Feature Parameter Dimensions style?

[vball85jb]

thread561-272960

I have the same problem that was started in this thread. All user created dimensions are solid filled but feature parameter dimensions are open arrows, what to I need to change so they match the filled arrows automatically so we don't have to change them manually every time?

 

[JohnRBaker]

What version of NX are you running?

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.

 

[ryancook]

John,

I'm having the same problem, except not only are the feature parameter dimensions open arrow, they are also a different font than the user created dimensions. I have checked my "Annotation Preferences" and they are consistent with my user created dimensions, since having the "Use sketch dimension style" check-box un-checked should use the "Annotation Preferences" defaults, right? I am running NX 7.5, any help would be appreciated

 

[vball85jb]

We are using NX 8.5.2.3

 

[JohnRBaker]

I was not able, using NX 7.5.5.4, to reproduce the described behavior. Both the 'Feature Parameters' and user added dimensions appears to always honor what was set in Annotation Preferences.

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.

 

[lee30bmw]

I have always had the same problem as well. In Prefernces > Annotations, I have the arrows changed to "solid", but the the symbols always start as 'hollow' arrows and I have to change them manually. I am using NX 7.5.5.4

 

[lee30bmw]

And...

 

[Toost]

Could it be that the settings stored in the template part gives the open arrows but the customer defaults overrides the settings when it comes to dimensions on drawings ?

- Open the template part itself, Preferences - Annotation, check the arrow settings, then press "load defaults" - OK and save the part.
try create a new part and see how the arrows appears.

Regards,
Tomas

 

[baschuve]

We resolved this by editing the appropriate drafting standard file in “UGII/inh_files” (ansi.atp.prt in our case) then go to each drawing / dimension and Load Defaults for the Style - Line/Arrow tab. Could not use “Load All Defauts” due to the method NX uses to build the Feature Parameter dimensions with a User Defined Radial Symbol… We then set “UGII_ANNOTATION_TEMPLATE_DIR=” to a custom location with the updated inh files so users could pull this update. (Using NX7.5.5 and NX8.5.3)