Edit Attributes in Assembly Navigator 2

[Techomick]

Hello,

It seems that you should be able to edit attributes in the assembly navigator by just double clicking the field instead of right-clicking the part --> properties --> attributes.

Is it possible to send it to the "spreadsheet" and then save it back to NX, similiar to when you create part families?

I am using NX 7.5 and want to edit custom attributes.

Thanks,
Andrew

Design Engineer, NX 7.5

 

[JohnRBaker]

I assume that you're talking about editing the 'attributes' which appear in a Navigator user-defined 'Attribute Column', correct?

Well, that 'column' is simple a 'read-only' presentation and while the 'entries' may appear to be in 'cells' they are not equivalent to the 'cells' nor the 'columns' of a spreadsheet. And no, you can't send the contents of the navigator to a Spreadsheet, at least not with idea that if you then edit the values in the spreadsheet that they can somehow be back-loaded into the assembly to update the data. That's just not how 'navigators' inside of NX behave.

John R. Baker, P.E.
Product 'Evangelist'
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[RAGudorf]

John,
Is there any other method in NX to mass edit/update a select set of attributes acrossed mutlple parts in an assembly? Coming from Solid Edge where we had just that functionality (Property Manager) and used it routinely, I asked the NX salemens/demo jock loads of questions, this being one of them. That assembly attribute column(s) is where they pointed me to edit the attributes "in mass". Not being able to test this for myself, I believed them...

Thanks,
Ryan

--
Ryan Gudorf
CAD/CAM Supervisor
Budde Sheet Metal Works, Inc.
305 Leo St.
Dayton, Ohio, U.S.A. 45404
Tel: 937.224.0868
Fax: 937.224.1356

http://www.buddesheetmetal.com

 

[cowski]

Ryan,
Are you looking to edit component level or part level attributes?

If you want to assign/edit component attributes, you can select multiple components and edit them simultaneously. If you want to manage part level attributes from the assembly, that may be a bit trickier...

www.nxjournaling.com

 

[RAGudorf]

I think I'm talking about part level attributes as I'm not entirely sure what you mean by component attributes. One example is that we can get in the middle of a sheet metal design project and we/customer decide that the material needs to change. With Solid Edge Property Manager I could open it up in assembly environment and all the attributes in all the parts would be listed in a spread sheet type format. I could edit one of the parts material properties (it had a dropdown material list) and basically copy that (or search/replace), then paste that like excel into the dozens of files/cells that needed changed and viola, it was done. Save the assembly and all the attributes, weights, etc. were updated through all the parts. We didn't have multi-body parts or the ability, so it was all good at that point.

--
Ryan Gudorf
CAD/CAM Supervisor
Budde Sheet Metal Works, Inc.
305 Leo St.
Dayton, Ohio, U.S.A. 45404
Tel: 937.224.0868
Fax: 937.224.1356

http://www.buddesheetmetal.com

 

[JohnRBaker]

If you wish to 'drive' your attributes using Teamcenter, then this is probably possible, but without TC, you would need to write a custom NX Open application which would open, make changes and then resave a series of Part files as I know of no way to 'mass edit' the Part Attributes assigned to individual part files.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
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Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[RAGudorf]

Thanks John. We are in the process of implementing Teamcenter but without the proper training so far, I don't have a clue as to what's possible, or not concerning editing attributes.

Ryan

--
Ryan Gudorf
CAD/CAM Supervisor
Budde Sheet Metal Works, Inc.
305 Leo St.
Dayton, Ohio, U.S.A. 45404
Tel: 937.224.0868
Fax: 937.224.1356

http://www.buddesheetmetal.com

 

[Techomick]

I ended up writing an NXOpen application to do this. It is a shame NX cannot do this since our other users are not fluent in program writing.

Design Engineer, NX 7.5

 

[uwam2ie]

I often heard this requirement, in this case nx is still old fashioned and not up to date, I agree.
Hope we get it better in the next release.
regards

 

[JohnRBaker]

When you're dealing with global actions across multiple part files, this is where something like Teamcenter comes into play. Having the ability for NX itself to manage the content of multiple parts at one time, particularly something like Part Attributes, is not really the role of an 'authoring' system.

However, that being said, starting with NX 8.5 it actually IS possible that while you have an Assembly open that you can perform this task on as many or as few of the Components that you wish to make changes to (cowski was on the right track, just not with something that was doable in NX 7.5). So first select the Components of interest using the standard selection gestures for selecting/deselecting multiple items from a list, and while they are highlighted, press MB3, select the 'Properties' option and when the dialog opens in the top section labeled 'Context', select the option 'Apply to Part'. You can now either Edit any Part Attribute assigned to ALL of the selected Components in one operation, or you can also create new Part Attributes which will be assigned to again all of the selected Components. Note that once you've made all of your desired changes/additions, simply hit OK and you're done. You must remember that you will still need to actually save all of the now modified open Part files for these changes to be made permanent, and or course you will only be allow to save those files for which you have 'Write Access' to.

