How to assign attributes to multiple components of an assembly 1

[nithinv]

Hello NX mates,

I have created an assembly with around 260 child components. Now I need to assign a number of attributes (like description, size, detail no., hardness etc) to each and every component in order to create complete BOM. Is there any easier way to assign attributes to all components at a time (using spread sheet or something like that)other than opening all components and copy/paste/assign attributes individually?

I am new to to attributes and couldn't find any helpful thread yet. Hope my question is clear. Thanks in advance.

 

[JohnRBaker]

The take maximum advantage of the way NX works you should assign the attributes to the individual part files as Part Attributes. That way they would have been automatically inherited by the Components and would be already in place for being referenced by the Parts List. With this many Components I guess it would be safe to assume that some of them are the same part having been added to the assembly multiple times. With attributes assigned to the original master part files, this then reduces the number of Components that one would have add attributes to. Besides, attributes like Material are added automatically to your part files when you assign materials to your solid models.

Also what version of NX are you running? If it's NX 8.0 or newer, you can use Attribute Templates to pre-assign placeholder attributes with values either left blank or pre-assigned so as to make the process of adding attributes to the final master part files that much more efficient and consistent. And if there are certain attributes which can be one of only a few different values, you cans set-up lists of all the valid attribute values, be they strings, numbers, integers, etc. and then all you have to do is just select from the list the desired attribute value, again something that can speed-up the process of adding attributes to your part files as well as reducing the chance that you've misspelled an attribute name or value.

Trust me, you want to set-up your work flow so that as many attribute as possible are already assigned to your master part files. Adding or changing attributes at the Assembly level should be reserved for only those cases were the attributes assigned to one or more of the Components used in that particular Assembly are different then they would be in any other Assembly. In other words, it's most efficient if you used assigning attributes to the Components of an existing Assembly for only exceptions and Assembly specific cases.

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.

 

[MFDO]

Through NX’s Progressive Die Wiz’s “Bill Of Mat.” command could bulk edit/write File Property attributes and write them back in to each respective files. This is the method I use and the easiest way I see in your situation.

Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V9.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks

 

[nithinv]

Hi John,
Thanks for the inputs. I am using NX8.0. Assume that currently I am following the procedure you described above. I have set required attributes in customer defaults, hence when ever I create a new part the attributes are added to the component under Unset category. Then I select each attributes giving value to them. Thru this I have saved little bit time that I had spent earlier in this process as earlier I was typing/copy/pate attributes to each component.

 

[nithinv]

Hi MFDO,

Thank you.

Can you please explain the procedure you use for the same? Also do you have any idea that will it work with Moldwizard BOM also?

 

[JohnRBaker]

The Attributes are set using something called Attribute Templates and doing this one of two ways. You either open your Modeling template parts and go to...

File -> Utilities -> Attribute Templates...

...and with 'Part File' option toggled ON, create the desired attributes which can either be left bland or with default values. Then save your template parts and you're good to go.

OR, you open any part file and go to the same place as above, only now select the 'Catalog' option and then create the desired template attributes.

Now set-up your desired attributes like above and when you're done, in the 'Actions' section of the dialog, save the 'Catalog'.

Then go to...

Customer Defaults -> Gateway -> User Attributes

...and define the path to these catalogs. Now when you open any part file, even existing parts, the attributes in the Catalog template will be available in as Unset attributes.

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.

 

[MFDO]

I think MW and PDW share the same command.

So try the following.
1. Insert a part list inside your main assembly
2. In the Part List add new columns
3. With column settings, designate each new column/s with the attributes you want to edit or add
4. Now click the MW/PDW’s “Bill of MAT” icon and you will see a spread sheet with all the columns and rows as your Part list.
5. In the spreadsheet double click the cells and edit/add values.
6. When you close the BOM Spread sheet, it will update the parts with new attributes.

Hope this will work for you.


Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V9.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks

 

[gani009]

THIS PROBLEM CAN BE SOLVED THRUOGH JOPURNAL. HERE IS THE SAMPLE JOURNAL THREAD PLEASE GO THRUOGH THE SAME

ADDING_ATTRIBUTES

REGARDS,
GANESH

 

[nithinv]

Hello MFDO,

That was cool!!! The time which was required to add attributes reduced a lot. It works with Moldwizard also.

Thank you so much...

 

[nithinv]

Hi John,
Yes I was following the same procedure. But the catalog option you elaborated was new to me. Thanks a lot for your reply.

However the procedure which MFDO described above is much easier than this for bulk attribute adding/editting.

 

[nithinv]

Hi Gani009,

Thanks for the reference thread. I don't know much about journals but will try using that one.

It will be great if you could teach me where to define attributes as per my requirements in this journal file. Or shall I just copy paste that one?

 

[JohnRBaker]

Perhaps, but not everyone has 'Mold Wizard' or the 'Progressive Die Wizard' module.

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.

 

[gani009]

Hi Nithin,
Please Save attached journal to you hard drive or net work drive (this journal from some where in these posts)
then go Tools -> Journal -> play. It will pop up one window there browse the journal which you save and press run. It will add attributes specified in journal.
This journal will scan all the components in assembly and add "ORDER" attribute to each component in assembly and it will ask value of order you can enter user value in the box.

If you need any specific attributes and values according to that you have to alter the journal or let me know what attributes and values you want to add in components

nOTE

GANESH KOTHAKOTA
CAD/CAM LEAD
TECHMAHINDRA

 

[MFDO]

John,
This kind of useful basic functionality should be included in the NX Base Package. What do you think?

Probably most guys don’t know what I’m talking about, because they haven’t seen it working!


Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V9.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks

 

[nithinv]

Hello Ganesh,

Thank you for the journal file and procedure to use it.

 

[PrintScaffold]

But you can bulk-add part attributes from the assembly level?..

www.cadroad.com

 

[gani009]

Hi Nithin,
That's what I mentioned in post Tools->journal->play....

GANESH KOTHAKOTA
CAD/CAM LEAD
TECHMAHINDRA

 

[MFDO]

PrintScaffold,
This is how many clicks per one attribute? Then for the whole project = #of clicks x #of attributes X # of parts ( e.g. 11 x ~4 x 260 = 11,400 clicks minimum). So you think this is an efficient way to work!

Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V9.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks

 

[PrintScaffold]

MFDO,
Yes, this is an efficient way of work. Because you missed one important point in my video - I selected multiple parts before assigning attribute. So your fancy maths amounts only for #of clicks x #of attributes = 88 clicks. I am sorry to sink yet another your NX-bashing SW-promoting expedition.

http://www.cadroad.com

 

[MFDO]

PrintScaffold,
You missed the point! I was comparing NX’s own MW/PDW method to conventional method you showed. Out of the blue you are saying I’m trying to promote SWx. Why do you hate SWx so much?

As you say, if I want to bash NX, then why did I submit 7 ERs in the last month alone? (Since John showed me how to submit ERs) It’s only to make my and other NX users’ life easier. It’s true that some ERs are based on my past experience and if they are implemented, I'm sure you will be happy and will be in a better position.


Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V9.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks