Suppressing parts in assemblies and super-assemblies

[Anonymous]

I'd like to suppress parts in an assembly A and not have them appear in any assembly B where assembly A is placed, all the way up to the top. I've tried suppress, enable, visibility. I don't want to remove the suppressed parts yet because I'm trying out an idea in the assembly, but I don't want to have to hide the parts in every inheriting assembly either. I'm surely overlooking something simple but I've not found the right set of keywords to find the answer by searching.

Thank you

[Xun.Zhang]

Hello @Anonymous,

Sorry, It should be just working. 

Would you help share an example that not working for you?

[Anonymous]

Amazingly, it's never worked for me. I can put together an example
tomorrow. How should I be able to disable parts in an assembly (without
deleting them) and not see those parts when the assembly is placed in any
assembly? Visibility, enable, suppress, or something else? I don't have to
tinker with LODs? Seems like a simple task, but it's been one I struggled
along with a solution to.

Thank you

[gcoombridge]

In 'assembly A' suppress the parts you want hidden and save an LOD.

In 'assembly B' right click on the sub-assembly and choose 'representation'. Select the LOD from 'assembly A'. 

Also if you expand the browser node for 'assembly A' inside 'assembly B' you will be able to choose a representation.

Cheers,

Glenn

[mcgyvr]

You may want to utilize either LOD or Design View Rep functionality... They are beneficial workflows..

BUT

It sounds like you may be working in the "Master" view rep active hence why everything is still showing..

Check that and switch to default,etc... Master by default shows everything..

[Anonymous]

Hi Glenn, this is really close. Let's say I have Part 1 -> Assembly A -> Assembly B -> Assembly C ... -> Assembly Z. I suppress Part 1 in Assembly A, create the LOD, and select the LOD in Assembly B. It seems that I must then continue to select the LOD in all assemblies that that ever include Assembly A, directly or indirectly?  In SW, I suppress a feature in Assembly A, and it "disappears" from all inheriting assemblies without doing anything extra per assembly.

[Anonymous]

When I create a new assembly, View=Default and LOD=Master. With new assemblies, all works great if a LOD is created on each assembly before placing them in a higher level assembly. Perhaps that should be a new habit? I'm working with a large existing assembly. My question may be better stated as: Is there a way to force all containing assemblies to recursively switch from Master to LOD1? Again, I'm trying to emulate the behavior that when I suppress something deep in an assembly tree that it's seen in no containing assembly, regardless of depth. I hope I'm describing this in a reasonable way.

Thank you

[mcgyvr]

If you don't want to use LOD or design view rep functionality then why not simply turn off visibility of the part and avoid needing to create those LOD/DVR's.. 

Both LOD and DVR have their use cases.. If you just want to globally hide something then just turning off visibility in the subassembly should accomplish what you want.. 

[Anonymous]

I'm dumbfounded. Toggling visibility indeed works in new assemblies but not in any of my imported assemblies. Is there any reason why that might be? The imported assemblies came from SW 2014, if that matters. I've been ignoring this stone-in-my-show for nearly a year now, assuming Inventor had a different way of doing things. I wish I would have asked sooner. At least I see it's possible now. Thank you!

[Anonymous · Accepted solution]

Assemblies that are loaded in assemblies higher up "don't know" that you create view representations afterwards. And you have to create proper view reps on every level, stay away from 'master'. Following should work with existing assemblies. Create a view rep in the master assy. Create a view rep in the sub assy. Set visibility and lock the view rep. Save sub assy. In master assy set the view rep of your sub assy to the locked one just created. Visibility of the sub assy should update. Lock the view rep of the master assy.

Now every time you open the master and activate the view rep it should show what you want to see.

BTW, if you only want control of visibility then stay away from LOD or suppressing.

[philip1009]

It is a mistake that's all too common, Suppress means different things between Inventor and Solidworks, LOD's weren't meant as a kind of configuration tool, they were initially created to save on computer resources back in a time where computers couldn't handle large inventor assemblies very well, they should be avoided unless your computer can't handle the assemblies you're building.  Setting up Design View Reps all the way up is the way to go until you want more functionality and may need to learn iLogic to build an assembly configurator.

[johnsonshiue]

Hi Kent,

Inventor LOD was designed to be a memory management tool. It helped overcome the RAM limitation on 32-bit Windows. As a result, the tool does not alter design data. It simply unload the component document to save memory usage.

Like other experts already mentioned, you may consider using Design View Rep to manage PartsList (BOM stay unchanged).  Or, you may want to look into iLogic. You use iLogic rule to drive parameters at all levels. Also you can suppress any component (IsActive() = False). Once you create one variation, use iLogic Design Copy to make a copy of the assembly. Then you can work on another variation.

Many thanks!

[Anonymous]

Hi everyone, thank you for all the help, and this got close. Seems like the thread is 1) Don't use LODs, 2) Don't use Suppress, 3) Do use Representations. When I set the representation in the assembly, should I enable Associativity?

In my assemblies, sub-assemblies only have "Leave of Detail : Master". If they don't, showing or hiding a component of a sub-assembly at this level, including using All Visible or All Hidden, shows a dialog saying "The components are associatively set by other Design View Represenation." The option "Modify Design View Representation" always grayed out and I always OK the "Remove associativity" because Cancel is not going to help. This blows away the all the Representation settings on all sub-assemblies. Is "Modify Design View Representation" what I should use and why is it always gray?

Maybe the underlying question is: How would you do the following? I have an version 1 of an assembly and I want to add and remove some parts and quickly make version 2 and then toggle between them. I'm learning about another suggestion "iLogic Copy Design" and perhaps that's what I need.

Thank you

[swalton]

There is the Link LOD command. 

See https://help.autodesk.com/view/INVNTOR/2019/ENU/?guid=GUID-DC5F1769-F926-4A3B-9F21-2CB4711FF9F2

What is your end goal? If you want to reduce the load on your computer while you work on a sub-section of your assembly, LODs are a good fit.

If you want to show or hide different components in the assembly window or drawing views, Design View Reps are a good fit.  Make sure to edit the design view reps at the level they were created to avoid breaking the associativity to upper level assemblies.  

[philip1009 · Accepted solution]

Associativity is recommended so that any design view rep of the same name at all levels of assembly will automatically update at the appropriate levels (making part1 of sub-assembly1 invisible will make that part invisible at all higher level assemblies with the same view rep name automatically), breaking associativity with higher view reps of the same name means changes with that assembly will not affect others (making that same part1 invisible only affects that assembly and you'll have to remember to make sure all higher assembly view reps show the same on your own).

I agree it's not exactly the best way to set up this automation, but when it is set up the correct way future changes will not be anywhere near as tedious.  It's a workflow that just takes getting used to.