Exporting Parameters

[Anonymous]

Hello 🙂

I'm using Inventor 2016.

In the parameter window, all parameters have a checkbox in the "export" column. What exactly does that control?

I am going through a course that claims that said checkbox controls which parameters will be imported automatically when the part is placed in an assembly. That statement appears to be incorrect. At the same time, neither does it control which parameters are exported to Excel xml.

As far as I can tell, manually setting a check-mark in said check-box does not do anything. Inventor automatically updates this checkbox once the parameters have been imported into another part file or assembly.

Which of the two behaviors is the one working as intended?

Thank you for your help. 🙂

[Anonymous]

I know that Solid Edge has such an export checkbox as well, but behind that box, you can enter a "new name". When checked, and a name is filled in, that parameter becomes available (under that new name) in formulas, properties, etc...

But here in Inventor, I have no clue what it does.

[mdavis22569]

Share what you have ... 

[mcgyvr · Accepted solution]

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@Anonymous wrote:

Hello 🙂

I'm using Inventor 2016.

In the parameter window, all parameters have a checkbox in the "export" column. What exactly does that control?

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@Anonymous

Export parameters checkbox for each row simply creates a custom iprop of that parameter..

Go to the iproperties...custom tab and see..

[Anonymous]

Hello Mdavis

this is a functionality question and is not related to a particular file. I was just wondering about how that check-box is supposed to work.

I mean, the user can definitely place a check-mark in it. But doing that has no effect (the two possible effects might have been to automatically link the parameters marked thus into an assembly (1) and to ONLY export the so marked parameters when exporting to excel.xml (2).

In my book, option 1 makes no sense and logically, it might actually create a circular reference, if the assembly was allowed to automatically import parameters from a based part file. While it IS possible to manually link parameters to an assembly (from a part file) those imported parameters can be used in an assembly but not be modified within the assembly.

Option 2 might have made some sense if it worked. But as far as I can tell, the export action simply exports everything to excel (as far as I can see, it does not even deign to differentiate between model, reference and user parameters).

The way it actually seems to work is this: the checkbox is there merely to show the user which parameters have been imported by other part files (or assemblies).

In my initial post I was merely trying to find out which one of the options is actually intended functionality.

Thank you for your help.

[Anonymous]

Hello Jdg.

thank you for your reply. Unfortunately I have never worked in Solid Edge 🙂 So... I don't know 🙂

[Anonymous · Accepted solution]

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The "export" check/tick box makes the parameter available via the Custom tab in iProperties.

This means it is visible to other applications. Windows Explorer, now called File Explorer, could search a file's properties and would also search iProperties. I don't know whether File Explorer can see the parameters.

When you Derive a file into another and select which parameters to you want to import, this will automatically can this check/tick box to Export.

If you are in an assembly you can import parameters. I have previously imported Sheet Metal Thickness and used that within the Weld. I don't know whether importing a component's parameters into an assembly/weldment automatically makes in Exportable.

HTHs

[Anonymous]

Hey McGyvr

Thank you for your reply. I see what you mean. Never occurred to me to look there because for the time being I don't really work with any of the I's in Inventor. I'll have to read up on those iProperties.

Thank you for clarifying that the checkbox is not supposed to work like my course seems to point out.

🙂

[Anonymous]

Hello Duncan,

thank you for your reply.

As I mentioned to McGyvr, I don't really work with iProperties at the moment. So I don't know why it would be important to have the parameters potentially visible via file explorer.

It's the same with derived parts - haven't yet gone there with the education I am currently taking.

About the assembly, I know it is possible to import parameters, but not edit them. And yes, in my list of possible uses for imported parameters in an assembly I forgot to mention the welding setup - again, we don't work much with sheet metal either...

Thank you again for your reply 🙂

[Anonymous]

If the "Export" is unchecked (fx parameters, ipt part) in a row and there is a parts list in a drawing, it will result in disappearance of values in the column which has the same name/description as the row in which uncheck for "Export" was done.

If I want a value (for example in sheet metal parts) to be exported to a column in assembly (or part) drawing parts list, I should make sure to check "export" for this row.

Correct or not?

[jtylerbc]

@Anonymous, that is correct.

The reason is that, technically, the drawing parts list displays iProperties, not Parameters.  As was mentioned earlier in this thread, the purpose of the "Export" setting is to create a custom iProperty that matches the parameter.  One of the major reasons to do that is simply to get parameter values into the parts list.

Without the box checked, there is no longer a property, even though the parameter still exists.  So the source that the parts list actually pulls information from does not exist.

[johnsonshiue]

Hi Folks,

Let me explain why "Export" status is needed. Inventor has been on the market for more than 20 years. Back then, personal computers were not as fast, compared to modern PCs. At that time, the Windows was 32-bit with limited RAM (capped at 3GB). The design could easily outpace the hardware.

The Export flag is a way allowing Inventor to manage source/derived objects more efficiently. When a parameter is marked as exported, it will be included in custom iProperty and also it can be derived. The dual meanings can be confusing I have to admit. But, it was to simplify the workflows.

Imagine if there was no such flag, Inventor might have to check all properties and parameters and see if there is a need to update. The update process might take much longer. Imagine there could be unlimited number of levels and number of derived objects. Some control is required.

Many thanks!