Is there a way without deleting the part from the assembly to make said part not show up in the drawing? I need to be able to do this in the model and not in the drawing. Suppressing the part create a level of detail, but I would have to create new views in the drawing and I don't want to do that.
The part is used in some cases, but not in others so I don't want to delete it from the assembly.
Thanks in advance!
Solved! Go to Solution.
Solved by karthur1. Go to Solution.
You can turn off visibility of a part (but you have to do this in each view in the drawing).
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If you create a Level of Detail, you can assign that to the main view in your drawing by editing the view and selecting that LOD. Views created FROM the main view should also change to the new LOD. If you need to do it view by view (on in one, off in another) you may have no choice but to re-create your views, all as base views.
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View Representation.... Expand the Representation folder. Right click on the View node and select "New". Turn off the part you want by right clicking on it and select visibility.
The part will still show up in the parts list.
That's what I was afraid of. Is there a way to set referenced parts to thier own layer and turn off that layer? That way I can just set the part to reference in the assembly model and it won;t show up in the BOM or the drawing. Right now they use the Phantom layer and I don't want to turn that layer off. Is there a global setting to place all referenced part on a specific layer?
Thanks for the response! This is not what I'm looking for. This turns off the visibility, but the part still shows up in the BOM. Also I'd have to turn of the visibility in every view.
Mike,
If you create a view rep, you can apply it to all the views on the idw and you can set it associative. That way if the model changes (in the iam), then the idw will update automatically.
You will still have the part in the parts list though. If you have cases where it is there sometimes and sometimes its not, maybe list it as optional in the parts list. Otherwise you might have to have two seperate assemblies (and idw). One with it and one without it.
If you make the part reference, you can hide all the reference data in the idw. Right click Base view in the idw and chose edit view. Go to the model tab.Under reference data select "off".
I never noticed that there was an option to not display references in the view. That will work fine for me.
The proper way is to create an iassembly and exclude or include parts you want.. because now you just have an incorrect BOM/parts list.
If you are happy with the workaround then go with it.. But its not technically the correct way.
The work around works because I have programming involved. IParts and iAssemblies are NOT an option!
That's funny! The only proper workflow for what you want to accomplish (under current state of Inventor) and it is not an option! LOL!
Regards,
Igor.
I don't see what so funny? You have no idea what my work flow is, and as I said earlier, I'm using programming to drive my models. IParts and iAssemblies are not suitable for the programming I'm doing!
It was just a figure of speech, so to say. Take it easy. Your work - your rules, I have no problem with that what so ever!
Best Regards,
Igor.
Another way to hide a part from the BOM:
Open the desired part
Tools-Document Settings-Default BOM structure-choose Phantom