of the ridge are parallel on the near end of the part. This situation often causes trouble for fillet features, especially if the center ridge changes convexity, from convex to concave.
2
Apply a variable radius fillet.
Do
Note
No
Use a Radius of 0.0mm at the end of the ridge where the edges are parallel and a Radius of 10mm where the edges meet at an angle.
296
Zero radius fillets may cause problems in manufacturing, so they should be used with discretion.
SolidWorks 2012
Lesson 8 Other Advanced Tools
3
Zero length fillet.
Suppress the variable radius fillet.
4
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Create a constant radius fillet with a Radius of 10.0mm.
Compare this fillet with the one created in step 2.
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Although both fillets transition from a 10mm radius to a point, the shape of that transition is different between the two examples.
5
Setback Fillets
Save and exit the part.
The Setback Fillet is the most complex fillet type to set up. The effect can be subtle or outlandish.
Do
No
Setback fillets are applied where three or more filleted edges meet at a single vertex. The setback is the distance from the common vertex to where each fillet begins to blend. Each edge can have a different setback distance.
The Setback Parameters can be used with Constant radius, Multiple radius or Variable radius fillets. In this example we will use a Multiple radius fillet.
Setback Fillet
Default Fillet
297
Lesson 8
SolidWorks 2012
Other Advanced Tools
1
Click Fillet
.
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2
Open the part Setback_Fillet. On this part we will work on only two, three-edge vertices, although it is possible to do more.
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Setback fillets are used in several applications, particularly cosmetic plastic parts and deep drawn sheet metal. They give the corner a blended look, and for drawn metal, they more accurately reflect the stretching of the metal than do default fillets.
Enter a Radius of 12.5mm and click the Multiple radius fillet option.
Select the five edges as shown.
The callouts can get very busy on the screen and are sometimes difficult to manage. Move them around to separate them and improve visibility.
3
Assign radius values.
It is easier to assign radius values before assigning the setback values.
No
The callouts make it easier to identify which value is assigned to which edge.
Do
4
298
Select the setback vertices.
Expand the Setback Parameters group box and click in the Setback Vertices selection list. Select the two vertices where the filleted edges meet.
SolidWorks 2012
Lesson 8 Other Advanced Tools
5
Assign setback values.
The callout for the setback distances can be a little daunting at first. As you start entering values, arrows will display indicating which edge the distance applies to and individual leaders will attach to each edge. Use the Tab key to cycle from one callout cell to the next.
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Tip
The fillet preview will disappear until you have entered all the values for a given vertex.
Using the Set Unassigned and Set All buttons can save a lot of set up time if there are many common values.
Do
No
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The final set up should look as shown below.
299
Lesson 8
SolidWorks 2012
Other Advanced Tools
6
Click OK.
The final result with edges displayed shows how SolidWorks patches together this complex fillet.
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This example uses only constant radius fillets. If you think about the added work to do this with variable radius fillets on each edge, you begin to see how complex the set up for this fillet type can be.
7
A Face Fillet is created between selected faces, instead of on selected edges as with the default fillet type. Face fillets are generally used when the edge between two faces is not as perfect as you would like it to be. For example, if you have an imported model with a chamfer on an edge, and you want to put a fillet over the chamfer, or if you have a model with extraneous breaks in the edges, face fillets are often a good approach.
Do
No
Face Fillets
Save and exit the part.
300
SolidWorks 2012
Lesson 8 Other Advanced Tools
1
Import a Parasolid file.
Import the Parasolid file Face_Fillet.x_t using the Part_MM template.
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Chamfer
Imperfections
Importing a Parasolid file creates a new SolidWorks document. You have the option of specifying a document template or allowing the system to use the default template. This choice is determined by the settings in Tools, Options, System Options, Default Templates.
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Note
Notice the chamfer on one side and the imperfections along the edge on the other side. Both of these will prevent edge fillets from being applied to this part.
2
Click Fillet
.
Click the Face fillet option.
Click in the Face Set 1 selection list to activate it. Select the flat face on the side with the chamfer.
Click in the Face Set 2 selection list to activate it. Select the outside face of the part.
In a situation like this one, where the face fillet is removing an existing face, the chamfer, the radius must be larger than the geometry it is meant to cover. Edge fillets often fail because the fillet is too large. Face fillets sometimes fail because the fillet is too small.
Do
Tip
No
Set the Radius to 4mm and click OK.
301
Lesson 8
SolidWorks 2012
Other Advanced Tools
3
Create fillet on the other side.
Flip the part over so you can now see the face that has two small cuts. Create a face fillet similar to the one just created on the other side. Save and close the part.
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4
Curvature Continuous Fillets
Face fillets enable you to create a fillet which is curvature continuous. This results in a fillet whose cross section is not circular, or arc-based, but is instead based on a spline. The default fillet type has a constant curvature and is tangent to the adjacent faces. The curvature continuous fillet matches the curvature of the surrounding faces, and then, like a loft, the curvature of the fillet is continuously variable.
Important!
This option is available only when creating a face fillet.
Abrupt transition between fillet and adjacent faces
Smooth transition between fillet and adjacent faces
Constant curvature fillet
Curvature continuous fillet
Do
No
Curvature continuous fillets are often used in consumer product design. This is because the tangent continuity between the default fillet and the adjacent faces creates a noticeable “break” or even the illusion of concavity. The curvature continuous fillet creates a smoother transition between the fillet and the adjacent faces.
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Lesson 8 Other Advanced Tools
Constant Width Fillets
The Constant width option is also only available when creating face fillets. When using the Constant width option, the Radius value actually specifies the chord length of the fillet. This option is typically used when filleting between two faces which are either at a very sharp angle or on a changing angle.
