Datums in assembly not adjusting after component geometry gets updated??

[BurgerMechE]

I'm using NX 8.5 with TC. I've made datums in an assembly off of component geometry. I update the component geometry and the datums are not updating to the locations where the adjusted component geometry now resides. The datums are associative but I can't figure if there is additional setting or check box I need to click. Any help would be greatly appreciated.

Thanks!

NX 8.5, windows 7

 

[cowski]

Since you are referencing component geometry, there must be a wave link somewhere. Make sure the wave link isn't broken. You might need to turn on "load interpart data" in your assembly load options and/or fully load any parts involved in the wave link. Otherwise, the link may not update until the master geometry is loaded.

www.nxjournaling.com

 

[BurgerMechE]

Thanks, it appears my organization only has so many Wave control licenses and I can't do it right now. Quite frustrating as this is a standard feature for almost all other main stream CAD packages.

NX 8.5, windows 7

 

[JohnRBaker]

You do NOT need a so-called 'WAVE Control' license to create WAVE links. All you need is an Assembly license.

Since you mention Datum Planes, when creating Datum Planes in the context of an Assembly make sure that the 'Create Interpart Link' option is toggled ON which will allow WAVE links to be created automatically, as shown below:

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

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

 

[cowski]

You don't need a wave control license to create and maintain links. The wave control license adds some additional functionality, but you should be able to track down your problem without it.

www.nxjournaling.com

 

[JohnRBaker]

Note that you can also simply toggle ON the 'Associative' option in the Datum Plane dialog when you're working the context of an Assembly when creating Datum Planes by referencing the edges and faces of various Components in the Assembly.

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

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

 

[BurgerMechE]

Thanks for the help. To get it to do what I wanted I needed to use Wavelink Geometry Linker as recommended. I didn't need the load interpart data function. Thanks again

NX 8.5, windows 7