Hiding Datums and Model Sketches in Drafting (NX 8.5) 1

[Tangentor]

Hi,

This seems like an incredibly basic question, and I've found some forum answers which partially answer my question, but I'm still having difficulties with this.

This is my first time using NX to create drawings. I have a ~150 part assembly, and am just attempting to put together some basic drawings of it and selected sub-assemblies at this stage. I have been using layers during modeling to selectively hide sketches, datums, points, curves, etc. However, when I try to create drawings of these models, everything shows back up again. I get datums showing up all over the drawings for each individual sub-part, sketches showing through everything else, etc. I have successfully used Edit > Show and Hide in some cases, and checking off View Style > Hidden Lines > Edges Hidden by Edges has sometimes worked for sketches, but not always. In the most recent drawing I attempted to create, datums don't even show up in the Show and Hide list. Layers don't appear to carry over at all in terms of providing the ability to selectively hide items in drawings. How am I supposed to do this?

I've also been repeatedly frustrated by layers being inconsistent between sub-assemblies during modeling. Although I have added all sketches/curves/datums to layers when creating the part (beginning at the main assembly with the Create New Component command to create a sub-assembly) all of these options are lost when I again make the parent the displayed part. If I want to hide them, I have to re-select each part individually and re-assign each piece of the model history to layers.

There has to be a better way of doing this. What am I missing here? I started using layers after they were presented by a Siemens teaching rep, and also in the tutorials packaged with the software. Is there any point in using layers, or are they just an antiquated/redundant/useless feature?

Thanks for any help.

 

[JohnRBaker]

Well if you work in the Master Model mode, where the parts that you're Drawing are actually Components of a 'Drawing Assembly' then you can use tools like 'Reference Sets' to prevent unwanted geometric data, like skecthes and datums, from even showing up in your Drawings in the first place. If used as recommend, there is virtually NOTHING that you have to do to accomplish what it is that you're attempting to do with layers and hide/show actions.

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.

 

[Tangentor]

So I should be using reference sets instead of layers? Is there some reason to have both functionalities? Is it a newer feature or something?

 

[JohnRBaker]

Reference Sets and Layers are very different and they each have their uses. However, in the context of any sort of Assembly, be it just a modeling assembly or one that will be used to create a Master Model Drawing, Reference Sets are the best mechanism for 'segegating' the geometric data that you wish to see when wroking on the Assembly versus what you need to see when looking at just the part model itself. Think of a Reference Set as a sort of 'filter' that you can apply when a part is added as a Component to an Assembly. If you don't want or need to see things like sketches, reference curves, trimming surfaces, datums, reference points, etc, simply make sure that you always use the 'Model' Reference Set when adding a Component to an Assembly since, unless you've done something yourself, NONE of these object types, by design, will be included in the 'Model' Reference Set. Generally, speaking if left untouched, the 'Model' Reference Set will ONLY contain the Solid bodies in your part file, unless there were ONLY sheet bodies (surfaces) and then they will be included. Therefore, when you add a Component using the default 'Model' Reference Set, you will see ONLY the Solid (or Sheet) Bodies. And this is done without having to ever mess with layers or Hide/Show while working back in the piece part model file. In other words, even if they are visible while looking at the piece part model file, if those items have NOT been manually added to the 'Model' Reference Set, they will automatically be unseen when looking at the Assembly. Not only will they be 'unseen. but if you have the 'Partial Loading' option toggled ON in your Assembly Load Options, NONE of that data (along with some other stuff) will even be loaded into memory when the Assembly is opened, thus improving the speed of loading and the performance while working in the Assembly. Where as, if you DO load all that extra stuff into the Assembly and then use Layers or Hide/Show to manage their 'visibility', that data will still have to be loaded every time that Assembly is opened during your NX session.

As for layers, while they can of course be used in an Assembly, their real value is when you need to 'segregate' the various geometric objects in your piece part files, although many people have found that using Hide/Show along with such tools as the 'Hide and Show' function where you can toggle ON/OFF entire classes of objects or using the explicit 'Hide' and 'Show' functions to control the visibility of individual objects, is almost all they need to manage the 'clutter' and to organize their model, albeit into a 'binary' world where eitehr you see something or you don't (an 'Occam's razor' sort of approach).

Anyway, I hope this helps you sort our what your options are and how you might best leverage the tools that you have in NX.

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.

 

[Tangentor]

Thanks for the response. I appreciate it.

It sounds as if Reference Sets perform the function that I was attempting using layers. I'll take some time to go through whatever tutorials there are in NX Cast related to reference sets, so that I don't completely mess up my project while trying to understand/use them. I'll also start making use of Partial Loading, as I think that this is probably slowing things down considerably for me, but I wasn't previously 100% clear on what it did (ie. how it defines what "partial" means).

Does Siemens (or anyone else) provide a recommended set of "Best Practices" anywhere for this sort of thing? I'm familiar with the Master Model concept, but the software doesn't constrain you to follow this approach in any way, so a set of rules/guidelines to follow would be very helpful to avoid unwittingly shooting myself in the foot. I would also like to know how best to manage linked expressions within my assemblies, WAVE relations, etc. I know from programming experience that mis-managing these sorts of things can lead to all sorts of headaches, but haven't been able to find a comprehensive guide on how to best organize these relationships in large assemblies. I find the NX help files almost completely useless/unusable. It took me 20-30 minutes to get the Java search applet working earlier today, and even then my searches return empty results.

 

[JohnRBaker]

I'm not all that familiar with the training material available either from Siemens PLM or any of our parteners, so I can't really comment on that.

However, the good news is that, at least with respect to Reference Sets, if you do NOTHING but just leave things as they are out-of-the-box and stick to using the 'Model' Reference Set when building your Assemblies, again the default behavior, they almost take care of themselves.

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.