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Curvature continuous and Constant width can be used together.
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The Constant width fillet works like an automatic variable radius fillet where the radius is determined automatically by keeping the chord length of the fillet constant.
Constant radius
Hold Lines
Constant width
Another option with face fillets is the use of Hold lines. A hold line is used to define the fillet’s tangent edge or rail. Defining the rail of the fillet defines the fillet’s radius. In this case the bottom edge of the part will be used.
No
Since the hold line will define the radius, you do not need to enter a radius value. Also, when you select a hold line, the Radius field disappears.
1
Open part.
Do
Open the part Cover_Sketches.
2
Click Fillet.
In the Fillet Type group box, select the Face fillet type.
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Lesson 8
SolidWorks 2012
Other Advanced Tools
Since the Hold line will define the radius, you do not need to enter a radius value. Also, when you expand the Fillet Options group box and select a hold line, the Radius field disappears. 3
Select faces.
Verify that the Face Set 1 selection list is active and select the top face of the part. Activate the selection list for Face Set 2 and select one of the three side faces.
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Note
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With the default condition Tangent propagation enabled, picking one face will select all three. 4
Add fillet options.
Expand the Fillet Options group box.
Click in Hold line selection list, and select the three edges as shown in the illustration. Click OK to create the fillet.
5
Results.
Do
No
The three vertical faces (Face Set 2) are completely removed. The fillet is created with a variable radius defined such that the fillet ends exactly on the hold lines.
304
Hold Lines
SolidWorks 2012
Lesson 8 Other Advanced Tools
6
Mirror and shell.
Mirror the body. Then remove the two flat faces by shelling the part with a wall thickness of 2.5mm.
Analyzing Geometry
Save and close the part.
SolidWorks has several tools that are used to obtain information and to assess the quality of curves and surfaces. They include: Display Curvature Show Curvature Combs Show Minimum Radius Show Inflection Points Zebra Stripes
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I I I I I
What is Curvature?
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7
To avoid getting too deep into mathematics, we will use this working definition: Curvature is the reciprocal of the radius. If a surface has a local radius of 0.25, it has a curvature of 4. The smaller the curvature value, the flatter the surface.
Introducing: Display Curvature
Displays the faces of the model rendered in different colors according to their local curvature values. You can assign different curvature values to the scale of colors. Red represents the largest curvature (smallest radius) and black represents the smallest curvature (largest radius).
Where to Find It
I I I
Displaying the curvature can be system resource intensive. In many cases you can improve performance by displaying the curvature only on the face or faces that you want to evaluate.
No
Tip
CommandManager: Evaluate > Curvature Menu: View, Display, Curvature Shortcut Menu: Right-click a face and click Curvature
1
Open part.
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Open the part Analyze_Geometry.
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Display Curvature. Click Curvature .
The part is rendered in colors according to the curvature of the faces. As you move the cursor over a face, a print out appears giving both the curvature and radius of curvature values. 3
Look at the fillet.
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2
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Notice the dramatic change in color from the body of the bottle to the fillet around the bottom. This indicates that although the fillet is tangent to the body, it is not curvature continiuous.This means the faces do not have the same curvature at the edge where they meet.
4
Show Curvature Combs
Turn off curvature display. Click Curvature again to turn off the curvature display. Show Curvature Combs provides visual representation of the slope and curvature of most sketch entities. You can use Show Curvature Combs to evaluate splines before they are used to sweep or loft solid
features. You can also indirectly evaluate curved faces by generating intersection curves and then evaluating the curves.
Show Curvature Combs gives
a graphic representation of the curvature in the form of a series of lines called a comb. The length of the lines represents the curvature. The longer the line, the greater the curvature (and smaller the radius).
No
Introducing: Show Curvature Combs
Do
When the comb crosses the curve, it indicates an inflection point. An inflection point is where the curve changes convexity.
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In the illustration below there are two very similar looking curves, both of which appear to have two inflection points.
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When you use Show Curvature Combs, it becomes obvious that the bottom most curve is not smooth and has many inflection points.
Do
No
You can use Show Curvature Combs to learn about how curves are connected. Look at the illustration below.
The two sketch entities are a circular arc and a quarter of an ellipse. The two curves are tangent but not matched in curvature. This is indicated by the fact that the curvature lines at the common endpoint are: I I
Collinear (indicates tangency). Not the same length (different curvature values).
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In the illustration at the right, the two entities are not tangent as indicated by the fact that the curvature lines at the common endpoint are not collinear.
Where to Find It
I
Shortcut Menu: Right-click the spline and click Show Curvature Combs
I
Menu: Select the spline and click Tools, Spline Tools, Show
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Curvature
Intersection Curves
Introducing: Intersection Curve
Show Curvature Combs only works on sketch entities. In situations
where you do not have a sketch entity, you will have to apply other techniques. For example, to evaluate a face or surface, one technique is to generate an intersection curve.
Intersection Curve opens a 3D sketch and creates a sketched curve at
the following kinds of intersections: I I I I I
Where to Find It
I
A plane and a surface or a model face. Two surfaces. A surface and a model face. A plane and the entire part. A surface and the entire part.
The curvature comb remains visible when you close the sketch (unless the sketch has been made into a feature). To remove the display, right-click the sketch entity, and click Show Curvature Combs again from the shortcut menu to remove the check mark.
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5
Intersection curves. Select the Front reference plane and open a
sketch. Click Intersection Curve
.
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Select the face of the fillet and the main body of the bottle.
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Click OK and then Cancel to close the Intersection Curves PropertyManager.
6
Results.
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No
The system generates intersection curves between the sketch pane and the selected faces. Two sets of intersection curves are created because the reference plane intersects the faces in two locations. Only one set is needed for this example.
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7
Show Curvature Combs.
Right-click one set of the intersection curves and click Show Curvature Combs. Note the following:
I
Color
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I
The fillet has a circular cross section as indicated by the curvature comb. The fillet and the side of the bottle are matched in tangency. The fillet and the side of the bottle are not matched in curvature as indicated by the different lengths of the curvature combs.
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I
The color of the curvature comb is controlled by Temporary Graphics, Shaded which is listed under Tools, Options, System Options, Color.
Depending on the color of the viewport background, you may want to change the temporary graphics color for maximum visibility.
8
Modify Curvature Scale.
Right-click the intersection curve and choose Modify Curvature Scale. Slide the bar right (decrease) or left (increase) to change the scale of the curvature combs.
There is also a slider to control Density, which is the number of curvature combs per curve segment.
Show Minimum Radius
Show Minimum Radius (of curvature) can be used to graphically
Where to Find It
I
Do
No
display the position and value of the minimum radius of curvature on the curve. This is important information for shelling and offset geometry.
310
Shortcut Menu: Right-click the spline and click Show Minimum Radius
I
Menu: Select the spline and click Show Minimum Radius
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Show Inflection Points
Inflection Points are those points on a curve
where the curvature changes direction, shown in the curvature comb display as a crossover. These points can be shown on the curve.
Where to Find It
I
Shortcut Menu: Right-click the spline and click Show Inflection Points
Menu: Select the spline and click Show Inflection Points
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I
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Inflection Points
9
Minimum Radius.
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No
Right-click the curve and click Show Minimum Radius. A graphic circle, tangent to the curve, appears on the screen. A radius value is attached to the circle.
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10 Inflection Points.
Right-click again turn off Show Curvature Combs.
Turn on the Show Inflection Points option.
11 Turn off the displays.
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A small bow-tie symbol appears at each inflection point in the curve.
Right-click the intersection curves, and turn off Show Inflection Points and Show Minimum Radius. 12 Cancel the sketch.
Continuity Explained
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Exit the sketch discarding the changes.
The concept of continuity applies equally to curves and surfaces (faces). For practical purposes, there are three types of continuity that we are concerned about in CAD systems. They are: I I
Do
No
I
Contact, or C0 continuity, Tangent, or C1 continuity, and Curvature, or C2 continuity.
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While there are orders of continuity higher than C2, they are not used in the SolidWorks software and therefore will not be addressed here.
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The concept of continuity can be explained using a series of spirals. In each case we are looking at how the gray surface patch is related to the colored spiral. Remember: continuity applies equally to curves and surfaces. We are only using surfaces here because the illustrations are clearer.
Thanks to Bill Campbell of R&D Engineering for submitting this example.
Do
No
In the first case the gray surface isn’t even touching the spiral. This represents no continuity at all. This condition is referred to as discontinuous.
In the second case, the gray surface is touching the colored spiral. They share a common edge but that is all. This represents contact, or C0 continuity.
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In the third case, the gray surface is not only touching the colored spiral, it is tangent to it. This represents tangent, or C1 continuity. While C1 continuity technically provides a smooth transition between the two surfaces, it is not very pleasing aesthetically. This is because of the sudden change in the radius of the two adjoining faces. At the common edge, the spiral has a radius of about 65mm. The gray surface is flat; its radius is infinite. In a finished product, this abrupt change can be both seen and felt. Tangent continuity is acceptable for most applications with the exception of Class A surfacing.
Note
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In the final case, the gray surface is touching the colored spiral (C0 continuity), is tangent (C1 continuity), and it has the same curvature as the spiral. This represents curvature, or C2 continuity. It is important to note that to have C2 continuity, you also have to have C0 and C1. When two adjacent faces have C2 continuity, we often say they are curvature continuous.
Zebra Stripes simulate the reflection of long strips of light on a very shiny surface. Using zebra stripes you can see wrinkles or defects in a surface that may be hard to see with a standard shaded display. Also, you can verify that two adjacent faces are in contact, are tangent, or are curvature continuous.
Introducing: Zebra Stripes
Properly interpreting the zebra stripe display requires some explanation. To illustrate, we will look at some examples using a box with a fillet.
Boundary Conditions
The way the zebra stripes appear when they cross the boundaries of faces tells you how the faces within a part are blended one into the other.
No
Zebra Stripes
Do
Tangent
314
Contact
Curvature Continuous
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There are three boundary conditions: I I
Where to Find It
I I
Contact – the stripes do not match at the boundary. Tangent – the stripes match, but there is an abrupt change in direction or a sharp corner. Curvature continuous – the stripes continue smoothly across the boundary. Curvature continuity is an option for face fillets.
Rotate the view and watch how the pattern of stripes changes. Pay particular attention to how the stripes blend from the face of the bottle to the fillet. The fillet is matched in tangency, but not curvature. Save this view display state so you can return to it later.
Curvature Continuous Fillets
The Curvature continuous option for face fillets creates a smoother transition between adjacent surfaces. Only face fillets can be curvature continuous. There are two ways to specify the radius of a curvature continuous, face fillet: 1. Specify a Radius value. 2. Use the Hold line option. This requires two hold lines, one for each set of faces.
Where to Find It
I
Fillet PropertyManager: Click Face fillet, expand the Fillet Options group box, and click Curvature continuous
No
14 Turn off zebra stripes. 15 Rollback.
Do
Right-click the fillet, and select Rollback
.
16 Second split line.
Open a sketch on the bottom face and create an offset of 0.375”. Use this sketch to split the bottom face.
