is this a good practice to use boundary option in drawing

[godpaul]

suppose i have a long rod, but i am only interested in the sharp tip , so i use boundary option to hide the remaining body of the rod
i know that detail view can give similar result, but since i want to have the base view and projected view aligned together, that's why i use boundary option to hide the remaining body.

is this a good practice? any alternative?

thanks

picture

http://files.engineering.com/getfil...-2360-4b15-8254-faa994092fa4&file=Capture.PNG

 

[JohnRBaker]

If you only wish to see one end of a long item on your drawing, you should be creating a single-sided 'Broken View'. If you're using NX 8.0 or newer, this is relatively easy to do. Just place a normal view on your drawing, even if it runs off the side of the sheet. Then select that view, press MB3 and select the 'Add View Break' option. When the dialog comes up, set the Type to 'Single-Sided' and proceed with the steps outlined in the dialog. If you need more help understanding what to do, press the 'F1' key while the dialog is open to get the specific Help pages for this function.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[godpaul]

thank you John,

what will be the benefit when using View Bondary option on drawing? under what situation i should use?

 

[JohnRBaker]

Generally speaking, there is very little need to ever manually change the boundaries of a Drawing view. This functionality is really left over from the days when we didn't have as good a set of View creation/editing tools as we do today. In your case, the recommended approach is to use 'View Breaks' and NOT by messing with manually changing the boundaries of a view .

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Xwheelguy]

Unless you require 2 breaks at different angles....new breaks don't work so well with differing angles. Still doing it the old manual way here, as it's the only way that works AND allows for a clean looking break on the dwg.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JohnRBaker]

Tim, can you post an image showing a typical yet problematic multi-angle broken-view situation?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Xwheelguy]

This is NOT a 90° section of tubing - I can insert a single break at one end, but I cannot break both ends to enlarge or detail the bend area. The old View Break allowed me to draw the lines defining the view boundary as the breaks were put into place. Now, I can only put in a single break.

The easiest fix....errrr.....ENHANCEMENT (in my opinion) would be to add a dropdown listbox to add additional breaks, similar to that of the Variable Radius points, Leader Terminating Objects, etc.

VIEW_BREAK_PIPES_EXAMPLE.png

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JohnRBaker]

The best that I could do was to create TWO separate single 'Single-Sided' broken views, edit out the redundant curves from each one and then superimpose one view over the top of the other giving the illusion that it was a single, properly broken view, as seen below:

Note that I've brought this to the attention of the Drafting Product Managers and have asked them whether there are any plans to allows a second 'Single-Sided' break to be added to a view, which can be set to an arbitrary angle, as you can do with the first 'Single-Sided' broken view, and not limit this view to only a Perpendicular or Parallel orientation relative to the first 'Single-Sided' break.

May I suggest that you contact GTAC and have them open an IR/PR asking for this enhancement, which would help give credence to my request that there is a need for something like this in NX.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.