ID Symbol read file name?

[jkcone]

Hello
I'm trying configure ID Symbols to display the last three digits of it's associated part file's name when their created in NX5 drafting using Auto Balloon & a selected Parts List.
Does anyone have any suggestions?

Thanks in advance.
James

 

[JohnRBaker]

You already have a thread covering this topic. Why are you starting another one only a couple of days later?

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[jkcone]

I didn't know why I hadn't receive any input.
I don't mean to sound impatient.
I though maybe I was asking the question in the wrong way or something?
I know you guys have a lot to keep up with here.

James

 

[JohnRBaker]

The only solution at the moment would be to write some custom code, using either NX Open or KF (Knowledge Fusion).

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[jkcone]

Is there a way for the ID Symbol to read & display the entire file name, not just the last three digits?

 

[JohnRBaker]

Yes there is.

Once you've created your assembly and you have both the ID symbols and the Parts List displayed, select the Parts List object and then press MB3 and select the 'Style' option. Now on the 'Parts List' tab you can change the 'Main Symbol Text' from 'Callout' to 'Part Name'. You will probably also want to change the Symbol type from a 'Circle' to a 'Rounded Box'. And then after you hit OK, you will probably notice that the 'Rounded Box' is not large enough so you will need to edit them by selecting them (you can select them all using a Filter and doing a Select All), press MB3 and select the 'Style' option and change the size of the ID symbol.

Of course, if this is going to be your standard, you could update your drafting templates with an included Parts List with these changes already incorporated and with the default ID Symbol changed to a 'Rounded Box' of sufficient size to accommodate you typical file name length.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[uwam2ie]

1.have you ever taken a look at tubular notes
no Id Symbol but is doing the job
2.a trick is to move the partname in the first partslist column and then do autoballon

 

[jkcone]

Thanks John, that sounds like what I'm looking for. I'll try that right away.

Thanks UWAM2IE, tubular notes is completely new to me. I'm always looking for tips & tricks. I'll give it a try.

Any suggestions on how to keep assembly components from being displayed in the parts list? Like screws, dowels & such.

Thanks,
James

 

[JohnRBaker]

Yes, you can select any component in the assembly and add an attribute titled 'PLIST_IGNORE_MEMBER' and that component will be ignored. Note that the value of the Attribute is irrelevant just that an Attribute by that name is there. Now if these are items which you will ALWAYS wish to be ignored by the parts list, go back to the master file and add this Part Attribute and then it will be taken care of automatically. In fact, what I do is I've added this a default Attribute to my modeling template files, just that I spelled the name 'PLIST_IGNORE_MEMBER-X' and then wrote a note for the value reminding me to edit the name. That way, I don't to stop and look-up the name of the Attribute all of the time, I can just edit the Part Properties changing the name of the Attribute by removing the '-X' and then I'm good to go.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[jkcone]

Thanks John. That's a BIG help & a GOOD idea!

James