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17 Roll forward and Edit Feature.
Right-click in the FeatureManager design tree and select Roll to Previous. Edit the definition of the fillet.
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The face set list that represents the bottom of the bottle (Face Set 1in this example) now has two faces listed because the bottom was split into two during step 16.
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Click in the Hold line list, and select the edge of the face for the second hold line.
Second Hold Line
Click Curvature continuous, and OK.
18 Intersection curves.
Repeat the procedure you used in step 5 on page 309 to create a new set of intersection curves that represent the bottle with the curvature continuous fillet.
19 Inspect the curvature.
Do
No
Notice particularly how the curvature display for the fillet has changed. The unequal lengths of the curvature comb indicate that the fillet is not circular in cross section. This is understandable. Curvature continuous fillets are not circular. Also, the last comb element on the body and the first element on the fillet are the same length. This indicates that the fillet is curvature continuous with the body of the bottle.
how the stripes blend from the body of the bottle to the fillet.
23 Save and close the part.
Wrap Feature
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22 Turn off zebra stripes display.
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The Wrap feature takes a flat sketch and wraps it around a cylindrical or conical surface, embossing (adding material), debossing (removing material) or scribing (splitting faces). The sketch must be a single or multiple closed loop, (not an open loop), and must be on a plane that is parallel to a plane that is tangent to the surface.
1
Extrude a cylinder.
Open a new part using the Part_MM template.
On the Top reference plane, draw a circle with a 250mm diameter centered on the Origin. Extrude a thin feature 180mm tall with a wall thickness 25mm to the inside.
2
Define a plane.
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No
Create a reference plane tangent to the cylinder and perpendicular to the Right reference plane.
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3
Draw a sketch to wrap. Change to the Front view.
Equation.
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4
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On the newly created reference plane, draw a sketch as shown.
Write an equation that sets the overall length of the sketch equal to pi times the diameter of the cylinder.
5
Introducing: Wrap
Exit the sketch.
The Wrap feature will emboss (add material), deboss (remove material) or scribe (split faces) a sketch around a cylindrical or conical face.
No
The Wrap feature can also deboss or emboss while allowing you to specify a pull direction. This is for creating inset areas on plastic parts.
Where to Find It
I
Do
I
318
CommandManager: Features > Wrap Menu: Insert, Features, Wrap
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6
Click Wrap
.
If you have not pre-selected the sketch, the system will prompt you to select one. Select the cylindrical face. Select Deboss and set the Thickness to 12.5mm. Fillet. Add 25mm radius fillets to the corners of the cam
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track.
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7
8
Save and close the part.
Name the part Cylindrical_Cam.
Note
Better cam design would use spline transitions rather than simple fillets, to make the transitions smoother. A fit spline might be used for the contour instead of simple lines.
Deform Feature
Deform is a feature which can alter an existing solid or
surface body regardless of the existence of any parametric data. That is to say that you can deform native SolidWorks parts as well as imported geometry.
No
The Deform feature supports three types of deformation: I I
Do
I
Introducing: Deform
Where to Find It
Point Curve to curve Surface push
Deform provides a simple way to change virtually any model, whether
organic or mechanical, and is useful when creating design concepts or making geometric changes to complex models that would otherwise take too long using traditional sketch, feature, or history editing. I
Menu: Insert, Features, Deform
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Point Deformation
The Point option allows you to apply a bump to a part at a point, and allows you to control the diameter of the effected area as well as the height of the bump. The Deform Distance the deformation will be.
determines how high off the face of the part
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The Deform Radius determines the size of the area to be effected. The center of the radius is the selected sketch point. The Shape Options determine the cross-section of the deformation. I I
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I
Stiffness - Minimum Stiffness - Medium Stiffness - Maximum
1
Open the part Deform. This part is a native SolidWorks part, but it could have been imported and the same functionality would be available. Also note that the changes in shape we will make to this part are independent of the features which created the part.
2
Apply a split line feature. Create a Split Line to break the curved face of the
model. This split line will be the dividing line between the finger grip section and the rest of the grip.
Do
No
The sketch should be drawn on the Front reference plane of the part and curve with the part. A 3 Point Arc works well with a radius of about 300mm.
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3
Place a 3D sketch point on the model.
Open a 3D sketch and insert a sketch point directly on the face of the model.
Exit the sketch.
5
Click Deform . For Deform Type, click Point.
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4
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This sketch point will be the center of the Point deformation.
For Deform Distance enter 3.8mm.
For Deform Radius enter 63.5mm and click Deform region.
No
Under Shape Options, click Stiffness - Medium and Maintain boundary, which limits the deformation to the just the face that has the point on it.
6
Click OK.
Do
This is an example of a shape that may be difficult to model directly using lofts or may be difficult to add to an imported body.
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Curve to Curve Deformation
7
Second deform feature.
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The Curve to curve option is a precise method for deforming complex shapes that transition from initial curves to target curves. The initial and target curves can be edges of faces, surfaces, and section curves, or free sketch curves.
Show the Finger Grip sketch and click Deform 8
.
Create the finger grip. Click Curve to curve and select the model edge as the Initial Curves as shown below.
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Select the spline in the Finger Grip sketch as the Target Curves . For the Fixed Curves/Edges/Faces deformed face from step 5 as shown.
Note
, select the
Initial curves cannot touch fixed entities.
If the preview does not match the Target Curve closely enough, move the Shape Accuracy slider to the right.
No
Fixed Face
9
Click OK.
Do
This is another example of a shape that may be difficult to model directly using traditional techniques.
