A New Openness1 Feb, 2001 By: John E. Wilson
In Release 5 of Autodesk's Mechanical Desktop, profiles no longer need to form a closed loop. In fact a profile can be as simple as a single line. They are created by the same command, AMPROFILE, that is used to create closed profiles, but in the Desktop Browser these new open profiles have the prefix "Open" attached to their feature names. You can use only three commands-AMEXTRUDE, AMRIB and AMBEND-with open profiles. In this column we will look at those commands to find out how to use them and see what we can make with open profiles.Extrusions
You can't revolve, sweep or loft open profiles, but you can extrude them. In setting the parameters for such an extrusion, you assign a thickness, or width, to the open profile when creating a 3D feature. Mechanical Desktop lists the resulting 3D feature in the Desktop Browser as a thin extrusion, even though there are no thickness restrictions other than the profile's inability to self intersect. You can't, for example, assign a thickness to a U-shaped profile that is larger than the radius of the arc in the profile.
When you invoke AMEXTRUDE and select
an open profile, Mechanical Desktop displays an expanded version of the Extrusion
in the bottom panel.
The open profile, though, consists of just three lines and requires only
six constraints, while the closed profile consists of eight profile line,
two construction lines and requires 18 constraints.
dialog box for you to use in setting the thickness. You can have the thickness
value applied exclusively on one specified side of the profile or for an equal
distance on both sides of the profile. You can also use one thickness value
for one side of the profile and another value for the other side.
Figure 1. The 3D feature shown in the top panel can be made by extruding either the open profile shown in the middle panel or by extruding the closed profile shown
Your main reason for using open profiles in creating extrusions is likely to be that for some geometric shapes, they require less work than a closed profile. Not only do they have fewer objects, they need fewer constraints and dimensions. An example is shown in Figure 1. The top panel in this figure shows an extruded 3D feature. You can make that 3D feature by extruding either the open profile shown in the middle panel, or by extruding the closed profile shown in the bottom panel. The open profile, though, consists of just three lines and six constraints (four dimensions and two horizontal geometric constraints). The closed profile, on the other hand, requires eight profile lines, two construction lines and 18 constraints (five dimensions and 13 geometric constraints).
Figure 2. When you extrude an open profile, an option named Extend lengthens the profile until it meets a face as shown here. Thus, the single-line open profile that requires just one dimension shown on the left in this figure can create the web-like feature shown on the right.
Ribs are a sketched 3D-feature type introduced in Mechanical Desktop Release 5. You will often use them to model
Figure 3. Mechanical Desktop's new Rib features model the ribs that add strength and support to the parts. Ribs are easily made from open profiles, and you will often make a polar or rectangular pattern of the rib feature.
Rib features can only be used as dependent features.
They can only be created from an open profile, and the length of the profile automatically extends in both directions to an adjacent face. Also, if the profile is too long and extends beyond an adjacent face, it is trimmed back to that face. The profile can contain multiple open objects-lines, arcs and so forth-that are connected end-to-end.
You specify the thickness of the rib in a dialog box.
The rib is formed by pushing the profile along the plane of the sketch plane, rather than perpendicular to the sketch plane as extrusions do.
The rib feature terminates as the profile meets existing faces.
Rib features cannot have draft angles.
Rib features are created by the AMRIB command.
Although you can use AMEXTRUDE to create the geometry of a rib feature, AMRIB is usually much easier to use. Since Mechanical Desktop extends the open profile of the rib to meet adjacent faces, you often do not need to draw the entire rib, and you will add just enough constraints and dimensions to fix its position on an existing feature and to fix important points within the profile. Often, multiple ribs are needed to fully strengthen a part so, as shown in Figure 3, you will make a polar or rectangular pattern of a rib feature.
AMRIB displays a dialog box for you to specify the thickness of the rib. You can specify that the entire thickness of the rib will be offset to one side or the other from the profile or offset evenly on both sides of the profile. You can also specify a separate thickness value for each side of the profile. Mechanical Desktop will display the profile in its specified thickness and indicate the extrusion direction of the rib with an arrow. You can flip the direction of the arrow. Unlike the operations that create other sketched 3D features, you do not specify a termination because the rib automatically ends as the profile meets faces.Bend Features
Release 5 of Mechanical Desktop also introduces Bend features. Unlike the other sketched 3D features, bend features
Figure 4. The upper section of this figure shows two single-line open profiles that you use as bend lines in making two bend features. The resulting bend features are shown in the lower section.
