NX 6.0 to 8.5 1

[RyanVLee]

I am moving my current company from NX 6.0 a la carte licensing to 8.5 full mach bundles. We do full machine builds so alot of sheet metal, flat patterns, machining.

Beside the huge UI shock to some of my older user are there any other pitfalls or hurdles any of you have ran across making the jump to current from way behind and out dated

Ryan Lee
Design Engineer

If you can think it it can be modeled

 

[JohnRBaker]

One thing for sure, don't depend on simply opening and resaving your legacy files, make sure that you run 'refile' on your parts before you start using them since there were big changes made to the way lightweight models were handled with Assemblies in NX 7.5 and lightweight views in Drafting with NX 8.5. Both of these issues depend heavily on you running 'refile' on all of your legacy files which you intend to continue to use in the future.

Another big 'sticker shock' is that skipping this many versions will mean that at larger number of older commands have been either obsoleted and/or completely replaced with new functions. Also some functions, while they've not gotten a big redesign, did have their names changed such as 'Hollow' became 'Shell' and 'Taper' became 'Draft'. To help you with this, there's a new function called the 'Command Finder'. This will become a 'good friend' for you users as they look for the new and/or renamed functions (for example, entering 'hollow' will return 'shell' and will show you were you can find it).

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.

 

[DLH81]

John, I have a question about running the refile utility for older parts. What are the consequences of not doing the refile if you have old NX6.0 parts and are now running a newer version such as NX8.0 (and soon NX8.5)? You say that there are changes to how lightweight models are handled in assemblies and in drafting, but what exactly happens if you open an assembly in NX8.0 and there are various NX6.0 parts in the assembly? Slower load times? Other?

Just curious because the company I am at is currently on NX8.0 and planning to roll out 8.5 later this year. They refuse, however, to do a refile, so there are many older released parts still in 6.0 and 7.5. I've long suspected that assemblies load slowly due to the fact that many parts are in 6.0 and 7.5, but haven't been able to convince the "higher-ups" that the refile is necessary. They don't want to spend the time or money to do that. I'd like some good concrete data to give them on why it is important to do a refile, so any info you have is helpful!

NX 8.0/TC8

 

[SvenBom]

One example is Drafting. When placing a view, you will have a new option in Style dialog box, in General tab. Under View configuration/Representation, there are 4 options: Exact, Smart Lightweight, Lightweight and Exact (pre NX8.5). If you do not run refile, the creation of a drawing for a large assembly will take a lot more time and Smart Lightweight will not work the same. Also, with new Smart Lightweight option, you can place Lightweight views and create better section views. Also, you can dimension those lightweight views, etc.
In short, with refile, you will do drawings faster.

 

[looslib]

If you are not running under TeamCenter, you can set up the refile utility to run in batch mode over a weekend.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

As SvenBom has stated and I had alluded to in my first post, the biggest issue is being able to leverage the work that has been done to improve performance when working with large Assembly models, first in NX 7.5 with making lightweight representations the new out-of-the-box default when creating Assemblies, to the use of this same lightweight technology for the creation of Drawings with NX 8.5. And while it is true that running 'refile' is NOT absolutely mandatory, with respect to these issues discussed here, moving to NX 7.5 is about as close as we've ever come to telling people that you REALLY need to SERIOUSLY consider doing a 'refile' NOW!!!! And just so that you understand, those of you who have already done a 'refile' when you moved to NX 7.5, and the only new parts added to your archives are ones created from scratch in NX 7.5 or NX 8.0, that when you install NX 8.5, while it's still best to run 'refile', as far as leveraging the lightweight benefits for Drawing large assemblies, you're already OK. In othere words, it was the NX 7.5 'gateway' that was critical in terms of getting the proper lightweight data updated and propagated throughout your part files and Assemblies.

Now if you don't run 'refile' and you later wish to take advantage of the lightweight views in Drafting, while the new parts (created in NX 7.5 thru NX 8.5) will work fine since the new lightweight data is automatically being created on-the-fly as you create and edit your models, if any older pre-NX 7.5 parts which have NOT been 'refiled' are included in an Assembly, when you attempt to add your Drawing views the Hidden Line results will not be correct. What will happen is that only the new parts will be properly rendered while the legacy, non-refiled parts, will be ignored.