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The Surface push option modifies surfaces of target bodies by pushing tool bodies into them. You can select a customizable pre-built tool body or use your own tool bodies.
Tool Body
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Surface Push Deformation
The surface push deform approximates the surfaces of the tool bodies, while maintaining the identities of the surfaces of the target bodies (the number of faces, edges, and vertices remains unchanged in the final target body).
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Surface push deform provides more efficient control of the deform shape as compared to point deform. It is also a predictable way to create specific features based on tool body shapes.
Use surface push deform to design free-form surfaces, tooling, plastics, soft packaging, sheet metal, and other applications where it is useful to incorporate the characteristics of tool bodies into existing designs.
Joining Surfaces
In the next step we will create our own tool body. We want to do this by extruding a sketch using the Offset From Surface end condition. However, the sketch spans two faces, and the command only allows us to select one face. We need a way to combine two faces into a single surface body. This means utilizing surface and solid modeling techniques together which is fairly common in advanced modeling.
Introducing: Knit Surface
Knit Surface takes faces that touch edge to edge with no gaps or
overlaps and combines them into a single surface body.
Knit Surface is introduced here to demonstrate one of the advantages
of surface functions even if you only create solid models. Surfacing techniques are dealt with extensively in the Surface Modeling course.
The system knits copies of the two faces together, creating a single surface body. A Surface Bodies folder is added to the FeatureManager design tree.
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Select the two faces as shown and click OK.
The visibility of folders in the FeatureManager design tree is controlled by Hide/Show Tree Items in Tools, Options.
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Note
11 Extrude.
Extrude the sketch named Thumb Rest using the end condition Offset From Surface. The Offset Distance is 2.5mm.
Offset From Surface has two solutions. The
extrude can stop 2.5mm short of the surface, or 2.5mm beyond the surface. We want the extrude to go beyond the surface. Examine the preview and if necessary, click Reverse offset.
Select Surface-Knit1 from the fly-out FeatureManager.
Do
No
Clear the Merge result option and click OK.
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12 Hide the surface body. Right-click Surface-Knit1 and click Hide
.
13 Click Deform . For Deform Type, click Surface push.
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For Push Direction, select the Front reference plane. For the Deform Region select the two curved faces of the grip and the main solid body.
For the Tool Body select the extrude feature that was made from the Thumb Rest sketch.
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Set the Deform Deviation to 1.25mm. The smaller the value the more closely the deformation conforms to the tool body. The larger the value, the more subtle the effect of the tool body is. The tool body was built in the correct position so we do not use either the triad or the Tool Body Position options in the PropertyManager.
No
Click OK.
14 Hide the tool body.
Do
Right-click on the tool body either in the graphics window, in the Solid Bodies folder, or on the feature that created it, and click Hide .
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In step 13 we selected the solid body to deform and we selected two additional faces. What is the purpose of selecting those additional faces?
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Why Select Faces and the Solid Body?
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15 Results.
It is to limit the deformation to just the selected faces. If no faces are selected, the entire body is affected.
A look at the back of the finished part verifies this.
With additional faces selected
Without additional faces selected
16 Save and close the part.
The Move Face feature can operate on geometry in three different ways:
No
Move Face and Delete Face
I I
Do
I
Offset faces, moving them in a direction normal to the face. Translate faces, moving them in a selected direction. Rotate faces, rotating about a given linear axis.
Introducing: Move Face
Move Face will move a face on a solid or surface body, and extend or
Where to Find It
I
trim adjacent faces to match. Menu: Insert, Face, Move
Delete Face was introduced in Lesson 7: Lofts on page 246.
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1
Import a Parasolid file.
Open the Parasolid file named Move_Face.x_t.
2
Increase the length of the large cylinder.
Select
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Select the fillet and end faces of the large cylinder.
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Use the Part_MM template.
Click Move Face
.
Click Translate and set the Distance to 5mm.
Select the Top Plane to define the translation vector.
Click Flip direction to make the cylinder longer. Click OK.
Remove the fillets. Click Delete Face
No
3
and select the three fillet
Do
faces.
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4
Delete and patch.
The default setting for Delete Face is Delete and Patch, which untrims neighboring faces to patch the hole left by the missing face.
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Click OK.
Preview
5
Results
Increase the diameter of the large cylinder. Using Move Face, and the Offset option,
increase the diameter of the large cylindrical face by 10mm.
6
Chamfer.
Apply new 3mm x 45° chamfers to replace the three fillets removed in step 4. Save and close the part.
Do
No
7
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1
Open the part Delete_Face.
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Notice that when the boss was revolved, some extra material stuck out of the part. This is because the Up To Surface end condition for the revolved boss would not work because the profile intersects the surface that defines the end condition.
2
Remove the extra geometry.
Using Delete Face with the Delete and Patch option, remove the unwanted faces.
3
The Hole Wizard was introduced in the SolidWorks Essentials course.
The Hole Wizard requires a sketch containing points that locate the centers of the holes. This sketch can either be a planar, 2D sketch, or a 3D sketch.
Do
No
Using 3D Sketch with the Hole Wizard
Save and close the part.
If the sketch is 2D, all the holes will lie on the same plane and their directions will all be normal to that plane. 3D sketches enable you to place hole centers on non-planar faces, as well as on multiple faces where the holes go in different directions. The four counterbored holes in the part shown were created by a single Hole Wizard feature using a single 3D sketch.
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Open the part named 3D_Sketch_Hole_Wizard.
The appearance of the part has been made semi-transparent so it will be easier to see the previews of the hole features. 2
Rollback before the chamfer and fillet.
