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Autodesk Mechanical Desktop A Clean Sweep

By Derek Chavez,2014-11-29 04:18
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Autodesk Mechanical Desktop A Clean Sweep

Autodesk Mechanical Desktop: A Clean Sweep

    By Bill Fane

    The two most common methods used to produce a solid feature from a sketched profile in Autodesk? Mechanical Desktop? software are to extrude it or to revolve it around an axis. This month's tutorial covers another method of producing a solid feature from sketches, which is to sweep a profile along a path.

    Let's start with a practical example that will help to explain the basic process. Before going to bed tonight, go into the bathroom. Use a felt pen and write "I Love You" right across the countertop. Now take the toothpaste tube, and trace along the felt-pen lines as you squeeze out a ribbon of toothpaste.

    In this example, the felt-pen lines are the sweep path and the round opening in the top of the toothpaste tube defines the profile. The toothpaste is the swept extrusion. Trust me; in the morning your spouse or significant other will be most impressed with your understanding of the principles of sweep paths.

     Figure 1: A part created by sweeping a profile along a path.

     Figure 2: Start by sketching the desired path

    The part shown in Figure 1 was made using a sweep. This part would be almost impossible to produce if you were limited to just using extrusions, but it becomes a simple three-step operation if you sweep along a path. All you have to do is:

    1. Create and constrain the path. 2. Create and constrain the profile to be swept along the path. 3. Perform the sweep operation.

    Now let's look at each step in detail.

    There Are Two Kinds of Sweep Path... No, this is not the start of a bad joke, there really are two kinds of sweep path: 2D and 3D. This month's tutorial will cover 2D paths, and next month we'll look at 3D paths. To create the part shown in Figure 1, you must first create and constrain the path. Follow these steps:

     Figure 3: Next, constrain and dimension the path.

    1. Sketch the path shown in Figure 2.

    You can draw a sweep path using lines, circles, arcs, polylines, and so on, exactly as you do with a regular part-profile sketch. There are only two limitations:

     All sketch elements must lie in the same flat 2D plane, which must be the current sketch plane. The path cannot cross itself (be "self-intersecting"). So, for example, you cannot produce a figure 8 in one sweep path. 2. When you are ready, use the AM2DPATH command to turn your sketch into a sweep path. You can start this command by:

     Entering AM2DPATH at the Command line. Going to the menu bar and selecting Part > Sketch Solving > 2D path. Going to the Part Modeling toolbar and selecting 2D Path from the flyout under the Profile a Sketch button. Right-clicking in the graphic area and selecting Sketch Solving > 2D Path from the shortcut menu. 3. Whichever method you've used to open this command, you must now select the objects for the sweep path. Use the usual Mechanical Desktop selection techniques and press the Enter key when you are done.

    4. The software now prompts you to "Select the start point of the path." Pick a point near one end of the path, which creates a work point that is automatically constrained to the end of the path.

    Note: You do not need to use an object snap because the software automatically snaps to the closest end of the selected object and creates a work point at that end.

    5. At the next prompt, you are asked "Create a profile plane perpendicular to the path?" For this exercise, just press the Enter key and accept the default of <Yes>to create the work plane. 6. Now use the usual Mechanical Desktop techniques for profile sketching to dimension and constrain the path as shown in Figure 3.

     Figure 4: Now create the profile. Constrain and dimension it.

    Note: Do not delete the Fix constraint that was automatically applied at the start of the path, or you will run into problems in the next process.

    Creating and Constraining the Profile Follow these steps:

     Figure 5: The AMSWEEP dialog box.

    1. Because the work plane you created using the AM2DPATH command is automatically set as the sketch plane, you can start sketching directly on that plane (see Figure 4). 2. When your sketch is finished, use the AMPROFILE command to turn it into a profile.

