There are always a bunch of new goodies in the assembly bag, and this year is no exception. There are so many new assembly features, it makes more sense to split them up over two weeks. This week, we’ll start with enhancements to mates and pattern features.
Editing Limit Mate Values
You can now view and edit the Min and Max values of a limit mate (both angle and distance) in the Graphics Area. Simply double-click the dimension to bring up the Modify Dimension dialog box, and edit the values without re-entering the Mate PropertyManager.
The workflow for creating symmetry mates now more closely matches the workflow for other mirroring commands. You select the symmetry plane first, and then the assembly references second. Previously, the symmetry plane was selected last, even if pre-selected. This means you can now pre-select two faces and a plane, and SolidWorks will automatically select the Symmetry mate when the mate command is activated. If multiple planes are pre-selected, SolidWorks uses the first plane as the symmetry plane.
Copy with Mates
Copy With Mates now supports more advanced mates, including width, limit, and symmetry mates. The UI has also been split into two parts (component selection and mate assignment) for a cleaner workflow.
The width mate now includes functionality similar to the new-in-2014 slot mate. You can select geometry to drive the limits of width mates (as normal), and select additional options to define movement and positioning. The following options are available:
Centered: Centers a tab within the width of a groove. This is the same functionality as in previous releases.
Free: Lets the components move freely within the limits of the selected width faces. This constraint could replace and simplify a limit distance mate, especially if the width component is configured to change length.
Dimension: Sets a fixed distance (or angle) dimension from one selection set to the closest opposing selection set of faces or planes.
Percentage: Sets a fixed distance (or angle) based on a percentage of total width from one set of the selection set to the center of the other selection set.
Profile Center Mate
The Profile Center mate automatically centers and aligns simple component profiles, such as rectangular and circular parts. This single mate can fully define the components, replacing up to three separate mates. The parts can also be offset by a given distance. The mate differentiates cylindrical and rectangular parts, and activates different options for each. For example, cylindrical parts include the ability to lock rotation, while rectangular parts can be quickly rotated by 90 degrees and locked in position.
The new Chain Pattern allows you to pattern components along a path or loop, either by distance, or by keeping all components connected. This allows you to accurately simulate chains, treads, rollers, and more. Plus, combined with the new Path Length Dimension, it’s easy to control the result.
- To start a chain pattern, select the Chain Component Pattern command under the pattern dropdown.
- There are three types of Chain Pattern: Distance, Distance Linkage, and Connected Linkage. Each method is described below. Select your desired type from the Pitch Method pane of the PropertyManager.
A distance-based chain pattern doesn’t actually have much to do with chains. It simply patterns a single component along a path by locking a common point to an assembly sketch (or curve, edge, etc.). It’s probably best for things like roller bearings or roller conveyers, where all the patterned components are axially symmetric, and not linked to each other.
- Choose the chain path, using the SelectionManager if necessary. Also select the Fill Path check box if you want SolidWorks to automatically calculate the number of instances based on path length and component spacing. Otherwise, input your desired number of instances manually. You can then select Equal Spacing in the Chain Group pane to fill the path completely, or input any distance to partially fill the path.
- Select the component you wish to pattern. (You can only pattern a single component in distance mode.)
- Select the Path link and the path alignment plane. These two features are used to define a point, which is locked to the chain path. The alignment plane will also always be parallel to the path plane (or the face normal alignment plane, if using a 3D sketch). At this point, your component can move along the path, and rotate about the Path Link point.
- The resulting pattern is a combination of a path mate and a linear pattern. The pattern instances are not connected in any way to the seed, but only reflect its orientation.
Distance Linkage Method:
This option allows you to create a pattern that moves together as one unit, but does not have connected links. The pattern locks both ends of your link to the chain path, as opposed to just one end, as above. The patterned components can be equally spaced along a path, but still have accurate motion.
- As above, choose your chain path, using the SelectionManager if needed.
- Select the number of links to pattern, define equal spacing, or choose to fill the path based on the spacing distance entered in Chain Group 1.
- Select the component you wish to pattern. (As above, you can only pattern a single component in distance linkage mode.) The part you wish to pattern does not have to be mated in any way to the chain path. The pattern command will mate the part correctly when completed.
- Select two Path Link features (such as the dowel pins in the bike chain shown below), and the path alignment plane (such as the symmetry plane of the patterned component). These features are used to define two points, which are locked to the chain path. The alignment plane will also always be parallel to the path plane (or the face normal alignment plane, if using a 3D sketch). At this point, your component can move along the path, and the centers of the Path Link features are locked to the path, so there is no rotation.
- The completed pattern is starting to look more like a real chain. All the components are oriented correctly, and move as one when dragged. However, we’re still limited to patterning one component, and have to manually determine the correct spacing to make a perfect loop.
Connected Linkage Method:
The Connected Linkage method is what you really want to use when making a true chain. It allows you to pattern up to two components in a pattern defined by component lengths and linkage positions.
- Again, starting with a path and two completely unmated components…
- Select your path as above, and choose a number of instances, or check the Fill Path box. Notice there is no spacing option, since the spacing is completely based on the size of the patterned component(s).
- For your first patterned component, select the part, then select the two Path Link features, and the Path Alignment plane. These behave exactly the same as in the above Distance Linkage method.
- If you have a second component to pattern, check the box next to Chain Group 2. Repeat the selections from Chain Group 1. Keep in mind, the green Path Link feature from Group 1 will mate to the green feature from Group 2, and red to red.
- The final pattern will be seamlessly connected, and we never had to measure any distances to get it right. The chain moves realistically when dragged, and can even drive movement in other components.