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1
We are going to use midpoints of edges to help locate the holes. To make sure the midpoints are in the correct locations, rollback before the chamfer and fillet features. Hole Wizard. Click Hole Wizard on the Features toolbar, or click Insert, Features, Hole, Wizard.
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3
Make sure the Type tab is showing.
Set the properties of the hole as follows: I I I I I I
4
Hole Specification: Counterbore Standard: Ansi Metric Type: Socket Head Cap Screw Size: M5 Fit: Normal End Condition: Up To Next
Click the Positions tab. Click 3D Sketch because we want to create
multiple holes with different orientations on different faces.
No
The Point tool is active.
Do
5
330
Select the faces.
Select the four faces on which we want to place holes. The system automatically adds On Surface relations to the selected faces and generates previews of the holes.
SolidWorks 2012
Lesson 8 Other Advanced Tools
6
Locate the first hole.
Now that we have the holes in their approximate locations, we will use construction geometry, sketch relations, and dimensions to precisely locate the points.
7
Locate the second hole.
This point should have: I
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I
On Plane relation to the solid face (created automatically in step 4). On Plane relation to the Front
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The first hole should be located in the center of the face as shown. Sketch a construction line between the diagonal vertices of the face. Add a Midpoint relation between the construction line and the point.
I
8
reference plane. Dimensioned 10mm from the vertical face as shown.
Locate the hole on the curved face. Activate the Front reference
plane.
Click View, Temporary Axes.
Sketch two construction lines: one vertical and one at a 45° angle. Both construction lines should be Coincident to the temporary axis.
Add a Coincident relation between the angled construction line and the sketch point for the third hole.
Deactivate the Front plane by double-clicking in the blank space of the graphics window. Locate the fourth hole.
No
9
Do
The final counterbored hole has to be centered with respect to the highlighted face shown in the image to the right. There are a number of ways this can be accomplished. In this example we will use construction lines.
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Sketch a construction line between the diagonal vertices of the face.
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Starting at the midpoint of the construction line, sketch a second construction line capturing the Along X relation.
Add a Coincident relation between the sketch point and the construction line. Remember: The point already has a On Plane relation to the face of the solid.
10 Click OK and Roll to End. Click OK to create the Hole Wizard
feature.
Right-click in the FeatureManager and click Roll to End.
No
11 Save and close the part.
Do
Performance Considerations
Performance Settings
When working complex parts, performance tends to slow as the geometry gets more complex. Sweeps, lofts, variable radius fillets, and multi-thickness shells all have an impact on system resources and performance. There are, however, some steps you can take to minimize this impact and optimize system performance.
The Performance tab for Tools, Options, System Options contains settings which affect all documents. Turning off shaded previewing can improve performance.
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The Image Quality settings for Shaded and Wireframe (Tools, Options, Document Properties) also have an impact on system performance.
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Use the lowest possible settings that still give acceptable image quality.
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Image Quality
Suppressing Features
Suppressing a feature causes the system to ignore it during any calculations. Not only is it removed from the graphic display, the system treats suppressed features as if they aren’t even there. This will significantly improve system response and performance when working with complex parts.
Parent/Child Relationships
Parent/child relationships affect suppressing features. If you suppress a feature, its children will automatically be suppressed also. When you unsuppress a feature (turn it back on again) you have the option of leaving its children suppressed or unsuppressing them as well. The second implication of parent/child relations and suppressed features is that you cannot access or reference any of the geometry of a suppressed feature. Therefore, you need to give careful consideration to modeling technique when you suppress something. Don’t suppress a feature if you will need to reference its geometry later.
Accessing the Suppress Command
There are several ways to access the Suppress command: I I
Press Esc to interrupt the regeneration of a part. This also works when opening parts, during rollback, and so on.
No
Interrupt Regeneration
Shortcut Menu: Right-click a feature and click Suppress Menu: Edit, Suppress
Do
When you interrupt the regeneration of a part, the system completes regeneration of the current feature and then places the rollback bar after that feature.
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Exercise 28
SolidWorks 2012
Face Fillets
Exercise 28: Face Fillets
In this exercise, apply face fillets as described.
I
Procedure
Face Fillets on page 248 and page 300.
Begin with an imported part. Import the Parasolid file named Gasket_Frame.x_t. Use the Part_MM template.
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1
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This lab reinforces the following skills:
2
Apply first face fillet.
The loop around the inside of the part has several features in it that will cause edge fillets to fail.
Apply a face fillet with a 2.75mm radius.
3
Apply outside loop fillet.
The outside loop of this part has an existing chamfer on it. Apply a face fillet with a radius of 1.5mm over the chamfer. Save and close the part.
Do
No
4
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Exercise 29 Variable Radius Fillet
Exercise 29: Variable Radius Fillet
In this part create a variable radius fillet to fit as specified. This lab reinforces the following skills:
Procedure
Variable Radius Fillets on page 294.
Open the part Faucet_Cover. 1
Full round fillet.
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I
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Apply a full round fillet to the narrow end of the part.
2
Variable radius fillet.
Apply a variable radius fillet as shown.
3
Link radius values.
Do
No
Use global variables to link symmetric radius values.
4
Save and close the part.
335
Exercise 30
SolidWorks 2012
Hold Line Fillet
Exercise 30: Hold Line Fillet
Use the provided part, images and dimensions to create a curvature continuous face fillet using hold lines. I I
Procedure
Split Line on page 190. Curvature Continuous Fillets on page 302.
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This lab reinforces the following skills:
Open the part Faucet_Cover-Holdline.
This is the same base part as was used in the previous exercise, but this time we will use hold lines to create a curvature continuous face fillet. Draw a spline. On the Right reference plane, sketch a spline like the one shown. The
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1
spline will be used to create a split line to constrain a fillet. Add a Horizontal relation to the spline handle nearest the origin.
