Add view changes in NX8 and 8.5

[DanKidman]

Hi all,

From NX8 onwards I've noticed that when I add a view in drafting it defaults to selecting the actual model for views rather than the drawing file. Is it possible to change this default behaviour?

 

[JohnRBaker]

This is the proper workflow when creating master model drawings.

John R. Baker, P.E.
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[DanKidman]

But that isn't what it was like in 7.5 (it defaulted to using views from the drawing) so I was just wondering why the change now and whether the default can be changed?

 

[JohnRBaker]

I'm sorry but you're going to have to provide more information since I don't understand what you're describing as "...using views from the drawing...". When you are being asked to place a view on a Drawing, the list of views being offered to you are the MODEL views. ONLY after it's on a Drawing does these views become a 'Drawing view'. Unless you're saying that you're attempting to make a Drawing of a Part file which is ALREADY a Drawing. If so, then you definitely do NOT understand how NX Drafting works.

John R. Baker, P.E.
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[jerry1423]

I think he is talking bringing in the views marked with an * compared to those without

 

[ewh]

I interpreted it as importing views from the model file as opposed to adding them from the modeling side of the draing file.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[JohnRBaker]

The change made between NX 7.5 and NX 8.0 was that when you're adding views to a Drawing, the list will NOW consist of ONLY the Modeling views of the Part file which is the 'Selected Part' as shown in the 'Part' section of the 'Add Base View' dialog. So if you wish to add a 'modeling' view from the current Drawing file you will need to explicitly select that 'Part' from the list of available files. We not longer show a single list of views from BOTH the Part being drafted AND the current Drawing file (distinguished via the '*').

In other words, nothing has changed in terms of what can be done, just the presentation and workflow scheme, with respect to the 'Add Base View' dialog, has changed.

John R. Baker, P.E.
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Product Engineering Software
Siemens PLM Software Inc.
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[DanKidman]

I appreciate nothing has changed in terms of what I can do and I know the views marked with the '*' have been changed but I was wondering why when I add a view the selected part now defaults to the model file instead of the drawing one. In previous versions it defaulted to the drawing file.

For example, if I have a part called MYPART.prt and I create a drawing the part which is selected by default is MYPART.prt, in previous versions it would have defaulted to MYPART_DWG1.prt

Thanks

 

[JohnRBaker]

It was causing confusion since only in that particular instance, that is when it was pointing to the CURRENT Drawing part, did it include the '*' labeled views. So we changed the behavior so as to only show the explicit views for the Part file ACTUALLY being referenced. And once that decision was made, it was now more logical to default to the Master Model part since that is almost always where the user will be going to select the views that he/she would wish to place on the Drawing.

John R. Baker, P.E.
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[ewh]

I must have missed that class, as I always take my views from within the drawing file. This allows someone to finesse the model concurrent with the bulk of the drafting being done by someone else.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[cowski]

I agree with ewh.

Also, if you default to the model views, won't that cause more confusion with exploded views since those must be created in the drawing file? Or has there been an enhancement regarding exploded views?

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[JohnRBaker]

It's a judgment call and depends on how people approach the pre-Drawing creation workflow. Besides, there are some applications which automatically creates views which are intended for eventual placement on a Drawing but it creates these as Modeling views, such as NX Sheet Metal where you can create 'Flat-Pattern' views. These 2D, view-dependent, wireframe 'views' can only be found in the Master Model part file. At the moment, I can think of only one situation where a view intended to be used on a Drawing MUST be created in the Drawing file and that is in the case where one wishes to place an 'Exploded-View' of an Assembly on the Drawing of that Assembly.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
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Siemens PLM:
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To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

And another issue which makes defaulting the referenced part file to the Master Model the more logical choice is when the designer has used PMI to add dimensions and/or annotations to the model. Since PMI objects can only be inherited onto a Drawing if the views placed on the Drawing are Modeling views from the Master Model part file where the PMI objects were originally created, this is just another reason to assume that it's best to make the Master Model the default referenced Part file when you go to add a Base view to your Drawing. If that's NOT what you want, it's take but a single gesture to switch the reference to another part file, in this case, the current Drawing file.

John R. Baker, P.E.
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Siemens PLM Software Inc.
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To an Engineer, the glass is twice as big as it needs to be.

 

[capnhook]

Sounds like we are rapidly approaching the day when the master model "concept" goes away, and the drawing finally resides with the model like it should have been all along? Seems most logical to me, and others....

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]

 

[JohnRBaker]

Sounds like we are rapidly approaching the day when the master model "concept" goes away,...

WHY would possibly make a statement like that? Except for the idea that as PMI becomes more extensively used that the need for formal multi-view 'drawings' may be reduced, I see NOTHING which would suggest that 'Drawings' will soon move back to residing inside the same file where the part model exists. Nothing in this thread alludes to that in any way. Even the issue of the Exploded Views is an anomaly which will be addressed some day so that it too fully supports the Master Model concept, that is that the model and any resulting Drawings will reside in different part files.

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.

 

[capnhook]

Nah, I predict PMI and GD&T will soon overrun all these stinking "cartoons" everyone has to make in order to actually tell someone else what a part looks like, and what actual features really control the fit and function. All those part annotations belong with the part. Exploded views are just an assemblies parlor trick.

So goes the "master model".

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]

 

[SDETERS]

Is the Master model approach used in other areas than just drawings? FEA, CMM programs, Cam Tool paths ECT?

 

[JohnRBaker]

By definition, every Component in an Assembly is a 'Master Model', in that the Assembly is simply of collection of pointers back to the original 'Master' part files where the Component's geometry was defined. As 'Master Model' Drawing is simply a specialized 'Assembly'.

BTW, you can also use PMI in a 'Master Model' mode in that you don't have to be in the same part file as the geometry to assign PMI dimensions and annotation including GD&T. Master Model is also supported with CAM and CAE operations. In fact, CAE enforces the Master Model approach even when used in native mode without Teamcenter being in the picture.

And while I agree that over time the expanded use of PMI, applied to the actual model geometry and/or its features, will reduce the need for, and eventually the actual creation of, traditional fully dimensioned, annotated, multi-orthographic-view based Drawings, it will be years before this is the norm and so until then, the most effective use of Drawings will still be as separate documents which reference, but does not actually contain, the part model's geometry.

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.