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Turn off part in drawing

13 REPLIES 13
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Message 1 of 14
meck
2310 Views, 13 Replies

Turn off part in drawing

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!

Mike Eck
Master Drafter/ CAD Programmer
Using Inventor 2018
13 REPLIES 13
Message 2 of 14
JDMather
in reply to: meck

You can turn off visibility of a part (but you have to do this in each view in the drawing).

 

Visibility.png

 


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Message 3 of 14
cbenner
in reply to: meck

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.

Message 4 of 14
karthur1
in reply to: meck

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.

Message 5 of 14
meck
in reply to: cbenner

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?

Mike Eck
Master Drafter/ CAD Programmer
Using Inventor 2018
Message 6 of 14
meck
in reply to: JDMather

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 Eck
Master Drafter/ CAD Programmer
Using Inventor 2018
Message 7 of 14
karthur1
in reply to: karthur1

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".

Message 8 of 14
meck
in reply to: karthur1

I never noticed that there was an option to not display references in the view. That will work fine for me.

Mike Eck
Master Drafter/ CAD Programmer
Using Inventor 2018
Message 9 of 14
mcgyvr
in reply to: meck

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.

 



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Message 10 of 14
meck
in reply to: mcgyvr

The work around works because I have programming involved. IParts and iAssemblies are NOT an option!

Mike Eck
Master Drafter/ CAD Programmer
Using Inventor 2018
Message 11 of 14
IgorMir
in reply to: meck

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.

Web: www.meqc.com.au
Message 12 of 14
meck
in reply to: IgorMir

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!

Mike Eck
Master Drafter/ CAD Programmer
Using Inventor 2018
Message 13 of 14
IgorMir
in reply to: meck

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.

Web: www.meqc.com.au
Message 14 of 14
brad
in reply to: IgorMir

Another way to hide a part from the BOM:

 

Open the desired part

Tools-Document Settings-Default BOM structure-choose Phantom

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