Chapter 13: Getting More from Mates
Analyzing degree-of-freedom
When working with motion in SolidWorks, you need to be comfortable with the concept of
degrees of freedom. When inserted into an assembly, each model begins with six degrees of freedom:l Translation in X (tX)l (^) Translation in Y (tY)
l Translation in Z (tZ)
l (^) Rotation about X (rX)
l Rotation about Y (rY)
l (^) Rotation about Z (rZ)
When applying mates, and especially when troubleshooting motion or overdefinition problems, it
is important to look at how each mate translates into degrees of freedom being tied down. For
example, a Coincident mate, planar face to planar face, ties down one translation degree of freedom
(in the direction perpendicular to the faces) and two rotational degrees of freedom (about directions
which lie in the plane of the faces). What remains are two translational degrees of freedom in the
plane of the faces and one rotational degree of freedom about an axis perpendicular to the planar
faces.
A point-to-point Coincident mate ties down three translational degrees of freedom, and the part
can only rotate.
An edge-to-edge Coincident mate ties down two translational and two rotational degrees of freedom.
As a result, a part that you mate in this way can only slide along the mated edge and rotate around
the mated edge.
Tip
When using face-to-face Coincident mates, it takes three mates to fully define a block type part. When using
edge-to-edge Coincident mates, it only takes two mates.
Something to be careful about is that a degree-of-freedom analysis frequently predicts an over-defined
mate scenario when SolidWorks does not in fact display any errors or warnings. For example, if
one block is mated to another with the simple case of three face-to-face Coincident mates, and
each Coincident mate ties down one translational and two rotational degrees of freedom, then the
mating scenario ties down 9 degrees of freedom, so the part is overconstrained by three rotational
degrees of freedom. However, SolidWorks has a lot of forgiveness built in, so it frequently
allows situations like this, where parts are severely overconstrained. When troubleshooting any
overconstrained situation, you should not take this forgiveness for granted. If SolidWorks reports
an assembly as overconstrained and the reason is not intuitively obvious, try reducing some of the
degrees of freedom constrained. For example, instead of making two faces coincident, consider
making them simply parallel, or mate a point to a face instead of two faces.