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How to show and Hide dimensions displayed when selecting a feature and performing an MB3 --> "Show Dimensions" in the Part Navigator?
Solution
NX has the ability to show dimensions associated to many features by selecting that feature in the Part Navigator (PNT), and using MB3 --> Show Dimensions.
To hide feature dimensions which were made visible via MB3 --> Show Dimensions, the user needs to refresh the graphics window (MB3--> Refresh in graphics window or <F5>.
Now the question may arise that what if users want to selectively control the visibility of dimensions, since all dimensions will be hidden upon a refresh operation.
The answer is to convert those dimensions to PMI (See Requirements Note below).
To accomplish this, select any feature in the PNT and use MB3--> Show Dimensions
Select the dimensions to convert and use MB3--> Display as PMI.
The dimensions which are displayed as PMI's now will not be hidden upon a Refresh. You will now be able to hide them using MB3 --> Hide on the dimension.
Now if you want to later show these PMI dimensions, you need to expand the PMI node in PNT and select the dimension you want to show. You can either use MB3 --> Show/Hide or use the show/hide icon just beside the dimension node to show/hide them
Requirements Note:
'Display as PMI' may not be available if the following conditions are not met:
1. "Allow PMI Bidirectional" edits must be enabled.
a. Go to 'File--> Utilities--> Customer Defaults'.
b. Expand the category, 'Drafting--> General/Setup.
c. Select the 'Workflow' tab.
c. Toggle ON 'Allow PMI Bidirectional Edits'.
2. 'PMI' application must be active (turned ON) in the NX Start menu.
Also - not all dimension types are supported for the "Display as PMI" conversion. These dimensions are referred to as "cartoon" dimensions.
Notes and References
Hardware/Software Configuration
Platform: INTEL
OS: window
OS Version: 1064
Product: NX
Application: DESIGN
Version: V1847
Function: FEATURE_MODEL
Ref: 001-6903143