Exercising Your Design1 Jul, 2002 By: Greg Jankowski
When creating assemblies, the methods used to mate (constrain) the design can be used to document the way the product functions. This is referred to as design intent. Mates should be added to the components so they behave as they would in a physical prototype. SolidWorks allows you to use a number of different methods to capture and simulate the design intent for assemblies, including assembly motion.
This allows you to not only review and document fit and form, but also simulate the product's function within the assembly. This is accomplished by using mating constraints that allow for the analysis of motion for the assembly. When you design movable assemblies that move, fit and interference checks can be done in the open or closed state, and at any point in-between.
Figure 1. Here you can see an inkjet cartridge holder designed in SolidWorks.
Assembly motion can be depicted as follows:
- Under-constrained assembly components (Figure 1 shows an assembly where the lid moves up and down around the rear pivot point)
- Parametric mate (for instance, angle and distance)
- An assembly layout sketch or simple skeleton part
An assembly constraint is a method in which SolidWorks limits the way an assembly component or sub-assembly can move. For example, the assembly components in Figure 1 have been fully constrained except for the rear pivot-area for the lid. This allows the lid to move up and down.
An assembly component or sub-assembly has six degrees of freedom when it is dropped into an assembly. Assembly mates allow for the constraint of this freedom. If you want to create an intelligent assembly, the component should be constrained to prevent undesirable assembly motion, while allowing the under-constrained assembly components to move in the manner intended. Some assembly components may not move at all and should be fully constrained. An under-constrained assembly component has a (-) in front of the component name in the SolidWorks FeatureManager.
Typically, an assembly component needs three mates to fully constrain all six degrees of freedom. If all degrees of freedom are not accounted for (up/down, left/ right, front/back), then the assembly is under-constrained. Figure 2 shows the mate types available.
Figure 2. These are the different types of Mates.
- parallel, which constrains the components to be parallel to each other;
- perpendicular, which constrains the components to lay perpendicular to each other;
- tangent, which constrains the components so they will remain tangent to one another;
- concentric, which constrains circles to share the same origin;
- coincident, which constrains the components to lie on the same plane, face, or edge;
- distance, which constrains the components with an offset distance;
- angle, which constrains the components by specifying an angle between the components.
Exercising the Design
A good way to determine how an assembly component is constrained is to select the Move Component function, and drag the assembly component to see how it moves. If the motion is not what you expect, then review, modify, and add assembly constraints (mates) until the component is fully constrained or constrained less than the degrees of freedom required to simulate assembly motion. This can be referred to as exercising your assembly. A designer should understand how assembly components interact and how they are constrained.
Collision Detection and Physical Dynamics
Assembly motion can be analyzed by the use of collision detection. This is an option within the Move Component function. It allows a component to be moved until a collision occurs. SolidWorks will stop the movement and indicate that a collision has occurred. Using the example shown in Figure 1, a designer can determine the maximum open angle of the lid by just dragging it up. When a collision occurs, the motion stops. The maximum angle could then be measured. If the angle is insufficient, the design should then be altered.
Physical Dynamics takes this a step further by allowing for the under-constrained assembly components that are under-constrained to interact with one another. In the example shown in Figure 1, Physical Dynamics can be used to insert an ink cartridge into the holder. With physical dynamics turned on, the user could slide the cartridge in the holder and review the fit, form, and function of the holder design. To perform this study manually takes a fair amount of time and effort. Physical Dynamics allows the designer to quickly and easily get visual feedback as to whether the cartridge will slide into the holder and close the lid or not.
Configurations can be used to define the angle or distance setting for a mate. By defining the angle or distance value, the assembly component can then be precisely located or positioned. A configuration can also be used to suppress a mate that will otherwise fully constrain the assembly component. This allows for the best of both worlds: precise positioning for drawing views and assembly layouts and under-constrained assembly components for assembly--motion and physical--dynamics studies.
The example that is shown in Figure 2 has the following three configurations:
- Closed. A configuration that shows the lid in the closed state (angle mate set to 0 degrees).
- Open. A configuration that shows the lid in the open state (angle mate set to 85 degrees).
- Motion. A configuration that suppresses the angle mate and allows the lid to move between the open and closed state by dragging.
The advantages of intelligent assemblies include mating constraints that can be defined based on the actual physical mating characteristics; assemblies that can be used as a virtual prototype for the design; and collision detection that allows for under-constrained assemblies to move (SolidWorks will indicate when a collision is detected). You should also note that many of the motion-related functions can be checked prior to creating a physical prototype, which helps reduce errors and resources spent on physical prototypes; and physical dynamics can also be used, which allows for under-constrained assembly components to interact with one another.
When creating your assembly, start by defining and modeling the design intent of your product. Next, exercise your assembly to determine if your design intent was captured in the mating scheme. Finally, use the design intent to perform virtual-prototype reviews and to better communicate your design.
About the Author: Greg Jankowski
Autodesk Technical Evangelist Lynn Allen guides you through a different AutoCAD feature in every edition of her popular "Circles and Lines" tutorial series. For even more AutoCAD how-to, check out Lynn's quick tips in the Cadalyst Video Gallery. Subscribe to Cadalyst's free Tips & Tools Weekly e-newsletter and we'll notify you every time a new video tip is published. All exclusively from Cadalyst!