Mate References
A Mate Reference marks the faces, edges or points of a part that it is usually mated by, and gives them a name. It is made in the part, from Reference Geometry, and saved with the part. In an assembly the mate reference shows under the component in the Model tree, its picks can be used in the Mate window, and two parts with mate references of the same name can be mated to each other in one step.
Each mate reference holds up to three picks, in order: the Primary, the Secondary and the Tertiary. Each pick says which mate it makes and which way it faces. Like a reference plane, it is a step in the History tree (Mate Reference1, Mate Reference2, and so on) that does not change the part.
How to Start It
Open the part, click Advanced on the Features tab, then Reference Geometry, then click Mate Reference.
Step by Step
- Open the part you want to mark, and click Advanced on the Features tab, then Reference Geometry.
- Click Mate Reference.
- If you like, type a Name, such as Shaft end or Base. Leave it empty and it is called Mate Reference1 (or the next free number).
- Pick the Primary entity in the view: a flat face, a round face, a straight edge, a circular edge, a corner, or a reference plane, axis or point you made. It is marked with an orange dot.
- If you like, pick a Secondary and then a Tertiary entity the same way.
- Beside each one, choose the mate type and the alignment (see below). Default and Any suit most parts.
- Press OK. The mate reference is added to the History tree and drawn as purple dots with its name.
- Save the part. An assembly reads the mate references from the saved part.
The Options
- Name: the name an assembly matches. Two parts whose mate references have the same name (capitals and extra spaces do not matter) can be mated by it. At most 40 letters, and no < or >. A part cannot have two mate references of the same name, even when one is suppressed: a name already used is refused when you make it or rename it, and an empty name takes the next free one.
- Primary, Secondary, Tertiary: the first, second and third pick. Only the Primary is needed.
- Mate type, one for each pick:
- Default: the assembly chooses from the two picks. Two flat faces or two points are made Coincident; a round face, a circular edge or an axis against another is made Concentric.
- Coincident: for a flat face or plane, a straight edge or axis, a point, or a circular edge.
- Concentric: for a round face, a circular edge, or an axis.
- Parallel: for a flat face or plane, a straight edge or axis, or a round face.
- Alignment, one for each pick:
- Any: the assembly chooses. Two flat faces made Coincident face each other; anything else takes the way that is closest to how the parts sit now.
- Aligned: the two picks point the same way.
- Anti-Aligned: the two picks point opposite ways.
What You Can Pick
- A flat face (where you click it) or a shown reference plane gives a plane.
- A round face gives its axis and its radius.
- A straight edge or a shown reference axis gives a line.
- A circular edge or an arc edge gives its center, its axis and its radius.
- A corner of the part or a shown reference point gives a point.
A face that is neither flat nor round (a spline face) is refused, and the panel says why.
Using Them in an Assembly
- Insert the parts into the assembly (or open an assembly that has them).
- In the Model tree, open a component. Its mate references are listed below its Front, Top and Right planes, each with its picks under it (Primary, Secondary, Tertiary).
- To mate by name: right-click a mate reference and choose Mate to Matching Reference. The component is mated to the nearest other component that has a mate reference with the same name: the Primary picks to each other, then the Secondary, then the Tertiary, as one step. Undo takes the whole step back.
- To use one pick in a mate of your own: open the Mate window (right-click, Mate), then click the mate reference row (its Primary pick) or one of the pick rows under it. It is picked as if you had clicked that face, edge or point in the view.
The mates made are ordinary mates. They show in the Mates folder, and you can edit, suppress, flip or delete them like any other.
Changing and Deleting
- Edit Feature (right-click the step in the part's History tree) changes the mate type and the alignment of each pick. To change what is picked, delete the mate reference and make it again.
- Rename the step in the History tree to change the name an assembly matches.
- The eye beside it shows or hides its dots. Hiding does not change the part, and a hidden mate reference still works in an assembly.
- Suppress it, or roll back above it, and assemblies do not see it.
- Delete removes it. Mates already made from it in an assembly stay as they are.
Good to Know
- A mate reference is frozen where it was made. It does not follow later changes to the faces or edges it was picked from. To move it, delete it and make it again.
- A pick more than a kilometre from the part origin is refused.
- An assembly reads the mate references when it reads the part. After you change them, save the part, then update the part in the assembly (or open the assembly again).
- Two picks that ask for different mate types (Coincident on one part, Concentric on the other), or for different alignments (Aligned on one, Anti-Aligned on the other), are left out, and the message says which. So is a pair the mates cannot join, such as a point and a round face made Parallel.
- Mating by name does not happen by itself when you drop a part into the assembly. Use Mate to Matching Reference.
- Parts read from a frozen copy or through a share link show no mate references. A subassembly row shows none of its own; the parts inside it show theirs.
- When several other components have a mate reference of the same name, the nearest one is used. Move the part near the one you want first.
Problems
- OK stays grey: the panel text says what is missing, or which mate type does not fit a pick. Choose Default for that pick, or pick something else.
- No other component has a mate reference called ...: give the other part a mate reference with exactly that name, save it, and update or insert it again.
- Mating would break other mates: a mate already in the assembly holds the part another way. Suppress or delete it, or choose other alignments, and try again.
- The parts end up back to back: set the Primary alignment to Aligned or Anti-Aligned with Edit Feature, save, and update the part. Or flip the mate in the Mates folder.