Autodesk Mechanical Desktop: Keeping to the Straight and Narrow
By Bill Fane
During the last few tutorials we have been working through the various 3D sweep paths available in Autodesk? Mechanical Desktop? software. This time we will cover the last two variants.
The good news is that I have run out of goofy "There are four kinds of sweep path..." introductions. The bad news is that I have not run out of bad jokes, such as "There are two kinds of people in the world; those who divide things into two categories and those who don't." 3D spline sweeps are great for creating free-flowing features like hoses and cables, but what if you want a 3D sweep to contain straight sections connected by fixed-radius curves? (Hey, that sounds a lot like a description of the piping shown in Figure 1.)
Figure 1: A section of 3D piping.
No problem. The process is very similar to that used for 3D spline sweeps. It requires just four simple steps: 1. Use the standard 3DPOLY command and create a 3D polyline. Define vertices by typing in coordinate triplets (x,y,z), by using object snaps to existing geometry, by using standard DDE (Direct Distance Entry) procedures, or a combination of the three methods. Figure 2 shows a sample 3D polyline. Don't worry about the radii to be used for elbows because a 3D polyline cannot contain arc segments anyway. This will be handled later.
Figure 2: A standard 3D polyline.
2. Start the AM3DPATH command and enter the Pipe option. When prompted, select the 3D polyline. In fact, you can select more than one polyline so long as they touch end-to-end to form a single, contiguous path. When you have finished selecting 3D polylines, you are prompted to select a start point near one end of the path.
Similar to the 3D spline path, a spreadsheet dialog box now automatically displays (see Figure 3). The function of each column in the spreadsheet should be obvious from the headings.
Figure 3: 3D Pipe Path dialog box.
There is a significant difference between the x, y, and z values in this table compared to those for the 3D spline paths we studied last time.
For a 3D spline path the values are relative to the origin of the sketch plane that was active at the time it was created. But for a pipe path the sketch plane determines the directions while the values are relative to the previous point.
You can edit any value at this point, and the path adjusts accordingly. If you change a value, succeeding segments move in order to remain horizontal and vertical. As indicated in step 1, here is where you can add radii at the corners. For now, let's leave the corners sharp and the vertices where they are. 3. When you click OK to continue, a work point and a work plane are created at the start of the path. You can now create a sketch, and then dimension and constrain it using usual Mechanical Desktop techniques (see Figure 4). Use two dimensions to tie the sketch to the work point.
Figure 4: The profile is dimensioned to the work point.
4. When you are ready, use the AMSWEEP command to sweep the profile along the path as shown in Figure 5.
Figure 5: The profile is swept along the path to produce the pipe.
Figure 6: A brick, a pipe, and two work points.
You can edit the 3D pipe path, and constrain it to existing features, using exactly the same procedures outlined previously for 3D spline paths. In this tutorial we're going to constrain the pipe path to a brick and then sweep a profile along the path (see Figure 6).
1. Draw the brick first and then add the two work points and dimension them.
2. Draw the 3D polyline to values similar to those in the previous example.
3. Start the AM3DPATH command and enter the Pipe option to turn the polyline into a pipe sweep path. 4. Sketch and constrain a circle, and then sweep it along the path.
To this point, the procedure is identical to the previous example except the brick and work points are created first. Now let's edit the path, starting with the corner radii.
5. Double-click on the sweep path object's entry in the browser. The dialog box shown in Figure 3 displays. 6. Click a box in the Radius column, enter a value, and watch as the blue sweep path updates to preview the change. You can enter different values for each corner or leave some corners sharp. Unfortunately, you cannot add a global value, but must edit each one individually. Constraining the pipe path to existing features is handled exactly the same way as it was for 3D spline paths. 7. Right-click the magnet symbol in the first row of the C column. When the shortcut menu displays, click Constrain to Work Point. You are now prompted to select a work point. Select the one close to the start of the path. The blue preview path will change to show the entire path shifting until the start coincides with the work point.
8. Similarly constrain the last point to the other work point. In this case, the last segment adjusts its length and angles until things fit.
9. Click OK to accept the edits, and then press Enter twice to bypass the next dialog box and command prompt. The drawing updates (see Figure 7).
Figure 7: The pipe has been edited and constrained.
Keep these points in mind about pipe paths:
You are not limited to a circular sweep profile. Rectangular ducting, or any other shape you want, works just as well. You can shell out the swept feature if you want hollow pipe or ducts. You can use any of the standard Boolean combinations. This means that you can join the pipe as we did in our example, or you could use a CUT operation to tunnel through to a larger piece.
Life on the Edge I have saved the easiest sweep for last, even though it appears to be the most complex.
Figure 8 shows a complex part. To create it, I extruded two ellipses and then intersected that feature with a two-arc profile.
Figure 8: A part with a complex edge shape.
Now I want to add the reverse-fillet groove feature as shown in Figure 9. This is so simple to do that it does not even require a separate sweep path.
Figure 9: The groove around the edge was created by sweeping a profile along an edge path.
1. Start the AM3DPATH command and enter the Edge option.
2. At the prompt, select existing edges on the part.
In this case, the edge formed a continuous curve so a single pick selected the entire edge. If your edge is formed from a series of lines and arcs then you must select each edge segment separately. You do not need to select all edges to form a closed loop. For example, you may want to add a groove to only three edges of a box (see Figure 10).
Figure 10: You can apply edge sweeps to some edges and not others.
3. When you have finished selecting edges, you will be asked to select a start point near the end of one segment. Select the start point.
4. You are now asked if you want a work plane placed at the start point. Click Yes. Now all you need to do is to create a sketch on the work plane, and then dimension and constrain it using the usual Mechanical Desktop techniques.
5. When you are ready, simply sweep the profile along the edge path using the usual AMSWEEP command. The profile will be swept along the part edge as shown in Figure 9. The new feature is automatically parametrically attached to the edge. Any editing of the base part automatically updates the swept feature so it still follows the edge. And in Conclusion... Over the last few months we have learned a great deal about 3D sweep paths. With them, you can easily make extremely complex parts and features. Without them, and being limited to the common extrude and revolve functions, you probably could not have made the example parts at all.