The settings for Assembly and Parametric relations are in the same dialog. You can only change these settings if you have started the Advanced Assembly or Parametrics module.
To change relation settings,
1. Click File > Settings > Relation Settings. The Relation Settings and Properties dialog box opens.
2. The Sets tab includes the following settings:
◦ You can change the default settings on the left side of the screen, or the settings for just the active relation set on the right side of the screen.
◦ Create at Contents: This specifies whether or not to attach the relation set to the contents or to the instance file when the part/assembly is saved. The default is the instance file and it cannot be changed after creating the relation set. When working with shared parts/assemblies, accept the default setting. This is because relation-set behavior is different between shared parts/assemblies and non-shared parts/assemblies.
◦ Var checks: This specifies whether or not error messages are issued for check relations.
◦ Redo Blends: Specify Auto to update blends automatically. Specify None to keep blends (in this case, make sure Chk & Fix is on, otherwise the operation may corrupt your part). Select is available only for the active relation set; use this option to select the blends that will be automatically updated.
◦ Keep Tangent: Specifies whether or not to maintain smooth tangential transitions between faces when modifying relations. It operates in the same way as the Keep Tan command in Modify 3D. Tangencies with freeform surfaces are not supported.
◦ Sticky Edge: Specifies whether or not Creo Elements/Direct Modeling is to automatically create the necessary coincident relations for coincident edges (see Edge and vertex handling below).
◦ Sticky Vertex: Specifies whether or not Creo Elements/Direct Modeling is to automatically create the necessary relations for coincident vertices (see Edge and vertex handling below).
◦ Chk & Fix: Switch on to detect and fix errors in your part while solving relation sets.
3. The Solving tab includes the following settings:
◦ Update on edit: When true, the Update option is on by default in the create and modify relation dialogs.
◦ Quickview on edit: Displays a preview of your changes in the viewport while you are creating or editing a relation.
◦ Dynamic Update:
▪ for Assembly R-Sets: Part movement is animated in the viewport when the relation set is solved.
▪ for Parametrics R-Sets: Same as above, except when Parametric relations are solved.
▪ Move parts together: All parts move simultaneously to their destination points.
▪ Trans & Rot together: Rotation and translation are done simultaneously. If turned off, rotation is done first followed by translation.
▪ N Steps: The number of the steps to complete the movement. A high number of steps produces a smoother, but slower, movement.
4. The Labels tab includes the following settings:
Labels can be displayed continuously for any value type relation, such as distance or angle. Labels for all types of relations are always displayed when you modify a relation. These settings determine whether value type labels are displayed continuously and how they are displayed.
◦ Style: Here you can set whether or not an icon, name, or value is displayed in the label, and its size, font, and orientation. In the Orientation setting, View keeps the label parallel to the viewport, while World keeps the label fixed in space so it rotates with the model.
◦ Types: Set the type of labels you want displayed. M types are Measure relations.
5. The Colors tab includes the following settings:
◦ Labels: The colors of labels when each condition is true.
◦ Freedom: The colors of parts in the viewport that indicate various degrees of freedom when you use dynamic position to move parts.
◦ Browser: The colors of relations listed in the Relations and Structure Browsers.
6. The Animation tab includes the following settings:
The tabs on this screen correspond to Distance, Angle, and Number relations. The same options appear on all tabs, and can be set for the Default and the Active Relation Set. If you are working with Gear or Rack relations, use the Angle tab to set the options.
◦ Step: The step increment that you want to be added to the animated value relation at each solve.
◦ N Steps: The number of times the step increment is to be added to the relation value during animation.
◦ N Cycles: The number of times that the step sequence should be repeated.
◦ Forward: The direction of animation is to be forward, that is, the step increment is to be added to the relation value.
◦ Backward: The direction of the animation is to be backward, that is, the step increment is to be subtracted from the relation value.
◦ Retrace: When set to on, the model returns to the starting position by reversing its direction. When set to off, the starting position is reached in one single step. This is particularly useful when doing angular animation with several cycles.
7. Click Close when you are finished. Changes are applied as you change settings.
Edge and vertex handling
Select Sticky Edge and Sticky Vertex on to minimize the number of relations needed to define face transformations. Creo Elements/Direct Modeling automatically creates the necessary coincident relations and maintains these after transformation. In the illustration below, the distance relation on the right is defined with Sticky Vertex set to on. When the relation is modified, Creo Elements/Direct Modeling transforms the shape and maintains the coincident vertices. If Sticky Vertex is set to off, you would need to define coincidence relations for the vertices as shown on the left.
