Changing Point Display from + to X 1

[Adeo]

Hi All

In NX4, can anyone tell me if it is possible to change the way points are displayed from the default + to an X that can also be plotted?

Currently I'm inserting a Target Point Utility Symbol and editing its origin to be associative to the model points.

Just wondered if there was another (more robust) way...the downside of this method being that the Target Points are "draw mode" and we've had instances of people picking them rather than the model points and creating erroneous (but fully associative!) dimensions.

Any help would be much appreciated - I've got freakin' loads of critical detail points to detail AND check on these parts ;-)

Best regards/Gruss



Adeo
Senior Designer
Aero/Industrial Gas Turbines, Aerostructures, F1, Catia V5 & NX4

 

[JohnRBaker]

Sorry, the graphical representation used for 'points' is hardcoded and cannot be altered.

That being said, I can't help but ask, what extra value is there in representing a 'point' as an x rather than as a +?

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[jerry1423]

No there really isn't a more robust way that I know of, nor can you change a point to look like an "X" - but I do have another suggestion (it may or may not be better):
You can associate the letter "X" (as text) to those points. the alignment position of the "X" should be in the missle of it (under "style"), and then associate it to the point using:
edit > annotation > origin > top right icon (point constructor) > toggle "associative" on" > in the origin location menu select "point" > select point > apply

I am on NX6, I do not remember how differnt it was in NX4

 

[jerry1423]

not "missle" but "middle"

 

[mmauldin]

I don't have NX4 to check this out on but you could try inserting a centermark with the extension length set to 0 and the angle set to 45 degrees. It works in NX6.

 

[Adeo]

Many thanks all!

@JohnR. - Apols, maybe I should have been clearer...The X ( or to be exact a 5mm high cross) is required by the customer for their in-house drafting standard for designating specific aerofoil datum points...I've contested it also, but the customer is always right, no?! ;-).

@mmaudlin - TOP MAN! This works a treat! :-D In NX4...

Insert>Symbol>Utility Symbol>Linear Centreline

Select Control Point, Set "A" to 0 and "C" to set the size of the cross.

Deselect "Inherit Angle from View" and set "Angle" to 45.

Thanks again - I'm making this one of our "Best Practices"!!



Adeo
Senior Designer
Aero/Industrial Gas Turbines, Aerostructures, F1, Catia V5 & NX4