Add base view doesnt use DWG part as standard 1

[kscnoname]

Hello,

I`m just setting up a new working environment for our company in NX8.5.
My question/problem is that since NX8 during the creation of a base view NX takes now the master model as basis.
And then the new standard is that it doesn't even create a component in the assembly navigator (found customer default to counter that).
Until NX7.5 UG always preselected the drawing part itself which makes more sens then the master model for us.

My question is does anybody now how I can force UG NX8.5 to use the drawing part as standard for the view creation?

Thanks

 

[Toost]

Why would you like that ?
Isn't it the model that you would like to show in the drawing ?

If i understand you correct, you want NX to create components when you add views ?
If yes, then you are not using NX the way it is intended, the "drawing specific components" are for when you want to show "something completely different" on your drawing than the model itself.
Example , you are creating a drawing of the generator for a car and you would like to show say the engine top cover next to the generator, then the top cover is an "drawing specific component" but the generator is not.


Regards,
Tomas

 

[JohnRBaker]

I think what's being discussed here is from where are the 'View' definitions, which will be used to show the part in the Drawing, coming from, the Master Model's file or the Drawing's file?

Under normal circumstances I'm not sure that many people would even care or would notice the difference even if it was pointed out to them, but there is a trend toword creating more 'view-specific' items inside the Master Model, like a Sheet Metal flat-pattern layouts or the new PMI 'Lightweight Section View', which will only be accessible when creating a Drawing IF the list of views are coming from the Master Model 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.

 

[kscnoname]

Hello,

our main reason to prefer it like it was up to NX7.5 is the following:
Sometimes you need to create specific geometry ONLY for the drawing. So we usually created these in the drawing part file because we don't want drawing specifics in the 3D model.
But if we do it like NX now intends we have to either be very careful and always select the drawing part during the base view creation or create the drawing specific geometry in the 3D model (where it shouldn't really be).

So to come back to my question does anybody have an idea where I can force UG to take the drawing part for the base views and not he master model (which would be an external view).

Thanks

 

[JohnRBaker]

Are you saying that you're not able to create curves while in the Drawing? You do know that you can now sketch either on the face of the drawing itself or inside any of the views on the Drawing irrespective of where the views were inherited from.

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.

 

[PhoeNX]

@kscnoname, if you set the variable NX_MASTER_MODEL_DWNG_DEFAULT_TO_ROOT_PART with a value of 1, NX will revert back to the pre NX8 methodology. As with any variable I was always caveat by saying, it will work now but don't count on it working in later releases as it may be disabled.


Anthony Galante
Senior Support Engineer

NX5.0.6, NX6.0.5, NX7.5.5, NX8.0.0 -> NX8.0.3
NX8.5.0 -> NX8.5.3, NX9.0.0 -> NX9.0.1

 

[kscnoname]

Hello,

regarding John R. Baker post:
We sometimes need additional geometry or sketches for the creation of the drawing in more than one view.
For example a camshaft with all the lobes and then it would not be very smart to create a Sketch over and over in every view.

@ PhoeNX:

Thank you very much. This is exactly what I searched for.

 

[JohnRBaker]

If there is additional geometry that is NEEDED to properly convey how a part is manufactured or utilized, then I would say that that geometry should be included with the design model as it would seem that that is were it should have been defined in the first place and NOT on the Drawing. After all, the trend in industry today is to make the 3D geometric model the repository for ALL the 'math' needed to produce the part itself. Drawings provide the mechanism to collect only the non-geometric data and that is changing as the use of PMI increases which allows this non-geometric data to be applied directly to the 3D model thus reducing to only a single 'document', the 3D model file, ALL the information needed to manufacture and maintain the piece part itself. Changing your workflow so that these 'additional' bits of reference geometry are created in the master part file itself will just move you further along this evolutionary and inevitable paradigm shift that is taking place in the manufacturing industry today. So the sooner you start, the better.

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.

 

[kscnoname]

Unfortunately we cannot force our customers to do these evolutionary and inevitable steps.
And it also seems that Siemens recognized that they cannot force customers to switch so they created a variable to switch back to the old modus.

 

[JohnRBaker]

But as Anthony has already warned you about, if we had intended this option to be something that we planned to fully support in perpetuity, it would have been implemented as a Customer Default. By the very fact that it requires an environment variable, this tells you that it is both something that we expect to NOT be used by many people (putting it in Customer Defaults signals that this is an officially supported and legitimate option, use of an environment variable confers NO SUCH STATUS) and/or that our intention are to eventually phase-out it's use altogether and therefore using the environment variable approach is simply the next step on the 'end-of-life' transition. After all, even without the varible, there is nothing preventing users from selecting the Drawing file when inheriting views simply that it must require an explicit action on the user's part to do so. The normal out-of-the-box version of NX is set up to 'enforce', albeit mildly, those practices and workflows which are both the preferred ones and which the downstream aspects of NX has been set-up with the expectation that this is the way that the user is actually using these upstream functions.

