NX X Centerline created in a Detail View is too long and cannot be shortened to the required length

NX for Design



When a 2D or 3D Centerline is created in a Detail View its length is derived from the original geometry selected to define the centerline, not the portion of the geometry that is visible in the Detail View. This can result in a centerline that extends well beyond the boundary of the Detail View and therefore needs to be shortened. When the Centerline is shortened, by selecting the 'Set Extension Individually' (in the 'Settings - Dimensions' section of the 2D/3D command dialog) and dragging one end of centreline, the distance the end point can be moved is limited. It cannot be shortened to less than ten percent of it original length. In some case this means that the centreline still extends significantly beyond the boundary of the detail view. This behaviour occurs in both NX 11 and NX 12.


There are several potential workarounds to this issue:

1. In NX 12.0.2, use the 'Automatic Centerline' command to add the centreline to the Detail View, rather than using the 2D or 3D Centerline commands. In NX 12.0.2, an automatic centreline is trimmed, by default, to extend just beyond the detail view boundary .

2. Use the 2D Centerline 'By Points' method, rather than the 'From Curves' option, and drag the centreline to extend it to the required length. (This workaround is only applicable if the geometry exists within the detail view to define the centerline by points. For example, using the center point (Arc Center) of the end of the hole/shaft and the center point of a chamfer.).

3. Expand the Detail view and then create the Centerline, using the following procedure:

a. Create the Detail View,

b. Select the Detail View Boundary and then select 'MB3 - Convert to Independent Detail' (an Independent Detail view is still associated to the parent view),

c. Select the Detail View Boundary again and then select 'MB3 – Expand',

d. Create the 2D or 3D Centerline in the expanded detail view. (Due to the scale of the view it may be necessary to change the Gap, Dash and Extension values of the centreline to get the required appearance):

e. Select the Detail View Boundary again and then select 'MB3 – Expand', to 'un-expand' the view

f. The centreline will be automatically trimmed to detail view boundary:

Notes and References

ER 9215727
PR 9237151
PR 9138865

Hardware/Software Configuration

Platform: all
OS: n/a
OS Version: n/a
Product: NX
Application: DRAFTING
Version: V11.0

Ref: 002-8005814

KB Article ID# PL8005814



Associated Components