weight update

[akosi]

is there a way where i can  update the weights of all my assembly without opening each assembly ?

thanks

inventor 2011

vault pro 2011

[msklein]

in the bom look at upper right side of screen for update mass properties

msk

[akosi]

but i still have to open the iam file to update the bom?

i have hundreds of iam that needs the weight to be updated and show in the titleblock,

to show it in the titleblock , i have to open the idw or iam and update the bom .

what i want to accomplish is , update the bom of these idws or iam without opening one by one...

help is greatly appreciated...

inventor 2011

vault pro 2011

[johnsonshiue]

Hi! Based on my understanding of how Inventor works, the physical properties need to be evaluated with the documents open (either manually or programatically). There is no way to access and compute the properties without the docments open.

If I were you, I would use Task Scheduler to accomplish this task. Here is what you need to do.

1) Identify the folders and the projects containing the iam and ipt files.

2) Go to Tools -> Application Options -> check the checkbox "Update physical properties on save" and select "Parts and Assemblies" radio button -> Apply -> Close and close Inventor.

3) Go to All Programs -> Autodesk -> the corresponding Inventor folder -> Tools -> Task Scheduler.

4) Create an Update Design task by pointing to the project or the folders containing the iam and ipt files -> select only .iam type. Make sure in check "Rebuild All" in the options.

Then run the task.

After that, the mass properties in all iam and ipt files should be up-to-date. BOM and Drawings should be able to find the updated properties.

Let me know if you have any question.

Thanks!

[msklein]

Best i can tell you is that you can do this from the idw. Haven't tried to do it at the very top assy idw and verifed  that the lower idw's also update.

hope this helps some.

MSK

[akosi]

this make sense..ill try this one...

ill post the result

thanks a lot

[akosi]

1. i  "get latest from vault " from task sched first, so i can have a copy of the files to my local drive

2.  i "update design" and pick the iam that needs to show the weight

3. i open the idw that supposed to have the updated weight of the iam to see if it has the updated weight but still its not updated

4. so i have to open the iam file and then the idw weight now becomes updated.

in short, it doesnt work, enlighten me please.....

i need another option

thanks

inventor 2011

vault pro 2011

[johnsonshiue]

Hi! I am a bit confused here. The workflow should work because what I showed you is an automated way to ask Inventor to update physical properties and save the change. It is no different than opening the assembly and doe rebuild all and save. Could you open one of the assembly undergone Update Design? Then go to iProperties. Are physical properties up-to-date?

Opening a drawing referencing an iam or an ipt is very close to opening the iam and the ipt manually. These model files have to be loaded or the drawing will be empty.

Thanks!

[akosi]

i made a new iam , once i saved it , it update the physical properties -> no substitute level of detail but if i make a subs level of detail it will not give the update eventhough the current level of detail is using master and if i remove the subs level of detail, it will update the properties once saved.

ive checked the old iam that doesnt update it has subslevel of detail. i need to have this subslevel of detail

any options?

thanks for replying,

inventor 2011

vault pro2011

[johnsonshiue · Accepted solution]

Hi! When you try to update the mass properties in non-Master LOD, Inventor will prompt you "if you want to evaluate the mass properties based on Master or current LOD." If it is based on Master, it will grab the cached mass properties from Master LOD. If it is based on current LOD, Inventor will compute the mass properties by excluding any suppressed components.

I think you might need to set another flag in Application Options so that mass properties will be evaluated based on active LOD. Go to Tools -> Application Options -> Prompts -> find "Do you want to calculate the Mass Properties for the Master LOD? Yes or no (calculate as of current LOD) -> set the answer to the question to "No" and set the Prompt to "Never".

Then run the workflow I suggested.

Let me know if it works for you.

Thanks!

[akosi]

i tried the workflow several times..and it works...

thanks a lot

[Pantera7777]

Is there any possibility to update the weight in iAssembly?

I would like to place items into iAssembly from STEP pr PRT files and have different weights for all of them.

So could I avoid the step making .ipt files and go straight to .iam and have weights updated?

Many thanks

[prhoads3W8KL]

In order to draw the views of a drawing, Inventor must open the model in the background.  In other words, the drawing certainly does have access to the model file to be able to pull info from it and "push" commands to it, such as when a BOM detail is pushed form the drawing to the model.  It is merely a decision on the part of Inventor's developers and management not to make the mass properties stay up to date automatically or at least allow the user to update mass properties from the drawing.  Autodesk needs to prioritize basic ease of use deficiencies relative to competition over cosmetic changes from year to year.  Some years, the updates were so slim, the only thing I can tell Autodesk did was change the splash image.  

[johnsonshiue]

Hi Peter,

You got a great point here. Indeed, there is no technical reason why mass prop should not be updated or computed in a model-based view in the drawing. It is true the model is loaded when creating the view. I have to speculate why such workflow is not offered is probably for performance concern.

Mass prop compute is a relatively expensive process. For a single part, depending on the geometry, it should be fast. But, for a large assembly, it can take a while. I am not sure if you are aware an option in Tools -> App Options -> General -> Update physical properties on save. This will guarantee the mass prop to be always up-to-date.

Based on your reply, it sounds like you have some discontent regarding Inventor. I am more than happy to hear it. You can contact me directly (johnson.shiue@autodesk.com). Or, you can start a new thread describing the issues.

I cannot give you any promise that your concerns would be addressed immediately. I am just an engineer happening to know Inventor workflows really well and I like to help our users. But, I can guarantee you that every issue, concern, defect, wish, and comment will be carefully reviewed and necessary actions will be taken. Regarding the splash screen, that is out of my control.

Many thanks!

[prhoads3W8KL]

The option in setting does help, but it does not work when saving from the drawing, for some reason the mass does not update even though the dialog says the model is to be saved.  You have to switch back to the model and then switch back to the drawing as a work around to get it to update.  This is very basic stuff, not something I would think Autodesk would still be messing with and trying to get right in 2019.  I am hard on Autodesk only because I know y'all can do better.  

[stevenwestlake]

Thanks Mark, knew it was in there some place, just could remember where.