sketch Dimensioning

[holyghost]

Hi ,
I am unable to give dimension with extruded edge or face to newly created sketch. It works fine in nx7.5, But nx8.5 its not why? Is there any solution. please have look on jpg pic.

Thanking you

 

[JohnRBaker]

Make sure that when you're in the Sketch task that the 'Selection Scope' option is to set to either 'Within Work Part Only' instead of 'Within Active Sketch Only'.

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.

 

[holyghost]

Hi John,
Thanks for the Reply. But can you guide me where exactly that option available. I didn't find while sketching.
Thanking you

 

[holyghost]

Hi john,
I found it . it is top
thanks

 

[Dave K]

That setting likes to change on you too, so you'll have to keep an eye on it.

-D

-Dave

NX 7.5

 

[JohnRBaker]

While that may be your first impression, there's actually some logic as to how this works.

The so-called 'Selection Scope' option on the Selection Bar is controlled by Dialog Memory which retains what the last used setting was.

Now in the case of the Sketcher, these settings can be different for different types of operations. For example, while you're creating/adding curves to a Sketch you may actually like to work so that your selections are taking place 'Within Active Sketch Only' so that there are no unexpected snapping to points or curves/edges in the Work Part (or some other Component if you're working in the context of an Assembly) as you're dragging and rubber-banding geometry on the screen. However, when you go to assign Geometric Constraints or create Constraint Dimensions then you might WANT the ability to select points or curves/edges in the Work Part as well as the active Sketch so for those functions you could set the 'Selection Scope' to 'Within Work Part Only' and now that will be retained as the default for these functions while Curve creation will still return to 'Within Active Sketch Only' when you select one of the Curve functions. This way you can sort of 'fine-tune' the selection behavior using different defaults for different functions.

Anyway, give it a try and see if you can perhaps better leverage this capability to your benefit.

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.

 

[SamSlivinski]

It certainly is diffirent coming home from another program, but once I was used to it I prefer it.

Sam Slivinski
Using NX 6
Manufacturing/Aerospace

 

[RUGmechanic]

John,

I understand the philosopy of the selection scope but
is there a setting somewhere to set the selection default to "within work part" or "within active sketch"?
Every time I start sketching, the default setting is "within active sketch". I would like to change that to "within work part".
So when I start constraining to part geometry, I don't have to change the selection intent.

Thanks,

NX8.5



Older budweiser

 

[JohnRBaker]

As I explained previously, the setting is retained via Dialog Memory so that it returns to whatever your last usage was, and in the case of the Sketch functions, as again previously stated, these are a function by function basis. What this means is that if last time you created curves it was set to 'Within Work Part Only' and when you last created a Constraint it was set to 'Within Active Sketch Only' then that's what it should be the next time you're creating/editing a Sketch. If this is NOT behaving this way it's possible that Dialog Memory has been disabled one way or the other. The first place to check is to go to...

Customer Defaults -> Gateway -> User Interface -> General

...and about 1/4 of the way up from the bottom of the dialog check to see that status of the 'Save Dialog Memory between Sessions' option. If it's NOT toggled ON, do so and hit OK and restart your session. The other way in which this has been disabled is if the folder where the Dialog Memory is supposed to storing it's data is not write enabled, the data will not be saved between sessions.

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.