Bend features are created by the AMBEND command. This command first asks you to select one open profile to serve as the bend line, and then displays the Bend dialog box. In this dialog box you select one of three combinations for specifying the bend's size parameters: (1) angle and radius; (2) radius and arc length; or (3) arc length and angle. In most cases you will choose the angle and radius combination.
Edit boxes appropriate for your selected
combination of size parameters are opened in the dialog box, and, as you enter
values in these edit boxes, Mechanical Desktop displays their effect on the
part. See Figure 5 for an example. The section of the part that will be bent
is highlighted with a blue outline. This bend side is further identified by
the presence of a straight arrow anchored on the open profile and pointing toward
the bend side. Also, the direction of the bend is indicated by a curved arrow.
Options in the dialog box allow you to flip these directions independently.
Figure 5. Mechanical Desktop indicates the bend side of the feature with a straight arrow and the direction of the bend with a curved arrow. Furthermore, the radius of the curved arrow is that of the bend radius you specify in the Bend dialog box.
If your current 3D-space viewpoint is looking directly, or almost directly, down toward the plane of the bend-line profile, or if you have specified a small bend radius, you may have trouble seeing the bend direction arrows. If this is the case, right-click in one of the edit boxes for entering bend parameters. A shortcut menu will appear, and you can select Pan, Zoom or 3D Orbit from this menu to change your viewpoint and zoom level for a better look at your part.
Bends always start at the bend profile-the profile becomes one of the bend's two tangent lines. The inside bend radius of 90-degree bends must be equal or larger than the maximum thickness of the part's cross section. The parts you bend can have any cross-section shape, provided the bend radius accommodates the cross-section thickness.
The plane of the bend profile can be on the top surface, the bottom surface or within the part you want to bend. You must, however, set the bend radius to a value that matches the part's thickness and the plane of the profile. For instance, if you intend to bend a part that has a rectangular cross section 6mm thick and the bend profile is on the bottom surface of the part, you must specify a bend radius of at least 6mm for 90-degree bends down and at least 12mm for 90-degree bends up. If the bend profile is in the middle of the part, the minimum bend radius for 90-degree bends will be 9mm for either direction.
To precisely position flanges and
holes on bend features, you must adjust the location of the bend profile to
account for the curved length of the part's surface through the bend. You can
make this adjustment by adding a factor to the dimension of the profile on the
bend side of the parent feature. For 90-degree bends this factor, which is derived
from the arc length of the bend, is 0.5707963 multiplied by the bend radius.
Suppose, for example, you intend to make a 90-degree bend having an outside
bend radius of 0.25. Furthermore, you want the top of a bend to be 1.0000 inches
from the bottom surface of the part, and the bend profile is on the bottom surface
of the part. If you dimensioned the bend profile to be 1.0000 from the end of
the bend, the resulting height will be only 0.8573 inches. If, on the other
hand, you assigned it a dimension value of 1.1427 (0.5707963*0.25+1.0000), the
resulting height will be the 1.0000 inches you want. This example is illustrated
in Figure 6.
Figure 6. To adjust for the distance through the bend arc, add a factor to the dimension that positions the bend profile. For 90-degreebends, this factor is 0.5707963 times the bend radius.
Your most common, but not only, reason
for bending 3D features will be in designing sheet-metal products. You no longer
have to move the drawing plane about, making and constraining numerous profiles
to be extruded or revolved to form walls and flanges. Instead, you can make
a flat pattern of the part, and bend it into the shape you want. Mechanical
Desktop does not, however, have the sheet-metal design capabilities that certain
Mechanical Desktop add-on products have. The program knows nothing about bend
allowances or relief cutouts, and there is no practical method for unfolding
a part. (You can, however, temporarily unfold a bend by suppressing its bend
Figure 7. This is an example of a flat pattern you might make modeling a sheet-metal part. This particular example has three open profiles for making three bends. The notes in this figure explain how the profiles are constrained.
Figure 8. Here you see the flat pattern shown in figure 7 after it has been folded and holes have been made through the rounded tabs. This model of a sheet-metal part is easily constructed when you use bend features
Even though open profiles don't significantly add to the 3D geometry capabilities of Mechanical Desktop, they certainly simplify and ease your work in making thin walled features, ribs and bends.
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