NX Get "The first object associativity type is invalid" while creating a dimension.

Have a drawing of a simple model with 4 holes in to dimension in drafting. Using Rapid Dimension, Method: Inferred to place the first dimension. For the first dimension the edge of the body is selected as First Object and the center of a hole as the Second Object.

For the second dimension Method is changed to Horizontal, as First Object the second extension line of the first dimension is selected and the center of the next hole is selected as Second Object.

For the third dimension Method: Horizontal is used. The first extension line of the first dimension is selected as First Object and the center of the hole down to the left is selected as Second Object. After selecting the second object NX processes the input a bit longer than normal and then the Alert: "The first object associativity type is invalid" is issued and no dimension is created.


What is going wrong when this Alert is occurs?

Solution

When creating the first dimension using Rapid Dimension command, since it picks the edge instead of a snap point as First Object and a snap point (centermark center) as Second Object, a perpendicular dimension is create. This perpendicular dimension has the edge as its first associativity object and centermark center as second associativity object.

Next when creating horizontal dimension, the horizontal dimension requires that both first and second objects are snap point type. So when creating the second dimension as horizontal dimension, it picks the second extension line of perpendicular dimension as its first object, which will inherit the perpendicular dimension's second object, (the centermark center), as its first object which is valid.

While creating the second horizontal dimension, it picks the first extension line of perpendicular dimension which will inherit the perpendicular dimension's first object which is line, and it is not valid for horizontal dimensions since horizontal dimension requires a snap point type instead of a line.
That's why a pop-up alert message occurs. Similarly, if you turn off the snap point options, when creating horizontal dimensions, it will not be able to select the edge the perpendicular dimension is associated to. 

Hardware/Software Configuration

Platform: INTL64
OS: windows
OS Version: 1064
Product: NX
Application: DRAFTING
Version: V1899
Function: DIMENSION

Ref: 002-8017557