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]

An update: I was just going over some of the more minor (at least in terms of how much discussion there was internally) enhancements which will be in NX 9.0 and I noticed that we've made it even easier to edit a large number of Part Attributes from within the Assembly Navigator. For NX 9.0 you would still go about first selecting all or some of the Components that you wish to edit the Attributes of and you would still go to the Properties -> Attribute tab, but now there's a new 'Context' option titled 'Interaction Method' with two modes, 'Traditional', which is what we have now in NX 8.5, and 'Bulk Edit', the new method.

In the current (at least in NX 8.5) method (AKA 'Traditional'), you can still use the workflow I described above but you will need to select each relevant Attribute individually from the list and it's not always easy to tell which attribute is actually being used by more than a single Component, whereas in the 'Bulk Edit' mode, there is a completely new dialog layout which will show all of the Names/Values of all of the relevant attributes at once and will allow you to edit any or all of them without having to open, edit and accept the changes to an attribute one-at-a-time. Now you will be able to see all the Attrbute names, their values, allowing you to modify them until the full list is exactly what you want, and then you simply confirm and accept all the changes with a single 'OK' gesture or hitting 'Cancel' to undo any changes that were made which had not yet been 'Applied'.

And this will work with or without Teamcenter, except that when working in TC you will also see the relevant TC specific Attributes with access to those which are not locked by TC.

Anyway, it appears that this issue of accessing multiple parts at once for purposes of modifying Attributes has been an issue and it's now getting special attention.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
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Siemens PLM:
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[Nham]

Hello,

Interesting topic. Latest update by John especially. Is it possible to add entirely new attributes this way? This would maybe be suitable to post as a separate thread but here goes anyway.

We have thousands of standard items migrated from ideas that are stored in tc that do not have certain attributes set. Attributes like DO NOT SECTION.

We could add this to tc but this gave the idea to do it in nx. These attributes are not needed in tc at all.

So is it in theory possible to load parts from tc to nx9 and mass add a specific new attribute and it's value? Any possibility to add attributes from command line utilities?

Please suggest better approaches also.

NH

 

[JohnRBaker]

For something like that, while it is possible to do this in NX 8.5 using that first technique I described on 13 Aug, there's actually another approach that you can use starting with NX 8.0 that will basically do this automatically with very little effort on your part.

What you need to do is set up an Attribute 'Template Catalog' where you predefine the Attributes that you wish to add to EVERY file created or even simply opened in NX, even if it's a legacy part file (I just tested this on a part file that hadn't been opened in 20 years, created before we even had attributes). You create Attribute Template Catalogs by going to...

File -> Utilities -> Attribute Templates...

...and when the dialog opens select the 'Catalog' option at the top. Now you can create whatever Attribute(s) that you like, which can have predefined values or simply just a title to use as a place holder. Once you've got all the attributes defined that you would like to see added to all of your part files, go to 'Actions' section of the dialog and use the 'Export to Catalog' option to create the Template Catalog which will be an XML file. Place this file in some unique location where all of your users can get access to it. Now got to...

Customer Defaults -> Gateway -> User Attributes -> All

...and in the 'Template Catalog' section of the dialog, define the full path to the XML file using the 'Browse' function. If you've set up a Site directory, setting this Customer Default using the 'Site' level, than this will apply to all of your users.

Now when you open one of those older part files and you go to...

File -> Properties -> Attributes

...you will notice that in the 'Unset' group you will find the Attributes that you added to your Catalog. All you have to do make these attributes 'active' is to select them and hit the green check box and they will be moved from the 'Unset' to active area of the dialog (if you had set a 'Group' when you originally defined your attribute catalog they will be found in that 'Group').

Now in your case where you're looking to add the so-called 'DO NOT SECTION' attribute, this is actually one of those special attributes that requires a specific format. It's a 'string' attribute with the title 'SECTION-COMPONENT' with a value of 'no'. To help you get started, I've create for you a 'Template Catalog' with a single entry, the 'SECTION-COMPONENT' attribute predefined (it's attached file). Simply set up Customer Defaults as I've described above. Place this XML file in that folder and restart NX. Now when you open your files and go to the File -> Properties function you will see the 'SECTION-COMPONENT' attribute ready to be activated. If you do activate it (by going into the 'Unset' group, selecting it and hitting the green check mark) you will note that it's been preset to 'no' so your part will NOT be sectioned when you create section views on your Drawings. Of course, if you later on want that Component on a particular Drawing to be sectioned, all that you have to do is go into the Drawing, select the Component from Assembly Navigator, press MB3, select Properties and for either the Component or the Instance you can then set the value of the 'Section-Component' attribute to 'yes' and it will now be sectioned. Alternatively, you could also delete the Attribute from the Component/Instance and the result will be the same, the Component will now be sectioned.

