Add parameter from created dimension to note in drawing

[pjwolstenholme]

Hello all,

Please would anybody be able to tell me if it is possible to add a created dimension (say the dimension for a PCD) from the dimension to a hole note and keep the link, rather than just adding it as dumb text? I know you can do this with the driving dimensions, by selecting from the pull-down menu, but am not sure how to do it with created dimensions. In SolidWorks, you simply click on the dimension in the drawing, and in Creo, you can add '$d0' for example (the paramter name for the dimension. I am unsure how to do it in Inventor.

Thank you very much,

Kind regards,

Phillip

[Frederick_Law]

Mark the parameter for Export and it will show as Custom Properties.

[pjwolstenholme]

Hello,

They are not driving dimensions though, it is just a dimension I have created in my drawing, but I want to use value in a note, and keep the link? When I go to my parameters window in the drawing, there doesn't seem to be any way of getting my created dimension in as a parameter?

[cadman777]

I don't know any way to add it to the HoleNote tool.

But you can add it to a Leader or to an existing Dimension.

LEADER:

In the Leader d.b., set Component>Source>Parameter>Precision, and then click on the button just to the right of Precision.

DIMENSION:

RMB on the Dimenision and select Text. Then set Component>Source>Parameter>Precision, and then click on the button just to the right of Precision.

It's an elaborate work-around to a function that should be a single click.

[SBix26 · Accepted solution]

@cadman777 , the OP does not have a model parameter to use for this.  They want to use a dimension placed in the drawing in drawing text.  I don't see any way to do this, period.

The only workaround, as noted by the others is to place the dimension in a model sketch, export it to custom iProperties, then retrieve it from there.  The dimension can also be retrieved in the drawing view instead of placing a new one, if that helps.

Being able to access drawing dimension values in a note seems like a useful idea, though-- Inventor Ideas forum.

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Sam B

Inventor Pro 2023.2.1 | Windows 10 Home 21H2

[cadman777]

I'm confused, b/c the words he used indicated he was talking about using a model parameter in a dimension hole callout, which I can't do in IV2010, nor does it seem like it can be done in 2023. In all the decades that I did 2d and 3d modeling and drawings, I never had a need nor the inclination to use a drawing dimension value in another drawing dimension. So it makes no sense to me when or why anyone would want to do that.

[IgorMir]

Exactly! 
Why would it be necessary to add to a Hole Note on the drawing the information from the drawing? Maybe the dimension could be referenced into the Note if it is itself is placed from the model's sketch on the drawing. But it is a long shot and I don't want to look into it. Because I don't see any need for it myself. Maybe someone else does...
For all other occasions - to link model parameters to the leader text (to any text, BTW) is a fairly straightforward process. 
Cheers,

Igor.
P.S. I think, Chris - the model dimensions can be added to a Hole Note in IV2010. Please have a look at the attached picture. Doesn't IV2010 got the same menu? The hole dimension callout is controlled by the hole itself. But any additional info can be added afterwards. And that includes dimension of PCD. Subject - that very dimension is available either like Model or User parameter in the model itself.

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@cadman777 wrote:

I'm confused, b/c the words he used indicated he was talking about using a model parameter in a dimension hole callout, which I can't do in IV2010, nor does it seem like it can be done in 2023. In all the decades that I did 2d and 3d modeling and drawings, I never had a need nor the inclination to use a drawing dimension value in another dimension. So it makes no sense to me when or why anyone would want to do that.

[SBix26]

In message #3 the OP refers to a note.  I think they are wanting to place a note on the drawing with specific instructions, explanations or details about a particular dimension, which they'd like to reference by its value.  Something like:

"Note: 4.15 dimension is to the center of the 12.0 radius, not to the nearby edge"

If this could be done, the two dimensions in that sentence would update when the drawing dimensions changed.  I can see using it, but very rarely.

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Sam B

Inventor Pro 2023.2.1 | Windows 10 Home 21H2

[IgorMir]

Hi Sam,

If such an instruction is needed - then there is a good point in creating that very dimension(s) on the model itself. And link them to the drawing text afterwards. Wouldn't you agree?
It all boils down to the way the design of any particular part is made. And if the design intent is preserved in the part carefully. I understand that it is not always easy to record the design intent from the word go. But in due course - its not that difficult to alter it either. 🙂
Cheers,

Igor.

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@SBix26 wrote:

In message #3 the OP refers to a note.  I think they are wanting to place a note on the drawing with specific instructions, explanations or details about a particular dimension, which they'd like to reference by its value.  Something like:

"Note: 4.15 dimension is to the center of the 12.0 radius, not to the nearby edge"

If this could be done, the two dimensions in that sentence would update when the drawing dimensions changed.  I can see using it, but very rarely.

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Sam B

Inventor Pro 2023.2.1 | Windows 10 Home 21H2

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[cadman777]

You are correct...nice!

I never noticed that before, but now I have a new method.

Thanx! 😁

[cadman777]

Thanx for the clarification. So in that case the OP should add a driven dimension to the model, and then access it in the drawing. He needs to learn how Inventor works so he can get the most mileage out of it.

[pjwolstenholme]

Thank you very much for all your help guys, much appreciated!

[pjwolstenholme]

Hello everybody,

I want to add the PCD of my holes to the hole note. I did export the dimension from sketcher, but don't know if there is any way to get it into my hole note.

My useal way of defining hole pattersns is something like:

8 HOLES Ø10 mm THRU

EQUI-SPACED AS SHOWN

ON A Ø150 mm DIA

[cadman777 · Accepted solution]

Just do like I told you:

If the model is a native parametric Inventor model, then get the dimension from the part model Parameters.

Otherwise, if the part is an imported non-parametric part, then make a UserParameter in the part model and use it.

I've been doing it like that for over 20 years b/c I couldn't find any other way to do it.

Look at my screen caps above and @IgorMir's MESSAGE 7 OF 14 to see how to do it.

[cadman777]

So did you do it the 'hard' way and did it work for you?

I just did it with pickets on a railing...the number of pickets and the spacing.

The drawing updated after a change was made so I didn't have to chase around the dimensions on the drawings and manually fix them.

[Frederick_Law]

I do this for bolt circle.

If you need a dimension in model, you can add a driven dimension.