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How to Create a BOM without an Assembly tree?

Experimenter
Experimenter

Hi everyone. I quickly browsed BOM posts, couldn't find anyhting on that:

 

Problem:

We are designing a product with many components in one work file. In this current stage we have many iterations, the desing changes on a weekly basis. That is why, we currently don't work with a "proper" assembly, where all components are loaded as a seperate part file. However, we still need a way of creating a BOM, which goes beyond doing verything manually in excel.

 

Approach:

Assigning properties to bodies (via "body properties" dialogue) and manually copying the columns to excel. This works, still quite some manual effort.

 

Question:

Do you have any other input? Will be much appreciated.

 

Thanks, Mattis

 

 

5 REPLIES 5

Re: How to Create a BOM without an Assembly tree?

Genius
Genius

Do you mean creating a structure without having to load any components?

In that case, just apply the non-geometric property to your parts and you will not be slowed down with any 3D representations.

 

If you are using Teamcenter or similar, you have a ton of other possibilities...

Re: How to Create a BOM without an Assembly tree?

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi Radiate,

 

Im assuming that you are creating systems of parts in a single part file. There are quite som ways to do this depending on if this is a true system engineering approach where there are interpart (component) dependancies. Depending on the requirements there would be a variation of aproaches here. Should this be more of components being designed individually but in a single part with the intention of later in the design process spearating the enteties into an assembly by creating new components either by using the standard NX behaviour while "New Componet" or Cut/Copy/Paste (depending on the dependancies) - or if WAVE links would be used I would do the following:

 

I hope it helps

 

Best Regards

Fred

 

(view in My Videos)

 

 

 

Re: How to Create a BOM without an Assembly tree?

Siemens Phenom Siemens Phenom
Siemens Phenom

@Radiate 

If I understand your question properly, you are assigning component names to the solid bodies and then you want to get a list of these components. If this is correct, then after you rename each of the solid bodies, you can turn off time stamp mode in the part navigator (right click in the background of the part navigator and turn off the check mark from 'Time Stamp Order'). This will change the display from features to individual solid bodies. You can then right click again in the background and select export to spreadsheet or export to browser. You could also select all of the solid bodies from the navigator and right click on them then select properties. In the properties dialog make sure that you are in 'bulk edit' mode. You can then right click on the background of this dialog and select export to spreadsheet or browser.

 

I hope this helps.

Regards,
Abe
Highlighted

Re: How to Create a BOM without an Assembly tree?

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

As long as the bodies & drawing are in the same file, you can assign a name to the bodies in non-timestamp view of the object navigator & add them to the parts list.

I made a video that shows this in NX1872. The theory is exactly the same for NX12, the only difference is in NX12 you use Edit Levels to select the bodies to add them to the parts list, rather than the parts list dialog.

 

(view in My Videos)

Anthony Galante
Senior Support Engineer
PhoenxPLM

Re: How to Create a BOM without an Assembly tree?

Experimenter
Experimenter

Thanks for all your support, solved the issue!

 


@PhoeNX_Support wrote:

As long as the bodies & drawing are in the same file, you can assign a name to the bodies in non-timestamp view of the object navigator & add them to the parts list.

I made a video that shows this in NX1872. The theory is exactly the same for NX12, the only difference is in NX12 you use Edit Levels to select the bodies to add them to the parts list, rather than the parts list dialog.

 

(view in My Videos)


Regarding the video, only difference in NX12: you have to edit&add levels (in this case renamed bodies) in drafting mode.

 

Regards