Anyway, give it a shot and see what you think.

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.

 

[Nham]

Thanks John,

Works well and feels like a useful method. Anyway, Current production version is NX7.5 and have to wait to implement this with real data and NX9 when that time comes.

 

[3dr]

@ John,
I've developed an assembly template controlled by 20 or more attributes spread out over 1 top level assembly and 4 sub assemblies. Editing them has proven to be tedious. Some are buried 2, 3 or 4 levels deep.

I'm using the Attributes Tab in Component Properties to edit them.
The issues are:
1. It shows you attributes from other higher level assemblies together with the ones I'm targeting to edit. (Confusing)
2. You have to switch from "Component" to "Part" to clear it up the visual mess and gain access to the "Part" level fields you want to change. If you forget you can wind up making an entry at the wrong level, then have to go back to see what happened and fix it. (Very annoying.)
3. The dialogue is always undersized for the content and needs to be expanded all the time.


Can you recommend a solution for this? I see the NX Open thing in this thread which I don't know much about. All I need is a method that will show me "only" the attributes of the part I've selected and make them available to edit / save. Being able to set the size of the dialogue would be a big plus of course.

I've put a lot of effort into this and I'm pleased with the performance of the assembly. If I could just find a solid solution for the misery of editing.
If I can't it's probably not a very deploy-able method with any one else in the group.

TIA for any help you can offer!

Dave

 

[JohnRBaker]

If it's truly the 'Part Attributes' that you're interested in editing, then I suggest that you change the 'part-of-interest' to be the 'Displayed Part' and then you can just go to...

File -> Properties...

...where you will only have to deal with the 'Part Attributes'.

Note that the ability to even edit 'Part Attributes from the Assembly Navigator was only added starting with NX 8.0 as more of a convenience than anything else. Up until then, you could only really edit those attributes assigned at the Component level. But if you need to edit only the Part Attributes it's probably still more efficient to do so while the 'parts-of-interst' are the 'Displayed Parts', particularly if you're going to be accessing anything more than just a few 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.

 

[3dr]

Thanks John,
I'll settle for that if I need too. Just didn't envision needing to do it that way when I set out to build this intelligence.

I designed parts and sub-assemblies to be as independent and interchangeable from each other as possible. Which means the controlling attributes are spread around and feed in from different levels.

The ideal is what I proposed but I'll take another look at what I've done. Maybe it would be better to control all assembly content from one individual part file set aside for that purpose only.

Thanks again for your input!

Dave

 

[JohnRBaker]

My suggestion was not aimed at the idea that somehow you need to not have different attributes applied at different levels of an Assembly, just that you were mentioning that it was "tedious" to have to make sure that you had you setting correct when editing PART attributes while working in the context of an Assembly. I was ONLY pointing out that if you were truly ONLY concerned with editing PART attributes, particularly since you made it sound like something that you were going to be doing frequently, that it just might prove more efficient and less "tedious" to do so at the individual PART file level. That was ALL that was intended in my reply.

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.

 

[3dr]

I understood that completely John. No harm or foul and I apologize if anything I said didn't come across well. Your the only reason I've gotten this far to begin with!

Going into the individual part does take away the tedium and I've done that at times. But it also blinds the user to visually seeing the assembly adjust to the input. There is some security in witnessing that take place and it gives you a chance to notice any parts that may not comply.

That's why I'm re-thinking the path I've taken. If I go the way of a controlling part it would need to be the top level assembly.

Is it safe to say that a developed application to do strictly part level attribute editing isn't practical?? That's what I took away from your initial response.
If there is any hope in getting around it with something custom I'd like to explore it.

TIA again

Dave

 

[JohnRBaker]

This is really why we provided the OPTION to now allow a ueer to edit the Part attributes while working in the context of an assembly since in the past, while there was no problem editing a part model by making it the Work Part while the Assembly remained the Displayed Part and then editing expressions or even adding/deleting features, if the user wanted to make non-geometric changes, in this case, edit the Attributes in the Part file itself, prior to NX 8.0 he had NO choice but to make the Component not only the Work Part but also the Displayed Part in order to do so. So as I alluded to, if you need to make attributes changes to some combination of Part, Instance, Component, Reference Set, then that's why we added the options that we did thus allowing you to do so while working in the context of the Assembly, but if as I said, you were really ONLY interested in Part attributes then the older workflow of doing this while working IN the actual Part file may still prove to be a better route to go. It's all about giving you choices so that you can work however is most efficient and productive for you personally.

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.