How to lock level of detail

[Anonymous]

How to lock level of detail in inventor assembly

[Xun.Zhang · Accepted solution]

Hi Jay,

Unfortunately, LOD can't be locked right now.

Thanks!

[CCarreiras]

HI!

Workaround: create view representations, lock them, and create LOD based in that view rep.

[johnsonshiue]

Hi! LOD is a memory management tool. Do you mind elaborating the need to lock it?

Many thanks!

[Anonymous]

Hii ,
I creates level of detail for my drawings and analysis(mechanical simulations).
For example I am creating one level of detail and i run my simulation and I will get solution like I have to modify my assembly to relieve stresses. Also I have to keep this case study as same for record.
Now I am creating another level of detail in that I will add few modification, then in previous level of detail the added component in new level of detail will come. So old level of detail may disturb.
That is why I have to lock level of details.
As you know in view representation we can lock view so new added item cannot come in lock view.
I think you got my point now.
So the concern is to lock the level of detail may solve the issue .
But as per Autodesk they don't have this option.
Thanks for help
Sincerely
Jay

[Anonymous]

Here's my take on the issue-- similarly to how the ViewRep setup works, it would be nice to offer lockability of LODs for the following reason: When a LOD is created, it may be only partway through design of a complex system, but is only ever intended to load a specific group of components (for memory management purposes). Hence, if there are more parts/components added to the assembly model AFTER the fact, those parts are then added to all created LODs (since they cannot currently be locked).

The problem is this -- There is no current solution to prevent changes to existing LODs. Suppressing the link to the Base Component is only a temporary solution to this, as IV requires a model update once the link is unsuppressed BEFORE being able to edit the included components from the Derived reference (and thus, automatically loads any unwanted new components/parts). Breaking the link permanently disables further updates from being captured by the model containing a Derived reference, so this is not a solution.

The only way direct way around this is to maintain each individual LOD (in the Derived reference) by periodically suppressing new components. Depending on quantity of components present, this can represent exponentially longer model update times, and unnecessary model maintenance, as the parts need to be loaded/unloaded for each LOD, upon activation. This is also an unsatisfactory solution, as this would need to be done EACH time a new component is added to the Derived reference, or whenever the model containing the reference is intended to be updated. This may or may not even be possible if one is working within a multi-user environment using a Vault implementation, due to the required assembly file potentially being checked out by another user (this frequently is the case in a small company working on big projects).

Obviously this affects productivity, directly, since it extends the amount of time required for each operation. The best current indirect workaround (to me, anyway) is to copy a locked, maintained ViewRep to a LOD of matching name (using the Copy ViewRep to LOD function, and containing only the parts intended to be present in a purpose-driven LOD). However, this, while simpler to implement, would still need to be done (each time) before updating a model containing a Derived reference. In order to avoid naming issues, it would also have to be done AFTER ensuring the previous LOD (the one intended to be updated) is deleted from the LOD list. I imagine that a Macro or an iLogic rule could be created to automate this operation (though I haven't tried to do so).

A caveat to my above workaround -- though this should work for Drawings (but you shouldn't be using LODs to manage drawing views anyway, that's what ViewReps are for!), I have not tested it against Derived references, and don't yet have evidence it won't screw up the part loading/unloading in a model containing a Derived reference, due to the deletion of the previous referenced LOD.

So, to wrap it up, PLEASE PLEASE PLEASE add the ability to lock a LOD to Inventor!

Also, I don't know if it belongs as part of this request, but another nice functionality would be for ViewReps and LODs to be "linkable" through an explicit operation. What I mean is this -- if a ViewRep is copied to a LOD (or the inverse), a context-menu option becomes available (via right-click) to associate the two representations (could be as simple as only being available if the names match) and any updates to component states within either one. Selecting this option would maintain a visibility/suppression state link between the two -- see my hypothetical example below:

1. Create ViewRep [named view], w/only desired components shown

2. Right click ViewRep, select "Copy to Level of Detail"

3. Mini dialog box pops up with a checkbox "Link Representations", add check to checkbox, click "OK"

4. New LOD (with matching name to its base ViewRep) is created, and a chain-link icon is visible next to both representation names, to indicate that they are Linked Representations.

