Hi all!
Would anyone know a way to exclude a component thanks to a part family parameter?
For me not possible because the exclusion or not of a component is managed from the assembly where it is inserted and not from the part itself
Edit: I may be wrong since the 2022 version that I don't have:
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Hello @twathle
You... you used Creo before 
Otherwise, to go your way:
Component Removal Status in Configurations - 2021 - SOLIDWORKS Help
Edit: @sbadenis , I'll go back to 2013 if you ever want to test 
Hello
Good question because the automatic generation of the part family does not retrieve this parameter.
Apart from the Hotline or someone already facing the problem, I don't see where to find the solution.
In macros it looks accessible:
boolstatus = Part.Extension.SelectByID2("10NR075EG-1@0_BLOC_REEG075_F35", "COMPONENT", 0, 0, 0, False, 0, Nothing, 0)
boolstatus = Part.CompConfigProperties6(2, 0, True, True, "10NR075EG", True, False, 0)
In the 2 lines above I made the switch to the 10NR075EG component.
The first line is used to select the component and the second to change the parameters (this line should correspond to the modification of all the 'component properties' accessible via the right-click on the part. Logically it should be the last 0 (I haven't checked though).
What's weird is that some parameters are accessible in Excel as "envelope" via syntax:
$ENVELOPPE@10NR075EG<1>
There is a good chance that the parameter 'exclude from the nomenclature' will not be accessible via Excel as a result.
NB: the Solidworks help does not even talk about the configuration of this envelope property in the families of parts
@coin37coin this is used to remove or not delete a component in a part family of an assembly. The request is to exclude a part automatically when it is inserted or not depending on the family of parts.
See if my link is functional on 2022 or + for the lower versions in my opinion it's done... hence the improvement.
The link in French to the 2022 function (non-existent before):
https://help.solidworks.com/2022/french/whatsnew/c_wn2022_assemblies_config_bom.htm
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As much for me as @sbadenis, I hadn't apprehended the question in this form (the joy of interpretations ^^)
Hello @coin37coin
Yet no I don't know Creo (used once or twice 
)
Thank you @froussel for your answer, but I probably wouldn't use your solution.
I don't know the VBA at all and don't want to dive into it for the moment (lack of time)
To be clear with everyone,
The need is not to exclude a default component as soon as it is inserted into an assembly.
I'm making a set with bridles.
In some cases, the equipment 
supplier's bills will be used, they do not need to appear in the bill of materials.
In other cases, we will prefer to buy them elsewhere , we have to buy them separately so they must be in the nomenclature.
I think that my solution can be controlled on a family of parts on the other hand for parts already inserted if I understood correctly even if you change configuration, if not excluded it remains not excluded and life versa. The solution only works, if I understand correctly, when inserting it into the assembly. (To be tested)
Another solution is to create a different colored flange (for Customer supply) and everything that is of this color must be excluded by checking the box exclude from the bill of materials or envelope component of your choice (customer supply)
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I have the impression that this new feature makes it possible to exclude a part from all nomenclatures. Before, you had to exclude it assembly by assembly (quite painful to do).
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Yes @froussel but only for integration?
See the 1st link in English, not sure I understood everything well.
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I can't test (I'm under 2020) but for me the parameter should allow you to change the assembly parameter during insertion I think (it seems quite difficult to do something retroactive).
Only a test on a version higher than the 2022 will confirm this.
In any case it doesn't answer the problem of @twathle because he wants to be able to make the modification according to his assemblies (one time yes / one time no) from what I understand
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That's also what I understand @Froussel ... and so I come back with my solution/help to the Solidworks page.
It allows you to control configurations via a family table in excel and to easily include/exclude subsets via an R (resolved) or an S (deleted).
The only problem I see is that you are forced to drive for each reference and not for the whole reference (if you have 3 screws, you are forced to exclude each of the screws and not all the screws)
The option you are talking about (available since SW2022), effectively allows you to exclude a default component as soon as it is inserted.
I did the test, a part already inserted will not be excluded if you check the function after the fact ==> it's only at insertion.
@coin37coin the solution you propose will put the component in my subset in the deleted state. I simply wish that it be excluded from the nomenclature.
Unfortunately, I think the only possible solution is to do it by hand.
No solution to automate this.
On the other hand, the permlet color solution quickly identifies the customer supply of the FI
Unfortunately I don't think this is possible.
1- The order is made (if I'm not mistaken) directly from the nomenclature extracted in Excel format. If an item is there, it is bought.
2- Until now it has been desired to keep "pretty" models so that the final model looks like something.
moreover we render with VISUALIZE at the end of each project, and even if we can reapply an appearance after the fact it would represent a lot of time spent to "put the right color" when it could be the right one from the start.
There's a problem that must really escape me (and as a result, I'm the clumsy guy on duty. Sorry)
But, when you right-click on your part, component properties and exclude from the nomenclature, why don't you select "change properties in:" to "specify configurations". Which allows you to choose where you want it to be excluded from the nomenclature
So indeed it will end like this if I don't find a solution...
but I have a fairly large number of configurations (232)
Luckily they are (normally) all in a row, but in case the configs from which I have to exclude the bridles do not follow each other... I would be very annoyed.
So if you have to type them by hand, no worries but I would have hoped that a tool such as solidworks would offer a simpler solution (especially given the number of options available in a family of parts).
Hello
I confirm what @froussel said, this parameter is not accessible in the part families or in component configuration (from which the data for the part family comes from).
So apart from doing it by hand or via macro (which could be quite "simple") no short-term solution.
For the long term, we would have to make an evolution request to SW to make this parameter accessible but hey, don't expect a quick deployment (count at least 5 versions I think).
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Hi all...
After talking to support, the option doesn't seem to exist at all.
they advised me to make an improvement request on SW's website directly.
I don't know how it works for the rest but if you want to consult the subject here is the ER number: 1-25418449711
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small correction,
they must first validate the subject and then assign an SPR number to it.
And once everything is done, then interested users will be able to vote to move it to the top of the "to-do list".
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