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.

 

[RyanVLee]

John thanks for the input I have by rough estimates 500,000 .prt files that have only been even partial refiled to 6. I plan on refiling with in 6 months to a dedicated sequil server to implement manager as a getting ready point for team center. I have a time line of 45 days to be up and running 8.5 and by the end of q1 to be using NX manager to manage our cad files. Our cad data is not very organized so i want to clean it up before the refile so i get all parts.

Will it hurts us to run 8.5 for 6 months before the refile?


Ryan Lee
Design Engineer

If you can think it it can be modeled

 

[JohnRBaker]

And another issue, particularly when making this big of a jump, that is going from NX 6.0 to NX 8.5, skipping 3 full releases in between (NX 7.0, NX 7.5 and NX 8.0) that when you do open these old legacy, non-refiled Part files, that the system must actually do the schema updates on the fly, sequentiality, meaning that first the file is converted from NX 6.0 to NX 7.0. Then it's converted from NX 7.0 to NX 7.5. And then from NX 7.5 to NX 8.0, and finally from NX 8.0 to NX 8.5. And if this file is NOT saved, the next time you open it the entire process is repeated. And this is for every non-refiled part that is opened. So if you've got an assembly with hundreds of older non-refiled parts this sequence of 'serial-schema-updates' will have to take place for every part in the Assembly. But where the real problem lays is that as far as the new lightweight data is concerned, just opening a file and just performing the schema updates is not enough as the file needs to be SAVED in order for the new lightweight data to be properly formatted, therefore this is why we recommended that out customers SERIOUSLY consider doing a full 'refile' of ALL of their legacy archives when moved to NX 7.5, or either NX 8.0 or NX 8.5 if they were moving from a release older than NX 7.5.

Anyway, I hope this helps explain why this is considered to be a 'big issue' and why you will be well served if you do a full 'refile' at this time.

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.

 

[RyanVLee]

John thanks it does and i am already starting to plan a refile thanks

Ryan Lee
Design Engineer

If you can think it it can be modeled

 

[JohnRBaker]

And to make my point about the impact on Drafting, here's an albeit simply example. the image below shows two drafting views of the same model, the view on the left was created using traditional exact representations while the view on the right was created using the new lightweight representations (granted, this is simple model which doesn't gain much using lightweight versus exact representations but I'm using it just to make a point so bare with me on this):

The issue is that the Assembly has two Components, the 'valve body' and 'cover plate' which are NX 6.0 non-refiled parts while the rest of the Components in the assembly have been refiled into at least NX 7.5. This is what I mean when I said that the older non-legacy parts are 'ignored' when the Drawing views are rendered.

Note that if you do have assemblies with non-refiled components in them, when you try adding a view to a drawing the system does warn you of this fact as shown below:

And if you select the 'Details' button you'll get a report lookin something like this:

So you see, while we hope that you do perform a 'refile' we do supply tools to help you detect and correct issues which might arise if you didn't get everything covered all at once. Which I guess goes to your question about moving to NX 8.5 but delaying the refiling of the NX 6.0 archives, now that you're aware of some of the issues it's really up to you as to whether they will be show-stoppers or something that you can temporarily live with.

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.

 

[Toost]

We have refiled our database ( Teamcenter) It IS NOT a simple task... We have quite an amount less hair and the remaining hair is all grey... ( and the result is not perfect)
But, we ran simple performance tests opening large assemblies ( there is a timing figure in the NX logfile)
Then made sure all components were fully loaded and File- Save ( Since all components are version-upgraded, all components are modified, all become saved.)
Then started a new session and opened the same assembly again.
The load time noted made us take the decision to run "refile". ( UGmanager_refile_program if one runs Teamcenter.)

Regards,
Tomas

 

[moog2]

one thing you will have to do when you open sheet metal drawings in NX8, created in NX6 is that the flat patterns will need to be deleted and re-put down, they've changed the way you lay down a flat pattern, it's no longer seen as a view in the drawing file, but rather a "view from part"
your old drawings will not honour the <W@$SH_MASTER_PART_NAME> unless you delete the flat pattern as re-do it