Can numeric parameter be formatted in an Inventor Drawing text box?

[s.mutschler]

In an Inventor Drawing (.idw), dimensions are formatted (i.e., as decimal or fractional) based on the style selected for the dimension annotation.  You can also force stacked-fraction formatting of specific numeric text within a text box.

However, text boxes don't seem to offer much control over retreived parameters.  When you insert a value from the parameter table into your text box or leader text, the retrieved parameter always gets pulled in as a decimal number regardless of how it was formatted in the part's parameters table.   

Are there any formatting functions that can be used within a text box or leader text to force fractional formatting for a retrieved parameter embedded within that text?

[mflayler2 · Accepted solution]

In the model the parameter is being retrieved from...

Go to the Parameters Dialog

Mark the Parameter for Export

Right click on the Parameter and choose Custom Parameter Format

Make your adjustments

This creates a Custom iProperty for that parameter.

In your drawing, in the text box...use the Custom iProperty instead of the Parameter value.  It will still update the same way as the parameter would.

[s.mutschler]

Thank you!  Nice trick!

However, I may have immediately discovered a programming oversight:

The "Custom Properties - Model" option only appears in the drop-down list in the dialog window for a Text Box.  That item does not appear in the list for the same drop-down in the "Leader Text" dialog window.  I can see no reason why the two dialogs should not offer the same list of parameter fetching options.  Both types of annotations really are just "text" boxes.

Is this intentional behavior?

[mflayler2]

I am able to place these (Custom iProperties - Model) in the drawing with Leader Text.

Inventor 2012 SP1

Make sure your referenced model in the drawing is the same as the one you modified and added the export.

[s.mutschler]

Stop that post.  I stand corrected.

The option appears in the Leader dialog, but only if the leader is associated with a View containing the relevant part (containing the iProperty).  Actually, only if the leader is "attached" to an element within the part drawing.

When I create a leader elsewhere in the drawing (free hanging as it were), I guess the program does not know what file to retrieve iProperties from.  Correct?

[mflayler2]

FYI: If you are not attaching to a model, then you wil not see the Leader Text.  So if you start Leader in the middle of the paper not attached to anything you will not see Custom iProperties-Model

[s.mutschler]

Thank you again.

[deondres034]

Is there a way to pull these properties into a dimension?

[Curtis_Waguespack]

Hi deondres034,
Can you clarify what you're wanting to do?

I suspect the question you asked, might not give us enough information to fully answer your overall question.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[deondres034]

Instead of using leader text and text boxes I'd like to pull those custom parameters into an actual dimension. For an example I dimensioned a hole size for an anchor bolt size in a base plate view. I want to tell it to use the actual anchor bolt diameter parameter set up inside my model so I won't have to go in the dimension and physically change it for every piece. Problem is that the type and property boxes are grayed. By doing this there will be less chance for human error when making corrections.

[Curtis_Waguespack]

 Hi deondres034,

I think what you're after can be done by using the Component dropdown box as shown:

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[deondres034]

The problem with doing it that way is that the parameters always come out in decimal form rather than fraction.

[cadman777]

Does anybody know if this got an answer somewhere else?

[johnsonshiue]

Hi Chris,

The formatting can be done at the parameter level, not at the drawing level. Drawing just display the value based on the styles and standard.

To change the exported parameter formatting, go to the Parameters table in the part -> find the exported parameter -> click click on the Equation cell -> click on the right-pointing arrow -> Custom Property Format. Then the parameter value will be shown in Custom iProperty based on the format options.

Many thanks!

[cadman777]

@johnsonshiue,

Thanx, but I already tried that before coming in here and asking.

I'm trying to automate as much as possible all dimensions and notes on the drawing so when anything changes (such as # of arrayed items, bolt sizes when no bolt is placed, etc.) it automatically updates. I don't want to use iLogic if possible.

[cadman777]

Does anyone know a way to format Parameters in the DimensionText DB and in the TextEditor DB?

Does anyone do this on their Inventor drawings, or want to do it?