    3. Dimension and constrain the profile exactly as you would for any normal extrusion.

    The sweep path is one sketch and the profile is another. You cannot dimension or constrain between objects in two different sketches, so it would appear that you cannot constrain the profile to the path. However, what you can do is place dimensions between the profile and the work point that was created earlier, and that operation will constrain the profile to the path. In this exercise, that is the purpose of the two 0.00 dimensions in Figure 4; they tie the center of the arc to the work point and, hence, to the path. If the profile is the first object in the drawing, as in this exercise, it will have a Fix constraint to lock it to the sketch plane coordinate system. Before you dimension the profile to the work point, you will need to delete this constraint so the sketch can move.

    Note: You do not have to completely constrain and dimension the path before you create, constrain, and dimension the profile. As you apply dimensions and constraints you can shift back and forth between the path and the profile as desired.

    Performing the Sweep Operation The AMSWEEP command produces the solid feature by sweeping the profile along the path. 1. Start the AMSWEEP command by:

     Entering AMSWEEP at the command line. Going to the menu bar and selecting Part > Sketched Features > Sweep... Going to the Part Modeling toolbar and selecting Sweep from the flyout under the Sketched FeaturesExtrude button. Right-clicking in the graphic area and selecting Sketched & Work Features > Sweep from the shortcut menu. 2. Whichever method you've used to start the AMSWEEP command, the Sweep dialog box opens (see Figure 5). As you can see, the AMSWEEP command has several options (see the sidebar). For now, just click OK to accept the defaults.

    3. The profile will be swept along the path to produce the solid part shown in Figure 1. Let's take a quick look at the options available to you with the AMSWEEP command (see Figure 5).

     Figure 6: A swept profile can cut a groove into an existing part.

     At the Body type box, you can select either Normal or Parallel. Choosing Normal keeps the profile perpendicular to the sweep path, so the cross-section of the sweep is constant. Choosing Parallel keeps the profile parallel to the work plane, so the cross-section varies. The preview window in the Sweep dialog box changes to show the difference as you select one option or the other. The Draft angle box lets you specify a draft angle for the sweep, which means the profile stretches or shrinks as it sweeps along the path. In the Type box on the Termination pane, you can choose how far the profile sweeps along the path. The default is to go the full length, but you can also have the path sweep until it hits a terminating plane or have it start at the first plane it encounters then run to the next one where it stops. The preview window shows the differences. Note: See "The Cutting Edge" section for information about the Operation option.

    The Cutting Edge So far, so good. But there is no rule that says a swept profile must be the onlyor even the firstfeature in a part. Figure 6 shows a rectangular plate with a fancy groove cut in it.

     Figure 7: A swept profile can also add a ridge.

    To produce this part I:

    1. Extruded a rectangle, and then set the top face of the resultant slab as the sketch plane. 2. Drew a path similar to the one shown in Figure 3. 3. Used the AM2DPATH command to turn the path into a sweep path. But this time I did not have it create the work plane because I could set the left face of the slab to be the sketch plane. I dimensioned and constrained this profile exactly as we did before (see Figure 4). 4. Used the AMSWEEP command, which opened the Sweep dialog box (see Figure 5). 5. Chose Cut from the drop-down list of Boolean operations in the Operations box, which produced the part shown in Figure 6. With a suitable profile I could just as easily have chosen Join, and, hence, added a ridge (see Figure 7).

     Figure 8: Sweep paths can have sharp corners.

    There Is No End to This Path Figure 7 also shows another interesting variation. A sweep path does not have to be an open-ended profile like the one we've been using. It can also be a closed loop of any desired degree of complexity, and any vertex between two objects can be the start point.

    I have an off-road motorcycle, and many of the mating parts in the engine do not have gaskets between them. Instead, one piece will have a serpentine groove in one face. A thin rubber ring is set into the groove. The mating part has a matching serpentine ridge, so that when the parts are assembled the ridge compresses the ring into the groove for a tight seal. If the manufacturer had used Autodesk Mechanical Desktop to design the parts, then the groove and ridge paths would be parametric and would automatically follow any changes to the size and proportions of the parts.

    Now That's Really Kinky... Figure 8 shows that the sweep path does not have to be a smooth, flowing curve like the other examples in this exercise. Conclusion Once you understand their basic principles, swept profiles are very easy to use. Admittedly, they are not used as often as the usual extrude and revolve functions, but they will often produce a part feature that cannot be made any other way.

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