How to define linear spacing in a drawing that updates automatically

[SEC_CAD]

Inventor 2022 DWG:

I want to define linear spacing in my drawing as per this extract from my old BSI PP 7308

The way that I did it was to manually edit the text prefixing the measured value

But my model geometry changed and now this manual equation is untrue (3 x 10.67 does not equal 32.61)

How can I automate my dimension text override so that the equation is always true, even if my model geometry changes again?

[cadman777 · Accepted solution]

I've done this in the past using Parameters in the dimension text edit dialog.

If your part doesn't change its name, then you may be able to do it.

It's a lotta steps to get it done, requiring planning ahead if you have a lotta parts you want to do this to.

You need to make some Parameters in the 3d part file that you can access in the drawing file dimension text dialog.

See attached example...

[SEC_CAD]

Thanks @cadman777 . I generally use parameters anyway.

It wasn't obvious to me how you had done it but I edited your numbers and the changes carried through to the drawing so I hunted for the mechanism.

I had never clicked on the pencil icon on the Edit Dimension dialog before. Seems odd to have a text edit dialog that opens up an almost identical text edit dialog. I wonder why Autodesk didn't just incorporate the parameter feature into the Edit Dimension dialog.

Thanks for you help and for quickly supplying the demo file.

Cheers 😀

[cadman777]

Glad it you fingered it out!

To answer your rhetorical question:

No telling. I too asked that when I first encountered that phenomena. Don't think anybody will ever know, except the developers and maybe Johnson S, cuz he's real smart and 'has connections'.

[johnsonshiue]

Hi Folks,

Many thanks to Chris' kind words! I might be quick-witted but I am not smart. I barely do my job.

Regarding this workflow, this is my personal interpretation. The Text Editor is a shared component within drawing environment. If it has to be integrated to Dimension Edit command, it might have to be refactored, which may incur unnecessary work.

About the parameters not being available there, I suspect it is a limitation. The drawing dimension is like measurement. Essentially, it attach itself to selected geometry. When the geometry changes, it updates. Now. if parameters are allowed to be added, the dimensions will have to fetch the updated value somehow. It could impact performance.

But, I do see the need to add parameters there. Let me work with the project team to see if my reasoning makes sense.

I need to scratch the above comments. I was mistaken. The model parameters and user parameters are both available to choose from the Text Editor. It is just that they are not immediately available within Dimension Text dialog. I have explained the reason earlier already. It is due to a shared component. I am sorry for the confusion.

Many thanks!

[IgorMir]

That functionality is accessible through the combination of Retrieve Model Annotations option and Edit Dimension Text DB. In there you add model's User Parameters in front of the retrieved model dimension. 
Chris has already offered a solution. I just took it a bit further and made the part asymmetrical. (IV 2020 format) 🙂
Cheers,

Igor.

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@SEC_CAD wrote:

Inventor 2022 DWG:

I want to define linear spacing in my drawing as per this extract from my old BSI PP 7308

The way that I did it was to manually edit the text prefixing the measured value

But my model geometry changed and now this manual equation is untrue (3 x 10.67 does not equal 32.61)

How can I automate my dimension text override so that the equation is always true, even if my model geometry changes again?

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[cadman777]

Although I never use RetrieveDimensions, Igor's method is a better method b/c it takes into account a change in the quantity of holes and their position on the part. This is a definitely a good reason to use RetrieveDimensions. Then, with a little iLogic you can set limits on the hole size, spacing, distance from edge of part, etc.

[IgorMir]

Hi Chris,

There is although one little workflow needs to be mentioned. The Automated Centerlines. Quite often it gets overlooked and a series of clicks is made to create the centerline between the arrayed holes. Only to find out that it goes sick once the amount of holes is changed. With the Automated Centerline it too goes sick. But to delete it and introduce a new one is a lot more straight forward process, than recreating it using Centerline tool.

Cheers,

Igor.

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@cadman777 wrote:

Although I never use RetrieveDimensions, Igor's method is a better method b/c it takes into account a change in the quantity of holes and their position on the part. This is a definitely a good reason to use RetrieveDimensions. Then, with a little iLogic you can set limits on the hole size, spacing, distance from edge of part, etc.

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[cadman777]

Good point!

There's always something messing around w/us!

Probably nothing a little iLogic can't solve.

But don't ask me how...at least not yet!