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NX7.5 PARTS LISTS
2

NX7.5 PARTS LISTS

NX7.5 PARTS LISTS

(OP)
My First post of 2012 that did not take long.  We are dealing with parts list in our assembly.  How do we make it when we automatic balloon the parts in the assembly, that we do not get a circle, square or any other symbol around our item numbers?  I do not want anything but the number.  I have tried turning this to none in so many different places I must be missing something.

Next question is item#'s OR PCO(out of the box term).  How does NX come up with the Item numbers?  I need to have where I can assign each component its own item number.  Also The item number will not be the same item number among all of our projects so adding an attribute to the part that it will keep will not work.

Thanks

RE: NX7.5 PARTS LISTS

Unless you assign them manually, the system will generate the callout numbers automatically using a scheme which you have no real control over. Now this does not require messing with Attributes, simply select the individual callout fields in the Parts List note and edit the number to be whatever you wish it to be.  You will then need to 'Cut & Paste' the Rows of the Parts List to get them into the actual order that you wish.

As for having an ID callout without a 'container' sysmbol (circle, box, etc), I'm not aware of any process that would accomplish this.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: NX7.5 PARTS LISTS

If you are on NX7.5 you can set the "ballon type" to Underline instead of circle/triangle etc.
  Select the partslist, ( make sure the "partslist" is selected and not the cell/column) RMB - Style- Parts list tab - Callouts : Symbol=Underline - OK

There is a directory containing example partslists,  "install_dir"\ugii\table_files containing two ".pax files", one for Teamcenter usage and one native
 Open the correct one thru Preferences - Palettes - Open palette file...
 ( which will open a new tab "tables" in the resource bar)

Then RMB the partslist - save as template... select the directory corresponding to the paxfile above and "it will be added to the paxfile".

In the next part, you can drag drop the partslist from the "tables tab" onto the drawing, RMB - autoballon.

you can also add the same partslist to your drawing templates.

RE: NX7.5 PARTS LISTS

(OP)
Thanks for the feedback.  The circle is not that big of an issue for us. The bigger issue for us is the use of the item #s and how they get assigned.  Then We have to cut and paste to get them in the order we want.  There is no auto sort after we put in our own Item#'s and to keep our item#s.  We are very paticular on how we assign our item#'s.  It works ok for a 4 or 5 part assembly but when we have 300 parts in an assembly things get complicated quick.  I hate to say this but I-Deas let us do this.  But it had its own issues also.  Once again thanks for the feedback

RE: NX7.5 PARTS LISTS

The item number issue is something that I also hope gets improved in future releases. It works, but is rather cumbersome if you want to specify item numbers. If you are running teamcenter, I think there is a solution possible at the project level; but I don't have the details.

RE: NX7.5 PARTS LISTS

Can you again explain how you desire it to work ?
 Do you want both automatic numbers and manual in the same partslist ?
 How would you like to enter the item number ? - as an attribute on the component instance ? ( which you can have that and that don't "transfer" into other assemblies, it will be stored on the "instance" in this assy/dwg file.)

The numbering is simply set by sorting the partslist on some or multiple columns. Then it will be numbered starting with the number/letter set under RMB- Style -partslist - items - Initial callout
 Regards,
 Tomas

RE: NX7.5 PARTS LISTS

(OP)
as an attribute on the component instance ( which you can have that and that don't "transfer" into other assemblies, it will be stored on the "instance" in this assy/dwg file.)  

The Above is what I want to get accomplished.

We would like to have just manual numbers only.  But would like to have the automatic system ID balloons attached to these manually assigned item#s

Also be able to sort by this Item#.  Plus we will be skipping item numbers when Parts get deleted and or added.  

 

RE: NX7.5 PARTS LISTS

OK, what you need to do is create, at the component level, a new attibute, say with the title of 'ITEM' (you can do this by going to the Assembly Navigator, selecting the Component of interest, press MB3, select 'Properties' and then select the Attribute tab.  Now create your new 'ITEM' attribute assigning it the value that you wish it to appear in the Parts List, '1' for the first place, '2' for the second and so on.

Now select callout column of the Parts List (not the entire Parts Lists note, just the column containing the callout numbers), press MB3, select 'Style' and then select the Columns tab.  Now select the icon to the Right of the field titled 'Attribute Name' (which should be blank at the moment) and from the pop-up list of available Attribute titles you should find 'ITEM'.  Select it and hit OK.  Now hit OK again and the Parts List should update replacing the system provide numbers in the callout column with those that you had assigned to the 'ITEM' attribute.  Now to sort the Parts List, select the entire Parts List note, press MB3 and select the 'Sort...' option.  In the dialog there will be a list of Attribute titles, one of which should be 'ITEM'.  Toggle it ON, and toggle OFF any of the others which might be on (you can also move it to the top of the list if you wish, but with only one item toggled ON it doesn't really make any difference) and hit OK.  Your Parts List should now be sorted based on the numbers you manually assigned to the Components using the 'ITEM' attribute (however, you will need to be careful that there are no duplicate numbers assigned and that for multiple instances of the same Component that the same attribute was assigned to all instances).

Anyway, this should give you what you're looking for.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

RE: NX7.5 PARTS LISTS

(OP)
That works perfect this works nice.  Many steps but once I have this done it should work great. Thanks for all the feedback.   

RE: NX7.5 PARTS LISTS

And as said before, when you have set the parts list up according to Johns description, save it as a template, then those steps need not be done again. - you will "only" need to manually create the "item" attribute.
 

RE: NX7.5 PARTS LISTS

And even the 'ITEM' attribute (as a Part Attribute) could be predefined in your template part files without assigning any value or just some dummy value, since it will be automatically inherited by the Component at which point WHEN you edit it at the Component level, giving it the actual desired numerical value, it will only pretain to THAT Component and will NOT pass back to the master part file.  So then all that you have to do, once the assembly is created, but before you even create your drawing with the pre-defined Parts List note on your Drawing Template file (as suggest by Toost above), is to go into the Assembly navigator and using my recommend workflow from earlier in this thread and 'edit' in the desired numerical values for the 'ITEM' attributes which already exist on the Components.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
http://www.siemens.com/plm
UG/NX Museum:   http://www.plmworld.org/p/cm/ld/fid=209

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

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