measure number between extension line

[jostroopers]

I have placed a part on a drawing.

I have added dimensions.

This model can occur in different lengths.

If I change the model in length, my model will be neatly adjusted in the drawing.

Only the number of the dimensions is no longer in the middle between the extension lines.

How can I make sure that the number is neatly in the middle between the extension lines after I have changed the length of the model.

[Sergio.D.Suárez · Accepted solution]

Hi, I think you should look for a way to identify the dimensions. In this example of ilogic, you will center all the dimensions of the active sheet

Dim oDoc As DrawingDocument = ThisDoc.Document
Dim oSheet As Sheet= oDoc.ActiveSheet
For Each oDrawingDim As DrawingDimension In oSheet.DrawingDimensions
    If TypeOf oDrawingDim Is LinearGeneralDimension Or _
       TypeOf oDrawingDim Is AngularGeneralDimension Then
        Call oDrawingDim.CenterText
    End If
Next

You can center a specific dimension if you identify it through the item, as in this example

Dim oDoc As DrawingDocument = ThisDoc.Document
Dim oSheet As Sheet = oDoc.ActiveSheet

oSheet.DrawingDimensions(1).CenterText

 Maybe you could put an event to the drawing file so that the rule runs automatically. For example, before any change of drawing view or before saving the drawing file.

I hope this helps with your problem. regards

[jostroopers]

Hi Sergio

Thanks for the quick response.

The first code works for me.

I placed it to the After Save Document event trigger.

Thanks a lot.

[CCarreiras]

Hi!

I tried the code but ia have an issue... i have to run it twice to center the dimensions.

Fisrt time i run the code, nothing happens.

It's supposed to work like that?

inv2020.1

[Sergio.D.Suárez]

The code is not supposed to do that, try this code

If the code does the same as above, try the following. 

Dim oDoc As DrawingDocument = ThisDoc.Document
Dim oSheet As Sheet= oDoc.ActiveSheet
For Each oDrawingDim As DrawingDimension In oSheet.DrawingDimensions
    If oDrawingDim.Type = 117474560 Or oDrawingDim.Type = 117474816 Then
        oDrawingDim.CenterText
    End If
Next

 Sometimes inventor performs the operations but the changes are not displayed correctly, a trick that works for me is to turn on and off so that they update themselves.

Dim oDoc As DrawingDocument = ThisDoc.Document
Dim oSheet As Sheet= oDoc.ActiveSheet
For Each oDrawingDim As DrawingDimension In oSheet.DrawingDimensions
    If oDrawingDim.Type = 117474560 Or oDrawingDim.Type = 117474816 Then
        oDrawingDim.CenterText
		oDrawingDim.HideValue = True
		oDrawingDim.HideValue = False
    End If
Next

I hope this helps. regards

[CCarreiras]

Hi!

After i add your fixes, it star to working well.

Then... i deleted the fixes (back to the original code again).... and now, it works well!!
Therefore...... your original code should work well.

Sorry,  i don't know what happens before.

[jostroopers]

After some tests with the length of my model, the dimensions were not placed in the middle. I also used the other codes but then nothing changed. I now have an event trigger after saving the document and have placed the rule in it twice. Now it works.