BOM reference issue

[xchrisgrassx]

Good morning everyone, simple question here. I was hoping someone might be able to inform me as to how I go about removing a part from the bill of materials. I have a few conceptual/visual aid components that I do not want in the BOM.

I checked the iproperties for some sort of reference only option, but came up with nothing.

Thanks in advance,

Christopher

Note - Not using vault

[coreyparks]

Open the assembly and edit the BOM from the assemble tab.  In the column called BOM structure change the part to Phantom.  Phantom parts show as normal parts in all drawing views but they do not show up in the BOM.  However if one of them is an assembly then the assembly won't show but all of the children of that assembly will.

[mcgyvr]

umm phantom is technically not correct. you should set it to reference. Its quickest to just right click on a part or sub in the model browser and select "bom structure..reference"

Phantom should ONLY be used for subassemblies that are built on the fly (ie non-stocking subassemblies) and like corey said the components of that sub are exposed at that upper level instead of being shown in the subs parts list.

[coreyparks]

Incorrect, reference parts do not disply correctly in the drawing then.  They show as phantom lines or solid lines but never shaded.  It all depends on how you want the drawing to look in the end.  I admit I usually don't use phantom parts like this but I assumed he wanted the parts to look "normal" while not showing in the BOM.  I normally use phantom assemblies to make subs that help me build my design but have no relevance to the BOM.

[mcgyvr]

Not incorrect..no mention of needing a shaded display in the drawing was in the original question. Reference is the proper setting to answer the original question as stated.

Your phantom suggestion is technically not the correct method but does function as a good workaround to avoid the inability (bug in Inventor) for reference parts to show as shaded in an IDW. But if his components are iam files then it doesn't work.

"Phantom" setting was actually taken from early ERP systems (before Inventor was even out) and was used to indicate a non-stocking sub-assembly in which during job order/work order release the components were extracted from the phantom subs and moved into the pick list for the upper level assemblies.

"Reference" setting allows parts that should not show up in the BOM nor on the parts list in an IDW but are used as "reference" geometry in the modeling process.

[coreyparks · Accepted solution]

     I agree Reference would be the way to go if it worked well, I have found very few times when it does however as I usually still want the parts to show the same as the rest.  I usually make all reference parts on color and state that on my prints.  ALL PARTS SHOWN IN RED ARE FOR REFERENCE ONLY.  I took the statement of "I have a few conceptual/visual aid components that I do not want in the BOM." to mean he was ok with how they were currently being displayed and wanted them to be removed from the BOM.  Phantom accomplishes this.  But you are right that if Reference worked better it would be the more correct method.  This is also why I stated the warning about assemblies.  Also sorry if I came across as an ****, it was not my intent, just a bit of a rough day today and I seem to be talking/typing before I really think about what I am saying, lol.

[xchrisgrassx]

Thanks for the help both of you, I will play around with both methods and do a little further digging.

[nadinbu]

Hello,

is it some way to change reference line type to gray and thin?

thank you