Note
To add the Horizontal relation, you must select the option Enable Spline Tangency and Curvature handles in Tools, Options, System Options, Sketch.
No
Use Show Curvature Combs and/or Show Inflection Points to make sure that the spline is always convex and smooth.
Do
2
336
Create a split line.
Use the spline to create a split line around the three tangent faces.
SolidWorks 2012
Exercise 30 Hold Line Fillet
3
Create another split line. On the Top reference plane, sketch a
One technique for creating symmetrical splines is to sketch construction lines using dynamic mirroring and then connect the ends of the construction lines with the spline.
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Tip
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symmetrical spline and create a second split line.
Another technique is to simply sketch the spline using dynamic mirroring.
4
Create the fillet.
Do
No
Create a curvature continuous face fillet using the two split lines as hold lines.
5
Save and close the part.
337
Exercise 31
SolidWorks 2012
Move Face
Exercise 31: Move Face
Use Move Face to edit imported bodies. This lab reinforces the following skills:
Procedure
Move Face on page 326.
Open the part Forged_Bracket. 1
Move end faces.
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Select the faces of the four holes and move them 10mm, using the Front Plane for the Direction reference.
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I
After you select the first hole click All co-
directional full cylindrical/conical on
the menu to select the other three holes.
2
Move the end faces.
No
Select the six end faces by selecting the front face and clicking All surrounding on the menu. Use the Front Plane for the Direction reference and move them 12.5mm.
Do
3
Tip
338
Reduce the diameter of bar.
Select all the faces of the bar feature except for the flat underside face (seven of them) and use the Offset option, with a distance of 1.5mm. Right-click one of the curved faces of the bar and use Select Tangency to select the faces of the bar.
SolidWorks 2012
Exercise 31 Move Face
4
Make the bar taller.
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Again select the seven faces of the bar and Translate them upwards 6.25mm using the Top reference plane for the Direction reference.
5
Measure distance.
Rotate the view so you can easily see the underside of the part.
Use Measure Distance to determine the distance between the underside of the bar and the bottom face of the part.
6
Extend lower face of the bar.
Select the underside face of the bar as shown and move it 19.05mm so it is flush with the underside of the bracket. The Direction reference can be a planar face as well as a reference plane.
No
Note
7
Resize the holes.
Do
Reduce all the holes by 2.5mm.
8
Close and save the part.
339
Exercise 32
SolidWorks 2012
Delete Face
In this exercise you will apply the various options available with the Delete Face feature. This lab reinforces the following skills: I
Procedure
Delete Face on page 246.
Open the part Delete_Face-imported. 1
Delete and patch. Click Insert, Face, Delete.
Bump to remove Artifact to remove
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Exercise 32: Delete Face
Split face to remove
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Select the split face and the two faces that make up the artifact. Use the Delete and Patch option.
The Delete and Patch option completely removes the edges around the faces, and restores the underlying, untrimmed base surface.
2
Remove the bump.
Click Insert, Face, Delete.
Do
No
Use the Delete and Fill and the Tangent fill options.
340
SolidWorks 2012
Exercise 32 Delete Face
3
Analyze results. The Delete and Fill option automatically creates a Filled Surface
feature to patch the hole. At first glance the results look pretty good. The Filled Surface feature is covered in depth in the Advanced Surface Modeling course.
Note
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Click View, Display, Curvature or click Curvature on the View toolbar. The curvature discontinuity around the edge of the patch is clearly visible.
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Edit the DeleteFace2 feature and select the Delete and Patch option. Notice the improvement.
Delete and Fill
Tip
Delete and Patch
Turn off RealView Graphics before viewing the curvature display. Save and close the part.
Do
No
4
341
Exercise 33
SolidWorks 2012
Hole Wizard and 3D Sketches
Exercise 33: Hole Wizard and 3D Sketches
Create this by following the steps as shown.
Procedure
I
Using 3D Sketch with the Hole Wizard on page 329.
I
3D Sketching on page 136.
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This lab reinforces the following skills:
Open an existing part named Hole_Wizard. 1
Reference planes.
Create two new reference planes as follows: Offset Distance – offset 25mm from the Front plane.
I
At Angle – angle of 10°
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I
Do
No
using a temporary axis and a model face.
342
SolidWorks 2012
Exercise 33 Hole Wizard and 3D Sketches
2
Hole size. Click Hole Wizard
.
Choose the settings for the description “CBORE for M6 Hex Head Bolt”. Use the Up To Next end condition.
3
Placement.
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Click the Position tab and select the curved face as shown. This automatically creates a 3D sketch.
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Position the hole’s locating point in the 3D sketch by adding On Plane relations to both the 25 off and the 10 deg planes.
4
Patterns.
Do
No
The objective is to have 5 holes equally spaced through a total angle of 160°, on both the front and back of the part, for a total of 10 holes. Do this by patterning the hole.
5
Save and close the part.
