Alibre Options: Creating Assembly Prototypes in Alibre Design10 Mar, 2006 By: Michael Todd Cadalyst
Harness the power of parametric engineering.
Engineers and designers not only create individual parts, they ensure that those parts can be assembled correctly. Alibre Design helps accomplish this task. Alibre Design is a fully parametric engineering 3D CAD package. So when a file is updated, those changes will occur everywhere that file is used -- including other parts, assemblies, 2D drawings and BOMs (bill of materials). This article will discuss editing parts within an assembly and the different assembly design methodologies: bottom-up and top-down.
Editing Parts within the Assembly
You can use two different methods to edit parts from within the context of an assembly. The value in editing parts from within an assembly is that you instantly see any changes made to the part in the assembly.
The first way to edit a part is right-click the part in the Design Explorer and select Edit. When you are in this mode, you can edit the part while the rest of the parts in the assembly remain visible, therefore allowing you to add inter-design constraints between parts. (I'll explain more about this method in the next section.)
The second way is to press the Shift key while right-clicking the part in the Design Explorer. When you select Edit, the part opens in a new window separate from the rest of the parts in the assembly. The advantage of this mode is that you only see the particular part without the rest of the assembly. In both cases, because you opened the part within the context of the assembly, the changes made to the part will instantly reflect in the assembly.
You also may have multiple instances of the same part in an assembly. In such cases, when that part is edited, the changes will occur in every instance of the part. For example, figure 1 shows three instances of a bolt in an assembly. If one instance of the bolt is changed, then all three bolts will change (figure 2) because all of the bolts are actually referencing the same part. The update is not limited to the assembly. If you made a 2D drawing of the assembly, then that assembly drawing also will reflect the changed parts. If you created a BOM of the assembly and an instance of the bolt is added or removed, the BOM also will parametrically update to show the correct number of bolts in the assembly. The BOM also will automatically update if the properties of the bolt change.
Figure 1. The three yellow bolts are actually instances of the same part.
Figure 2. When a change is made to one instance of the bolt, all are updated to show the change.
Assembly Design Methodology
You can use two different methodologies when creating assemblies: top-down and bottom-up. Each technique has its own strengths and weaknesses, but you can create most assemblies using a combination of these methods to accomplish the needed design results.
In the bottom-up method, each part is created separately from the other parts. After the parts are completed, they are inserted into an assembly and constrained together. The constraints that are used mimic the effects of assembling the physical parts together. These constraints include mates, aligns, angles, orients and tangents.
In the top-down method, the parts are created within the assembly; this technique allows you to create inter-design constraints so that when a feature changes in one part, the other parts also change. Although the parts are created from within the assembly, each part becomes its own individual file when the assembly is saved. These files are still treated as regular parts -- they can open up separately from the main assembly, and you can edit and insert them into their own 2D drawing or use them in other assemblies.
When using the top-down method, you can select a planar face of one part and create features in another part from that face. In figure 3, the key was created on the outside face of the gear and the sides of the key were constrained to the outside surface of the keyway hole using the Collinear Sketch Constraint tool. The key was then extruded to the opposite outside face of the gear (figure 4). Because the key was extruded using the To Geometry setting, the key will update parametrically if the gear width changes. With the sides of key constrained to the keyway hole, the key will change automatically if the keyway is enlarged or reduced.
Figure 3. I used the Collinear Sketch Constraint tool to constrain the sides of the key.
Figure 4. The key is extruded to the opposite outside face of the gear.
As you can see, you can create assemblies faster and easier by taking advantage of existing tools and using the right method for your project. Until next time, look for me online as the Alibre Assistant in Alibre Design.
In her easy-to-follow, friendly style, long-time Cadalyst contributing editor Lynn Allen guides you through a new feature or time-saving trick in every episode of her popular AutoCAD Video Tips. Subscribe to the free Cadalyst Video Picks newsletter, and we'll notify you every time a new video tip is published. All exclusively from Cadalyst!