Now it is true that one of the 'Hallmarks' of NX has always been its flexibility with providing multiple ways to do most everything that a user might wish to do, but it does NOT mean that we are obligated to make it just as EASY to use the non-preferred options as it is to use the preferred ones. Besides, changing these sorts of behaviors, like we did here, and then making it difficult to reinstatement them, is absolutely necessary if we ever hope to stop new users from picking up old and outdated habits just because the UI does not provide them with a clear and natural flow that leverages the best aspects and capabilities of the product. It's one thing to accommodate the 'muscle macros' of a legacy user, it's quite another to present, as a result of this, a less than ideal environment for a new user. I would say that many of our perceived weaknesses in our User Intface evolution over the years has been the direct result of us NOT removing/disabling old and outdated functionality and workflows fast enough or clean enough, mostly because we've always bent-over-backwards to not 'offend' any of our legacy users, even the ones that have been misusing or refusing to move-on to the more efficient and effective ways to use the software as new functions has been added and older ones have been de-emphasized/phased-out. I think you will see that we will be less concerned with this in the future as we become more aggressive and resolved to move forward quicker and in more significant ways.

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.

 

[carlharr]

Hello,

In NX7.5 with the specification set as default for views, we were also presented with the master model views (indicated with a *) in the view list - see image attached.

These seem to be gone in NX8.5, is there any way to bring these back?

We do a lot of sheet metal work, so we need to select the flat pattern from master model views.
But we also have many assemblies which contain scenery, and in these cases need to select views from the specification. The scenery MUST be shown in the specification, because it is structured elsewhere in the product BOM.

NX7.5 worked great for this, but it seems like NX8.5 isn't as good because now the engineer has to choose "drawing or model" before picking the view, which is an extra step.

Anyone know if it's possible to get the full set of views back?

http://www.jcb.com

NX 8.5 with TC 8.3

 

[JohnRBaker]

Nothing has really changed, except that starting with NX 8.0 the 'Add Base View...' dialog now defaults to preselecting the Master Model part file, where the views that you're looking for should be found. Granted, if you want to use the default view orientations as defined in the Drawing Template, you do have to take an extra step selecting the file.

The change was made because in the past the default was to preselect the Drawing template file but include the views (designated with the '*') from the Master Model part in the list. This was proving to be confusing for many people and besides, most people wanted access to the views as defined in their Master Model part file anyway and the way it was working prior to NX 8.0 gave the impression that these views were somehow secondary in importance (being relegated to the bottom of the list with some strange notation added).

And as previously implied, the use of the variable to override this behavior was intended as something which was for use during the transition only and will eventually be removed.

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.

 

[carlharr]

Thanks for the reply John.

The starred views work very well for us, as we deal with both modelled components inc. sheet metal, and assemblies containing scenery parts, so I think it's a shame they're gone.

In any case, our NX8.5 (with TC) is defaulting to the specification (drawing) file for selecting views, NOT the master model as indicated in the posts above.
I've re-set the dialogue to clear memory, and we've definitely not used a system variable.

Would you know why ours is defaulting to specification, is there some setting we've missed?
Screenshot attached shows selected specification file, and I've circled the master model which is not selected by default.

It doesn't matter which is the default for us, I'm going to have to prepare instructional guides either way as we've lost the starred views.
But I want to make sure we have the "correct" default long term so I don't have to do it again.

Thanks in advance, Carl

http://www.jcb.com

NX 8.5 with TC 8.3

 

[JohnRBaker]

The fact that you're running under Teamcenter may have an effect. I know on my system, running native Windows, the Master Model file is always what the dialog defaults to, not the Drawing 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.

 

[carlharr]

I'll re-test on Monday, thanks John.

http://www.jcb.com

NX 8.5 with TC 8.3

 

[carlharr]

Thanks John yes confirmed, my native defaults to model and my Teamcenter NX defaults to specification in the base view command.

I'll avoid mention of a "default" in the training material I think.

http://www.jcb.com

NX 8.5 with TC 8.3

 

[BOPdesigner]

So if the default/trend is now to create drawing views from the Master Model, then why doesn't my exploded view in the master model show up as exploded in my drawing file?

 

[ewh]

Maybe this will be ammunition for getting the company I work for to start using the master model method, but I doubt it. I think they'll opt for extra steps than change to master model.
As it is, we are supposed to finally be updating the software sometime next year... from 6.0 all the way to 7.5 (maybe 8.0 if we're lucky)!


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

 

[JohnRBaker]

Exploded Views are currently NOT inherited from the Master Model. For now, you'll need to create them in the Drawing file itself.

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.