343
Exercise 33
SolidWorks 2012
Do
No
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Hole Wizard and 3D Sketches
344
projected 143, 151 spiral 185 split line 191, 320, 336–337 split lines 190 through XYZ locations 158
Numerics 3D curves 143, 151, 308 See also curves 3D sketches 136–140, 174, 177, 342 space handle 136
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Index
A analysis curvature 305 deviation 247 analyzing geometry 305
B background images 133 bodies to keep dialog 64 boundary feature 260–262
Do
No
C combine 36 combined bodies examples 37 combining bodies 36 common bodies 50 composite curve 145 connectors 283, 286 constant width fillets 303 constraints 231 See also relations control points 295 convert entities 77, 153, 156, 244, 267, 277 copy sketch 234–235 See also derived sketch counterbore, See hole wizard curvature definition of 305 display 305 equal 13 inspect 305 show combs 306 curvature comb 336 curvature continuous fillets 302, 315, 337 curve file 158 curves composite 145 editing 159 from a file 158 helix 142 intersection 308
D deform 319 curve to curve deformation 322 point deformation 320 surface push deformation 323 delete body 57 delete face 246, 326, 340 delete and patch 329 delete picture 133 deleting solid bodies 57 deleting surface bodies 57 derived sketch 237, 278 See also copy sketch detailed preview 29, 66 deviation analysis 247 display curvature 305 dissolve library feature 150 dividing a curve, See split entities dividing an entity 244 dome 115 draft 233 in extruded features 250 drag and drop library feature 150 drill, See hole wizard
E edit curve data read from file 159 suppress 333 end conditions up to next 250 entities convert 77, 153, 156, 244, 267 split 244 equal curvature 13 explode, See dissolve library feature F face blends 248, 300 face fillets 248, 300 hold lines 303 faces
345
Index
SolidWorks 2012
G geometric relations along x 136 along y 136–137 along z 136–137 collinear 156 considerations in lofting 205, 209 on plane 140, 180 on surface 179 pierce 105, 144, 152
M merge result 26–27, 31, 52, 55, 58–59 merge smooth faces 125 merge tangent faces 125 mesh 239 minimum radius, show 310 mirror sketch 237 modify picture 133 modify sketch 236–237 move face 326, 338 offset 328 translate 327 move/copy body 33 multibody parts 26–27, 58–74 combining bodies 36 common bodies 50 creating 26 creating with cuts 64 feature scope 29 local operations 58 merge result 26–27, 31, 52, 55, 58– 59 merging 59 merging using loft 234 saving as assemblies 65 saving bodies as parts 65 sweep 106 tool body 32 multi-thickness shell 154
preview, detailed 29, 66 project curve 143, 151 propagate along tangent edges 214 properties, feature 333 R reading curve data from a file 159 reference geometry composite curve 145 curve through XYZ points 158 helix 142 project curves 143, 151 regeneration, interrupting 333 relations pierce 186 relationships, parent/child 333 replace picture 133 round corners 293
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H helix 142 hold line, fillets 304 hold lines 303 hole wizard 342 hollowing a part, See shelling a part
258 centerline 235, 240, 242 closed loop 287 compared to sweep 226 connectors 239, 243, 259, 283, 286 merging a multibody 234 mesh 239 preparing the profiles 241 reorder profiles 230 rules for profiles 241 tangency control 231–233
I indent 54 inflection points 276, 311 insert composite curve 145 curve through XYZ points 158 derived sketch 237 fillet 303 helix 142 loft 229 part into an existing part 32 picture 133 shell 154 solid body into new part 65 spline 8 split line 190 inspect curvature 305 interpolate 146, 228 interrupt regeneration 333 intersection curves 308
No
K keep edge 292 keep features 290 keep normal constant 197–199 keep surface 292
Do
L layout sketch 253, 275 library features 149–150 dissolve 150 feature folder 150 light lines, See zebra stripes lights 131 local operations 58 loft 229, 273 advanced 251 basic 228 blending between two bodies 234,
346
O offset plane 250 options 65, 301 orientation and twist control 196, 200– 213 follow path 197–199 keep normal constant 197–199 P parent/child relationships 333 parts inserting 32 inserting a solid body into a new part 65 performance considerations 332–333 pictures as backgrounds in parts or assemblies 133 pierce 186 planes offset 250
S saving solid body as a part 65 section views 154 select through faces 294 selecting items propagate along tangent edges 214 SelectionManager 119, 214 setback fillets 297 sharing sketches 243 shelling a part 154, 251 show curvature combs 306 show inflection points 311 show minimum radius 310 silhouette edges 156 sketch 3D 136–140, 174, 177, 342 convert entities 77, 153, 156, 244, 267, 277 copying 234–235 See also derived derived 237, 278 See also copy fully defined 14 intersection curve 308 layout 253, 275 modify 236–237 sharing 243 sketch picture 14 split entities 244 solid bodies folder 27, 31, 36, 59, 65, 68, 75 solid sweep 215 space handle 136 spiral 185 splines 8, 272, 336 control polygon 9 curvature comb 9, 306, 336 fit 13, 147, 280–281 handles 9 inflection points 9, 276, 311 minimum radius 10 proportional 255 spline points 9 split entities 244 split line 190–191, 320, 336–337
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splitting curves, See split entities splitting faces 191, 320, 336–337 stock feature 65 suppress features 332–333 surfaces delete 57 sweep align with end faces 213 along model edges 213 compared to loft 226 components 100 controlling twist 196, 200–213 follow path 197–199 guide curve 185 guide curves 103, 105 keep normal constant 197–199 merge smooth faces 125 merge tangent faces 125 multibody 106 options 106 orientation and twist control 196, 200–213 path 101, 103 profile 100 propagate along tangent edges 214 section 100, 105 show intermediate profiles 108, 196 show preview 107 tool body 215 twist 212 symmetry 13, 337
Index
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SolidWorks 2012
T tangent 146, 231 tap, See hole wizard threads, modeling 155 TIFF images as backgrounds 133 tool body 32, 215, 325 tools, options 65, 301 transitions straight and smooth 296 twist controlling in sweeps 196, 200–213 twisting along a sweep path 212
No
V variable radius fillets 294 variational sweep, See sweep, guide curves view picture 133
