Visualize/Callout Only An Assembly Part Number In A BOM

[TorsionalStress]

Using CATIA V5R18;

I created an assembly “A” of parts, now I want to call out only the assembly part number “A” and not each individual part making up assembly “A” in the BOM, how can this be done?

Any response will be greatly appreciated!

 

[DaSalo]

Very good question. I have been wondering this also. What I have been doing as a workaround is:

Right click => properties => Product Tab => Uncheck "Visualize in Bill of Materials" box for all components of the subassembly except for one. In the one component that I leave visible I set all of the parameters that I want to be displayed in the BOM. So this one component is the only piece of the subassembly that will appear in the BOM but it will look like it is representing the entire subassembly. Not an ideal solution but it does work.

CATIA V5 R20
PC-DMIS 2011 MR1

 

[TorsionalStress]

DaSalo, I forgot to mention that I’m using the recapitulation table because I used a lot of reuse patterns in folders. It’s odd though, I unchecked “visualize in the BOM” for all of the sub-components in the assembly, checked “visualize in the BOM” of the assembly itself and when I click on the “bill of material” feature under “analyze” I actually see the assembly there listed but not as a part?

 

[DBezaire]

TorsionalStress,
There are a couple of ways to accomplish this but here is 1 method.

Assembly A.CATProduct
Bom A.CATpart - add the part number you want to show in the recapitulation table
Component A - in the property tab turn off visualize in BOM
Part 1.CATpart
Part 2.CATpart
Part 3.CATpart
Part 4.CATpart

The above method will allow you to have individual parts of Assembly A

Derek



Win XP64
R20/21, 3DVIA Composer 2012, ST R20
Dell T7400 16GB Ram
Quadro FX 4800 - 1.5GB

 

[TorsionalStress]

What I did was, unchecked “visualize in the BOM” for the assembly so the table now gives all of the other parts and I called out the assembly “A” part number with a note and leader in the drawing area.

 

[DaSalo]

DBezaire,
Just to make sure I understand your method: You are simply adding a dummy part to the .CATproduct that contains no geometry and is only there to contribute the correct BOM information. You turn off visualization for all of the actual parts. Correct? I like this idea better than what I have been doing. It still seems like an odd workaround.

CATIA V5 R20
PC-DMIS 2011 MR1

 

[DBezaire]

That is exactly what I am doing DaSalo. This will leave all the other parts in the correct format if somebody needs to order an individual piece of the assembly.


Win XP64
R20/21, 3DVIA Composer 2012, ST R20
Dell T7400 16GB Ram
Quadro FX 4800 - 1.5GB

 

[TorsionalStress]

“That’s nuts!” If you can insert a component being either a “part” or “product”, which both have “part number” in the properties tab, then the part number should show up in the BOM. This is why up to now, I don’t like this software.

 

[DBezaire]

Torsioanl,
I only do this because our programmers that created the interface between Catia BOM export --> internal material management program --> SAP are for the lack of a better word lazy. I would be perfectly happy not managing a NVA part.


Win XP64
R20/21, 3DVIA Composer 2012, ST R20
Dell T7400 16GB Ram
Quadro FX 4800 - 1.5GB

 

[TorsionalStress]

Not blaming you, this is a CATIA issue and they should have the software automatically place the part numbers in the BOM coming from the part & product properties tab.