New Template Filters PAX 2

[MI95SHO]

Hello,

Hopefully this is a quick easy fix;
I have uploaded the company templates, created the PAX file, everything looks good, but when you go to File -> New, under the tab I have created for our templates, the default filters always are on picking "Relationship: Stand-alone Part" and "Units: Millimeters." Is there a way to change the defaults, ideally in the PAX file, to set both to All?
This is being done in NX8.5

Thanks in advance.

--
CAD Detail and Designer II
NX 7.5, 8, and 8.5 with SmarTeam Integration.
CATIA V5 R20-R22

 

[JohnRBaker]

Are we talking about Modeling templates or Drawing templates? If it's Modeling templates, generally speaking, the only option is 'Stand-alone Part'.

As for the 'Units', that's controlled by Dialog Memory. Just select what you want and the next time you open the File New dialog it will still be set to what you used the last 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.

 

[MI95SHO]

John-

I am referring to the Drawing Templates. I wondered if it was something with Dialog Memory, but each time I open NX or another file new, it returns for the drawing template menu to stand alone and metric.

--
CAD Detail and Designer II
NX 7.5, 8, and 8.5 with SmarTeam Integration.
CATIA V5 R20-R22

 

[JohnRBaker]

Then you may be having a problem with your dialog memory as it works fine or me. Make sure you've not disabled dialog memory from being saved from one session to the next in Customer Drfaults.

As for your 'stand-alone' that's not a setting but rather a characteristic of the template that you've chosen, but again, at least in my system, when I open the File New, even it's is a new NX session, it retains both the Units and whatever the last template I used, it will still be highlighted and preselected.

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.

 

[JohnRBaker]

OK, I think I see what it is that you're seeing and I think I know why, but I'm not sure that there's anything that you can do about it, and I suspect that we can't either.

It appears that NX behaves slightly different when you're using a PAX file designed for use when creating a new Modeling file versus when creating a new Drawing file. In the case of the Modeling file, there is nothing that you can do to control whether it's stand-alone of not. By definition, it will ALWAYS be 'Stand-alone' as there is no other way to create a so-called 'Reference Exsiting' type file when using a Modeling template. Now before anyone asks, "Isn't an Assembly a Modeling file which is 'Referencing' an existing file." (i.e a 'Master Model'), and while the answer is YES, we handle Assembly files in a explicit manner for several reasons, the most obvious is that it's safe to say that MOST all Assemblies will have more than ONE Component so we can't interfere with that capability in anyway, however, it's also safe to assume that when creating a Drawing which 'References' and existing file (i.e. a 'Master Model') that the vast majority of the time it will ONLY be referencing a SINGLE existing file or Component. And while we do allow you to reference multiple 'Master Models' on a Drawing we do it a very special way that does NOT confuse the software as to which FILE the Drawing is actually 'Referencing' as the assumed 'Master Model'. Therefore when you use the 'Referencing Existing', or Master Model, approach we optimize that workflow making certain assumptions which limits what can be done and so on.

Anyway, to make a long story short, it's this mechanism allowing both Master and non-Master Drawings, and the way we've chosen to trigger it, that appears to he at the heart of what you're having problems with. If the PAX file contains ONLY 'Stand-alone' entries, which by definition, Modeling files fall into this category, then NX has no problem remembering whether you had used the 'All' Units option or not and therefore it has no problem remembering exactly which template file you used the last time you had the 'File New' dialog open. And to verify this I even went so far as to creating a Drawing template PAX file which ONLY contained 'Stand-alone' entries and guess what, worked just like a Modeling template PAX file, NX remembered all the selections, even if I exit a session and restart NX.

But what that means is, if the Drawing PAX file has ANY 'Reference Existing' entries, even if they are ALL 'Reference Exsiting', then NX is not able to save BOTH the status of the 'All' Units setting and remember the explicit template that was last selected. I'm convinced that the reason for this is because in the case of the 'Stand-alone' there is nothing special that you have to add to the PAX file. In other words, by default, unless you indicate otherwise, entries are assumed to be 'Stand-alone', but if one single entry in a PAX files is flagged as 'Referencing Existing', by setting the '<UsesMasterModel>' option to 'Yes', then the system must try and resolve BOTH conditions, which Units to remember and which template to remember and its just was not designed to handle both settings. And while I'm sure something could be worked out to handle this in NX, I suspect that any request to do so would be given a very low priority since this is a rather arcane issue. However, if you would like to contact GTAC and have them open an ER, please feel free . . . just don't hold your breath.

So the bottom line is that there's nothing you can do, unless you wish to ONLY work with Drawing templates which would be used 'Stand-alone', that is, NOT in a Master Model mode. But if you needed to use the 'Reference Existing' for your work, even if you NEVER intended to use 'Stand-alone', you're going to have to live with the current behavior.

Anyway, that's what I've learned and I'm sorry that it didn't lead to where you wanted it to go.

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.