5. Effect a visibility/suppression state change in either representation, and update model. At this point, any components that have had EITHER a suppression or visibility change, or both, reflect these changes in both representations, without any additional maintenance necessary.

6. Any models/drawings that reference these Representations (appropriately) should then update without having to redefine any relevant design intent.

***I may edit this if I notice typos or decide to change wording around for clarification.***

[johnsonshiue]

Hi! I see your points. I have heard similar feedback. However, LOD is kind of misunderstood. LOD was designed as a memory management tool. It was essential to enable users to design large assembly requiring more than 3GB RAM to load on 32-bit Windows. By suppressing some components, the memory consumption would be reduced. Without it, Inventor user would be limited to 3GB RAM back in the old days.

Some users do try to use LODs for configuration purpose. iLogic has a functional called IsActive() helping user change the BOM attribute of an occurrence from Normal to Reference. It creates an illusion that LOD can alter BOM table. This workflow works for two configurations (Master vs non-Master). If you create a 3rd variation, the second one will be wrong. It is because a component occurrence can only have one BOM attribute (either counted or discounted).

There is room for improvement in every corner of Inventor. LOD is not an exception. The ideal behavior is that each LOD or state should be independent from others. And, the change to each state can be saved at the same time. Also, the state can be locked. We are working on a project called Alternative Representation. If you are interested, please sign up Inventor Beta program (https://bit.ly/InventorBeta) so you can test the latest internal build and participate in discussions.

Many thanks!

[Curtis_Waguespack]

---

@Anonymous wrote:

... if there are more parts/components added to the assembly model AFTER the fact, those parts are then added to all created LODs (since they cannot currently be locked).

---

Hi @Anonymous

Welcome to the forum.

I use this ilogic rule to help with the issue you describe, it suppresses the selected component in all but the active LOD:

http://inventortrenches.blogspot.com/2014/10/ilogic-suppress-cpmponents-in-all-but.html

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

It would be nice to have 2 different default setups for Level of Detail ...

1. Create LOD with all items unsuppressed by default and the user selects which items to suppress.

- This is the current Inventor method.

- Keeps the LOD always updated with new items as they are added to the assembly but allows user to designate specifically what items to keep out.

2. Create LOD with all items suppressed by default and user selects the items to keep unsuppressed.

- Once the LOD has been created and items selected to include (unsuppressed), all new items are suppressed by default. This method allows a LOD to be "locked" and will only change if user specifically modifies it. This is a perfect method if you use LOD in drawings or for analysis and don't want a LOD to be continually changing as your assembly evolves.

Note: this feature has been available in many other 3D cad systems for sometime.

[johnsonshiue]

Hi! Indeed, the ability to represent a model in different states within the same file at the same time is not yet available. Like I mentioned earlier, LOD is a memory management tool. It is not a tool to create multiple model states.

We are aware of the deficiency. We are working on a project called Alternative Representations. If you are interested, please sign up Inventor Beta (https://bit.ly/InventorBeta) and join the discussion.

Many thanks!

[craig.embry]

Seems like AutoDesk creating a work-around to do something that a lot of people have started using for "other" purposes might be more work than to just make the option available.  I too would like to see the LOD lockable from new states of the assembly.  I use these frequesntly enough for "other" purposes that it would be tremendously useful.  Even though the LOD was made for purposes other than what drafters are using it for now, you created an option that has morphed into other posibilities and advanced options for users looking to create their own systems of detail that work for them.  (LOD is in fact a way now to create model states, whether impied in creation of (or definition you have given) the utility or not.)  It seems to be a classic case of not truly listening to your customers.  We, as users, do understand that LOD was created for something else, but having the ability to pivot to customer demands and providing a better platform for those using it should probably be a top priority (even if its done with rolling eyes and a sigh).  Just my 2 cents.