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Calculating Mass for various Levels of Detail

9 REPLIES 9
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Message 1 of 10
Branon
4354 Views, 9 Replies

Calculating Mass for various Levels of Detail

Hi there,

 

I have an assembly in which I have created two levels of details (besides Master and the other default levels)

I notice that when updating the mass in iproperties, it is calculating all the components including all suppressed ones, no matter what level of detail is active (i’m assuming its calculating from the master LoD)

 

Is there a way the mass can be calculated dependant on what LoD is active or selected? It’s mainly for our GA drawings. In the title block we have a field called ‘Mass’ where we import the product mass from iProperties. I don’t want this to show all components in the assembly (ie. I don’t want it to show the suppressed components), but I would like to do is create a separate page, or view, showing all components and the mass.

 

To make it clearer, the product is a trailer and I want the title block to state the un-laden mass, with a separate view showing the loaded trailer plus its overall mass.

 

Would appreciate your advice.

 

Regards,

Brendan

9 REPLIES 9
Message 2 of 10
jakefowler
in reply to: Branon

Hi Brendan,

 

Thanks for posting this issue!

 

I believe this workflow should be supported, and with a quick experiment I was able to obtain a Level of Detail-specific mass value in both the Assembly environment and in a drawing title block.

 

In the Assembly environment, you should be prompted when calculating the mass properties using a non-Master Level of Detail, to ask whether you wish to calculate for the Master or current Level of Detail. If you don't see this prompt, it's possible that it has been suppressed on your machine. You can check this in the Application Options under the 'Prompts' tab: scroll down to the item "Do you want to calculate the Mass Properties for...", and ensure that the 'Prompt' field is set to 'Always'. (When this dialog appears, you will need to press 'No' to return the Level of Detail-specific mass properties.)

 

In your drawing title block, if you have inserted a Text field that includes the 'MASS' Property from the 'Physical Properties - Model' property Type, its value should update depending on the Level of Detail of the assembly represented in the drawing sheet. Are you using this method to place the mass value in the title block, or are you using a different workflow?

 

Also, is it possible to let me know which version of Inventor you are using? I am testing this using Inventor 2013, but if you are on an earlier version I will need to verify these steps on this release.

 

Hope this helps, and if not please let me know more details so that I can try to help you figure this out.

 

Thanks!

Jake



Jake Fowler
Principal Experience Designer
Fusion 360
Autodesk

Message 3 of 10
Branon
in reply to: jakefowler

Many thanks for this Jake,

 

You were quite right, this promt had been suppressed, and so upon unsuppressing, I was able to calculate the mass depenant on which LoD was active.

 

Due to stability issues I was having with Inventor, I did however end up resolving it a different way. I simply did a "save copy as" for the different LoD, and placed that copy on a seperate page in my GA drawing with all the cargo, and simply deleted the cargo from my main GA model.

 

I am running Inventor 2012 on a 32bit xp workstation. I often run into stability issues particularly creating drawings of fairly complex models (anything over 500 parts). This does sometimes, I feel, prevent me utilizing all the features of inventor. I'm never sure though to class them as software limitations, or hardware limitations........ or just a straight up pain in the backside 🙂

 

Never the less your advice has helped and I shall be utilizing this feature of future (less complex) models. 

 

Kind Regards,

 

Brendan

Message 4 of 10
jakefowler
in reply to: Branon

Hi Brendan,

 

Apologies for not replying back to this sooner; I’m very glad to hear that the last post helped to resolve your issue!

 

Regarding your stability issues with complex models: I think there is a fair possibility that this could be related to using a 32-bit platform. 32-bit applications have a limit on the amount of RAM they can address (technically 4GB, although typically the memory a Windows application can actually make use of will be less that this). When Inventor (or any application) reaches the limit of the available RAM, it will need to start making use of virtual memory, which will certainly result in performance issues and may also be causing some stability problems for you.

 

For dealing with larger models, it’s recommended to use a 64-bit system with enough RAM to handle the size of your datasets comfortably. You can see the system recommendations for Inventor 2012 here; it might be worth comparing this list with the specifications of your machine to identify possible hardware bottlenecks.

 

Hope this helps, and many thanks again for taking the time to post here!

 

Jake



Jake Fowler
Principal Experience Designer
Fusion 360
Autodesk

Message 5 of 10
llorden4
in reply to: Branon

I'm currently on Inventor 2016 and this functionality now appears broken or I'm overlooking something.

 

I have a custom LOD defined, and while in the assembly file I do get the option to update mass of Master or Current LOD.  In an IDW drawing I am still getting N/A displayed for Mass Properties of the assembly.  I have also updated the BOM in the IDW to ensure the properties are updated but no luck.  What am I missing?

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Message 6 of 10
llorden4
in reply to: llorden4

I found a solution / workaround so I thought I'd best post it.

 

While making another attempt to insert the Mass Properties variable into the view callout, I accidentally selected Volume instead of Mass and didn't notice until after exiting the editor and noticed an unexpected value being displayed.  Going back into the editor I overwrote the Volume property with the Mass property and it's been working ever since.  Makes no sense to me and can't say it's going to work for every case, but there you have it.

Autodesk Inventor Certified Professional
Message 7 of 10
jpv7489B
in reply to: Branon

Inventor 2020 here -- the poor workaround I'm using at the moment is to create all the level of details and then create a derived part with the particular level of detail -- at least this way I can get the weight correctly.

Sadly, I lose the BOM.

 

Please note that in this regard, SolidWorks has this completely solved and things works as intended (at least until 2019 version that is 😉)

Message 8 of 10
llorden4
in reply to: Branon

@jpv7489B, it's in another thread but another option I've been using is to create a custom iProperty and record the the mass properties of my current LOD.  Use the custom variable instead of the MassProperties variable when making your paper notations and you'll get reliable results.   I use an iLogic routine to update the custom iProperty whenever a model change is made.

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Message 9 of 10
jpv7489B
in reply to: llorden4

@llorden4, the problem with that is that you get a frozen weight value, whereas, in my use case at least, weight is a value that it's constantly changing due to several iterations in the design. I'm still working around the missing BOM -- but as I said above, coming from SolidWorks, it's a shame to encounter this kind of missing features.

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Message 10 of 10
llorden4
in reply to: jpv7489B

That's true ONLY if you don't apply an iLogic rule that will automatically update the custom iProperty as I mentioned.  I've had to use this process for some time now and it works well.  And I agree, we shouldn't have to make these kinds of work arounds.

 

Example code (requires you already have the custom iProperty created)

InventorVb.DocumentUpdate(False)	'required to get current mass properties
iProperties.Value("Custom", "WEIGHT") = Round(iProperties.Mass / 1 lbmass, 3)  
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