Trouble creating parts list - NX6 1

[Kevin0621]

I am using NX6.
I had previously created a drawing using parts list without any problems. I have created another assembly and when I insert the generic parts list, it displays only the first row with the column labels.
What is causing the parts list from updating. There are approx 80 detail parts in the assembly.

 

[cowski]

You refer to them as "detail parts", which makes me wonder if you have added them as components or only added views from these other part files. If you have only added views, they will not show up in a parts list.

www.nxjournaling.com

 

[Kevin0621]

Sorry. The assembly is made of approx. 80 component parts and several sub-assemblies.

 

[moog2]

edit levels, and make sure "master model" and "top level only" are ticked....
If they are, turn one off and on again, it sometimes wakes up the parts list.

 

[HercalloY]

Kevin0621,

I am also finding this issue with drawings in NX4. It really is frustrating as i can't figure out why its doing it! Strangely enough... another random drawing prt file seemed to work. So i've had to do a lot of customizing again in the new file!

 

[Kevin0621]

Well, I got it to work. I had to abandon the previous drawing with all my views set up, all 14 pages and start over again with a clean sheet. I opened a single view and added the parts list without a problem. I believe there is a sort of "bit" set somewhere in the part database that I can't figure out.
However, now I'm having trouble with the Autobaloon and the hole table features.
If I select Autoballoon, select the parts list in the part navigator, select the views I need and select OK, the hour glass spins like something is happening, then after about 10 seconds, nothing....
I create a baloon callout using the Identification Symbol without a text callout and it creates the symbol. I select the symbol, then right click the parts list in the part navigator, and nothing.
I created another view of the complete assembly and removed all components except one, added a Identification Symbol, select it, right click the parts list and update it, I get the symbol to update with the correct item number.
But, If I create a view with sub-assemblies or seperate details, follow the same procedure, nothing happens.
I've tried associating the views to the parts list also. Nothing.
I've set and reset the values of UGII_UPDATE_ALL_ID_SYMBOLS_WITH_PLIST to 1 or 0. If set to zero, Autoballoon will not work on other views.

Hole table is another issue too. I tried setting the values of UGII_DRAFTING_HOLE_TABLE=1 to get the function to appear. I can select the ordinate origin, or an existing one, select the holes, which it shows how many holes I selected, then the position of the table and select create hole table, nothing happens.

Any ideas?

 

[HercalloY]

Actually yes that is what i feel was a related issue that i've also had. Where i also add item balloons and then try and update the parts list to fill in item numbers in the balloons and nothing happens... they just stay blank. Each time the only way for me to get anything to work is scrap the whole part file and try again. Which really bites because often adding balloons and/or parts list comes quite a while after you've already done a lot of work!

Hmm i wonder what the cause is.

 

[Toost]

Can you guys create a dummy structure, including partslist which doesn't work, and upload ?

similar to:

Drawing
|
Assembly
|-block
|-Cylinder

( Zip the files since this forum only allows a single attachment per post.)

Regarding the hole table, if i remember things correctly the hole table was in NX6 a "not yet fully finished project and therefore under an environment variable". - It might have a some issues.

Regards,
Tomas

 

[HercalloY]

Ok i did up a dummy set of files. I never saved the drawing after inserting the Parts List. Just inserted some views of the assy... saved the Drawing. Then tried to insert a Parts List to determine if the strange event would happen with this set of files (which it did). So then i closed out the files without saving and zipped them up.

These files are created with NX4. I also get this issue when importing assemblies (i did a few like this recently and the Parts Lists wouldn't populate). I created these using the default "File -> New" in native NX4.

I did manage to find some Palette's that come with NX4 that have Drawing's and if i use those it seems to work as expected (but also i have used them and it not populate the parts list as well so there is something weird going on i suspect, not directly related to the seedfile that gets used). It's had me stumped for quite a while.

 

[Toost]

This is difficult to respond using the correct names , the oldest NX version i have is NX6.
When you insert the views on your drawing, you must NOT use "View from part" or , as i call them, "Drawing specific components".
components with this icon , see the attached image, will not ( and should not) appear in partslists.

The intended usage of the "drawing specific component" is when you want to display something which is related to the actual assembly but which isn't on the same BOM. Example, if you design a generator for a engine and like to show some of the surrounding details, these details can be added using "view from part".

The drawing you uploaded , has the assembly and components as "drawing specific components", -see the attached image.
I don't know or understand how /why the components are as they are. ( NX4 is a few years back in my memory.)
- Did you use the "file- new - drawing" option to create the drawing ? or ?

Regards,
Tomas

 

[Toost]

this is how the icons should look.

To my knowledge, a "drawing specific component" cannot be converted to a regular component.

Regards,
Tomas

 

[Kevin0621]

Not sure where the problem is stemming from. The assembly is a modge-podge of various pieces from different formats.
The drawing border came from the final customer in NX4 format with outdated attributes. The majority of parts were converted from SolidWorks STEP-214 files. Otheres were imported as x_t parasolids then coverted from metric to inch. The majority of components that were converted from STEP contained a single "body". I then created a parametric solid that matched and then deleted the "body".
It would be nice to have a "FIX EVERYTHING" button. I broke my "PANIC" button on this job and wasted 3 days recreating things.