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Creating assembly mates/constraints in SolidWorks is as easy as it sounds. Let’s add some!
Mates in an assembly do nothing but reduces degrees of freedom, and in particular inside SolidWorks, they also create mechanisms. Thanks to the capability of SolidWorks to make mechanisms ‘always on’ in graphics window. This simply means that to visualize any mechanism, you only need to click-drag a part, and rest of the parts will move according to the mates assigned.
In SolidWorks, mates (or assembly constraints) do two functions – they define relative placements of components and they create mechanisms as well. Whereas in other 3d CAD tools like (CATIA and Pro/E, to name as few), you first need to define assembly constraints/relative position of parts and then convert these constraints into joints to create mechanism as required.
Let’s see how to do so inside SolidWorks.
There are three types of mates in SolidWorks…
The post is split in three, with each containing one of the above mate type.
Standard mates, stated above, are used for positioning only, and are generally used in support to the mechanical mates. E.g., you want to create a gear mechanism, then first position the gears such that the only free degree of freedom remains is the axial rotation, and likewise.
List below shows the standard mates…
Let’s begin with the description of each, where some of them can easily be understood by their names.
Coincidence – superimposes two selected entities – point, line, plane
|Point||share co-ordinates||share infinite line||in plane|
|Line||share infinite line||share infinite line||in plane|
|Plane||in plane||in plane||share infinite plane|
Point : sketch point, line end-points & mid-points, spline control points, 3d vertices, 3d reference points
Line: sketch elements, centerlines, axis (temporary and created by feature), edges – sharp/tangent, curves, 3d curves
Plane: planner face, plane, surface
You can make the bottom face of the pin (red) touch the planner face of the link…
Parallel – makes two selected entities parallel.
Possible between lines and planes only. Requires linear/planner elements to be selected. You can use this mate to make side faces of the links parallel.
Perpendicular – well, I don’t think so further description is needed!
Aligns two lines and/or planes normal to each other. Requires linear/planner elements to be selected.
Tangent – defines surface-surface and/or curve-curve contact.
The mate is useful when you want to define sliding contact between surfaces or curves. In the example below, cylindrical face of the follower is tangent to the top face of the valve.
|Plane||Surface contact||Line contact||Point contact||Line contact|
|Cylinder||Line contact||Surface & line contact||Point contact||NA|
|Sphere||Point contact||Point contact||Surface & point contact||Point contact|
|Cone||Line contact||NA||Point contact||NA|
Concentric – makes the two selected cylindrical/conical faces share the same axis.
Well, not only faces, but you can select circular edges or sketch elements as well. In the image below, the mate makes the selected holes concentric.
Lock – locks the relative position of components.
This simply means, moving one component in any direction will also move the second one in the same direction, by the same distance. Links in the picture below moves simultaneously upon moving any one of them.
Distance – places two components at a defined distance.
In this case, the mate is applied to two faces of the link to place them at 5mm distance.
Note that you can also select points, lines and planner faces to apply this mate.
Angle – aligns two entities at an angle defined.
Select the two faces and/or lines to place them at an angle.
Note that each of the standard mate (except lock) supports alignment type – aligned and anti-aligned. Selecting any of the two options simply reverses the normal vector of the component, and so the alignment. In the image below for concentric mate, the pin can be inserted in any alignment.
Also, the software comes with a pop-up toolbar with standard mates listed, so you can simply select them as required, change alignment and even enter values, for example, for length and angle mates. You need only to select entities and it comes with the default mate type possible for the selection with a pop-up toolbar. You can turn this off by unmarking the option in the property manager for mates.