Question about the 500 Meter Limit on NX .PRT Files - Limit only for Components, or Assemblies to?

[MASawtell]

This is a question that is bubbling up pretty fast on a project that I am working on, and a definite answer is needed:

NX .prt files have a "1 Km Limit" which for all practical purposes equals to a 500 meter limit on the Positive X, Y, and Z Axis. Is that limit only for designing physical components (like say a tunnel), or does it also apply to a virtual assembly that could be Km in length, width, and depth?

It would be a bonus if anyone can point to me where at Siemens websites the definite answer is published. Thanks in advance for the answers

 

[JohnRBaker]

I doubt this is can be found on any public website. There might be a comprehensive discussion of this in the documentation included with the Parasolid toolkits, which is not included with NX but rather would have to be acquired separably when you license these toolkits.

As for your initial question, this is primarily an issue with respect to the Solid and Surface modeling data of the Master Part models and not necessarily Assemblies, although there are some considerations there as well. Note that in the case of Assemblies, generally the first issue that one encounters is how the Assembly is displayed. Note that there are some things that can be done to mitigate those issues but it only impacts how geometry is displayed not how accurate or precise that geometric data is being represented or manipulated.

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.

 

[MASawtell]

Thanks John on the answer for assemblies - takes care of a couple of questions I have gotten from the local peanut gallery.

 

[MASawtell]

Now a quick follow up about migrated data from IDEAS via CMM - where an item is over 500 Meters in size (like a tunnel) - does there need to be a manipulation to the defaults in NX to make said item "pickable" in an assembly or drawing of either the object or the assembly it is located in?

 

[JohnRBaker]

I have no experience with situations like that. Your best bet would be to contact GTAC as they should be able to help you with some of these issues.

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.

 

[MASawtell]

John, for future reference - here is a solution that was relayed to me via another channel (who apparently asked this question to GTAC already):

Variable to add to or edit in UGII Environment Variables: UGII_MAX_FIT_BOX_SIZE

Increase the Variable to be able to pick what you need in your assemblies and/or drawings.

 

[JohnRBaker]

Yes, this will help to resolve some of the display and selection issues encountered when dealing with Models that exceed the recommended working space. Please note however that this in no way changes the accuracy or precision of the models being created, it merely 're-calibrates' the presentation and graphical aspects of working with Models and Assemblies this large.

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.

 

[MASawtell]

Given the historical aspect of some of these elements, or the fact they are not under "direct control" of the client per se, that is something I can live with.

 

[Arkance/PhoeNX]

You don't have to set that variable anymore, there is a customer default (can't remember what version it appeared in).
File -> Utilities -> Customer Defaults -> Gateway -> Visualization -> View/Screen -> Maximum Size for an Objects Bounding Box.

Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[JohnRBaker]

Yea, I forgot that we added this option to Customer Defaults, which has been there since at least NX 5.0.

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.