Custom attribute in parts list 2

[cowski]

I have a component attribute that I would like to add to the parts list. Here is the procedure I follow:
[ol][li]place parts list[/li]
[li]add column[/li]
[li]edit text of cell, choose 'relationships', insert object attribute, choose desired attribute[/li]
[/ol]

This works in NX 7.5 but fails in NX 8, 8.5, and 9 with the error message: "Invalid annotation specified in entry field". The invalid entry, which NX has provided, is "<W@attTitle>".

Is there a new way to do this, or should I take it up with GTAC?

 

[JohnRBaker]

If this is a true 'Parts List' object, after adding the column, you select the column (not the cells but the column itself), press MB3 and select 'Style' and then select the 'Columns' tab and set the Column Type to 'General' and then either enter or select the Attribute name from the list, if it's a 'Key Field' toggle that ON and then hit OK. Now that attribute must be assigned to the Components or the values will not be inserted into the column. If you press the 'F1' key while you're in 'Style' dialog you'll get the help file which covers how to properly create a Parts List column and what the various options and settings control.

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.

 

[cowski]

Thanks John!

It has been well over a year since I last dealt with part lists, I'm going to claim brain fade on this one.

www.nxjournaling.com

 

[bafio]

I hope not to go OT but I looking for compiling NX9 drafting parts list with parts attributes.
Could anyone drive my step by step on how to do?

We work mainly with square and rectangular metal pipes and plain metal of various thickness. Often also a really simple folded sheet metal but I think this problem can be managed later.
1st step I've done was to open our seed (template) parts of pipe and insert 3 expressions. Length=X Width=X Thickness=X. Same think done for plain metal and folded Sheet metal
Now I expect that in NX9 some wizard drive me through the process to convert part expression to a row in assembly parts list. For expample in column "Description" I need to read something like "TUBE L=; W=; T=;" or "PLAIN SHEET METAL L=; W=; T=;"

At this moment not found not wizard nor helfull documentation or tutorial
On youtube I can easily lear How to do it on SolidWorks, Inventor and Solid Edge but seem NX is not so widely common


Regards

 

[Arkance/PhoeNX]

The video attached should get you on your way.


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 -> NX9.0.2, NX10 Beta

 

[bafio]

Follow your video is an impressive step over any of my idea.

Job done.

Is there a reason you not suggest me to format the string to:
LAM. L=<X.2@LENGTH> W=<X.2@WIDTH> T=<X.2@THICKNESS>
so to have exactly what I need? Maybe some bug or a new features in next realeses?

Just curious, from what version of NX (or UG) is available that feature?

Regards
Fabio

 

[Arkance/PhoeNX]

Nothing wrong with your suggestion at all. I just didn't think of it.


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 -> NX9.0.2, NX10 Beta

 

[bafio]

Another hint I looking for to automate the parts list creation is about the "Code" column. You can see it in the last page of the file attached to previous post.
Very often this information is taken from a portion of the filename without extension.
a) the portion to take is not fixed
b) sometime this information not fit at all with filename

To edit the information in this column we have a very expensive (non Siemens) piece of software that:
1) open an Excel sheet
2) read somethink from every component of assembly and this way compile the Excel sheet (see attached)
column A is for on/off visibility in parts list (click on button to on/off)
column B is the filename of the component
column C is for the code to see in parts list (TO ACHIEVE)
column D is for description (ACHIEVED)
other column not help now
3) permit a really fast copy/past from column B to column C and eventually correct the information in it.
4) hitting "Export to UG" Excel exit and the Parts List is completed. (With many sub assemblies this system is not correctly reports quantities)

We would like to dismiss this system in favor of entirely Siemens software.
We think that this expensive system (from NX2) causes random slowness problems when modeling some part/component.

I understood that starting from NX9 was adopted a faster system for simultaneous editing of attributes. I hope this (or any other way) can help us.
Help me please
Bye bye

 

[cowski]

Another hint I looking for to automate the parts list creation is about the "Code" column. You can see it in the last page of the file attached to previous post.
Very often this information is taken from a portion of the filename without extension.
a) the portion to take is not fixed
b) sometime this information not fit at all with filename

There were a few threads recently about using the expression system to retrieve the file name and split it up into pieces, they may be of interest to you.
thread561-360636
thread561-351996

If the expression system isn't flexible enough for what you need, perhaps a journal would do the job.

www.nxjournaling.com

 

[bafio]

Just to continue in this thread...
1 which version was first implemented for the =<X.2@xxxxx> functions?
2 Do I misunderstood the new features about fast attributes editing? (maybe "Edit attributes in bulk"?)
3 In past I try to do something for NX with VB2012 Express but found that need a license to compile or to run. Am I wrong?
4 Is there in NX some programming language that doesn't need license for compile neither run? For example we have license to run GRIP code but we haven't to recompile the code to our NX version
5 in the link you suggest, people talk (and you too) about "expression system". Where to start to find documentation about?
6 alternatively I'm looking to give to any member/part/component a "part name" and inherit that name instead of filename that need to be worked on.

Any way I'm following the suggested link so to learn something more

Thank you
I also appreciate

http://www.nxjournaling.com

 

[cowski]

[ol][li]The text formatting functions (e.g. <X.2@xxxx>) has been around for a very long time in UG/NX.[/li]
[li]There has been some work on the way attributes are handled/assigned in recent versions (the biggest change happened in NX 8), but I'm not aware of any new features known as 'fast editing' or 'bulk editing'.[/li]
[li]You can write code and run it as a journal, this doesn't require any special license. If you have an 'author' license, you can compile the code which confers some advantages.[/li]
[li]Using journals, you can write code in many popular languages (C++, Java, .NET {VB, C#, any .net compliant language}, etc).[/li]
[li]For more information on the expression system, look in the NX help file (search on 'expression'); I think the main information can be found in the "CAD modeling" section.[/li]
[li]Any attributes you assign at the part level will be inherited as component attributes when you use the part in an assembly. These component attributes can be 'overridden' if necessary without changing the underlying part attribute.[/li][/ol]

www.nxjournaling.com