Siemens NX8.5 - own machine from library shows planars and sketches 1

[SomiRo]

Hi!

I created my own milling machine and put it in the library. So far everything works fine, but i have a problem with the display of the machine.

In contrast to the assembly in modelling module, which shows no sketches and planars (i did hide the features in the part navigator), all sketches and planars are shown when importing the machine from the library. I couldnt find the difference to the pre-installed machines, which have also all sketches hidden in the part navigator in their modelling modules, but with them, no sketches show on import from the library.
For now, I can still hide the sketches in the manufacturing, but for the later use, there shouldnt be any sketches displayed on import from the libray.

I guess I just missed one checkbox somewhere... but I am clueless so far how (or where) to solve this problem

(nx8.5.0.23, win7/x64/sp1)

thanks!
regards, somiro

 

[JohnRBaker]

You need to set the Reference Sets for all of the components in the Assembly as be 'Modeling' and not 'Entire Part'.

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.

 

[SomiRo]

ah! thats it. thanks!

(if i understood correctly, the reference set defines how much info is loaded when the assembly is opened, and with 'model' its just the solid?)

 

[kukelyk]

You should remove parameters from the parts of the machine, somehow the NX is faster with dumb bodies.
And after that You can delete sketches and other unnecessary data. I think it is better then changing reference sets..


----
kukelyk

 

[SomiRo]

well, for now its just running fine and fast.
If I notice problems, I know where to get better performance, thanks

 

[JohnRBaker]

Setting 'Load Options' to 'Partial Loading' will reduce the impact of models which have a large number of features and thus lots of parameters.

And to answer SomiRo's parenthetical question, YES, Reference Sets allows you to decide exactly what objects are to be included with a Component when it's added to an Assembly. The default behavior is for the 'Model' Reference Set to contain only the body which represents the actual piece part making up the detailed part file.

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.

 

[cowski]

The default behavior is for the 'Model' Reference Set to contain only the body which represents the actual piece part making up the detailed part file.

In my experience, the OOTB default is set to "Sheets and Solids", which will grab every sheet and solid body in the part file and add it to the Model reference set. This can be changed (to "solids priority" or "no automation") in the customer defaults: Assemblies -> Site Standards -> Reference Sets.

www.nxjournaling.com

 

[JohnRBaker]

Unless you change the setting, the assumption is that the Solid AND Sheet bodies are what makes up the 'Piece Part'. And while one might argue that 'Solids Priority' might be a statistically better default, too many people who work with a lot of sheet bodies where complaining that these were not being included in their Assemblies so we changed the OOTB default to at least get ALL users in the ballpark.

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.