topic Re: How to set in Inventor so that the dimension appears underline when there is a break in Inventor Forum

How to set in Inventor so that the dimension appears underline when there is a break

dusan.naus.trz — Wed, 05 Jun 2024 07:15:43 GMT

How to set in Inventor so that the dimension appears underline when there is a break?

ČSN EN ISO 5456 - 2

https://www.n-i-s.cz/cz/zobrazovani-nabytku/page/592/

When Break View is used, the underlined dimension value is used. See attached image

Re: How to set in Inventor so that the dimension appears underline when there is a break

CGBenner — Wed, 05 Jun 2024 10:58:21 GMT

@dusan.naus.trz

Hello! I'm not seeing a specific option to set this in the Styles Manager. You may need to create a new Dimension Style for this situation, which has the text underlined, and then manually select it for dimensions in these areas.

Anyone else have any ideas on this? Good luck.

Re: How to set in Inventor so that the dimension appears underline when there is a break

dusan.naus.trz — Fri, 07 Jun 2024 15:50:34 GMT

Hello,

Thank you. I create New dimension style. It would be useful to automate this.

I create Ideas https://forums.autodesk.com/t5/inventor-ideas/drawing-dimension-appears-underline-when-there-is-a-break/idi-p/12825803

Re: How to set in Inventor so that the dimension appears underline when there is a break

dusan.naus.trz — Fri, 07 Jun 2024 16:17:54 GMT

If I modify the Dimension. The underline will not appear. Please fix it, it's a bug. What do you think?

Re: How to set in Inventor so that the dimension appears underline when there is a break

johnsonshiue — Fri, 07 Jun 2024 18:47:09 GMT

Hi! The behavior is indeed a bit confusing. However, the dimension text is driven by the text style referenced by the given dimension style. By default, it is the Note Text style. You may enable the underline in the style. Then the dimension value text will be underlined.

Many thanks!

Re: How to set in Inventor so that the dimension appears underline when there is a break

vladimir_michl — Mon, 10 Jun 2024 11:12:08 GMT

You can also solve it automatically, using the measure and "underline" trick with the following iLogic macro:

'Underline "broken" dimensions - a tip from www.cadforum.cz Sub Main() Dim oDoc As DrawingDocument oDoc = ThisApplication.ActiveDocument Dim oSheet As Sheet oSheet = oDoc.ActiveSheet Dim Scl As Double ' View Scale Dim oDim As DrawingDimension For Each oDim In oSheet.DrawingDimensions Dim oView As DrawingView Select Case oDim.Type Case ObjectTypeEnum.kLinearGeneralDimensionObject, ObjectTypeEnum.kAngularGeneralDimensionObject oView = oDim.IntentOne.Geometry.Parent Case ObjectTypeEnum.kRadiusGeneralDimensionObject, ObjectTypeEnum.kDiameterGeneralDimensionObject oView = oDim.Intent.Geometry.Parent End Select Scl = oView.Scale Dim d As Double d = dist(oDim.DimensionLine.StartPoint.Y, oDim.DimensionLine.StartPoint.X, _ oDim.DimensionLine.EndPoint.Y, oDim.DimensionLine.EndPoint.X) d = d / Scl If Math.Round(d,4) <> Math.Round(oDim.ModelValue,4) Then ' equal? 'oDoc.SelectSet.Select(oDim) If Not oDim.Text.FormattedText.Contains("<br/> \U+0305") Then 'was: <StyleOverride Underline='True'> 'oDim.Text.FormattedText = "<StyleOverride Underline='True'> <DimensionValue/> </StyleOverride>" oDim.Text.FormattedText = "<DimensionValue/><br/> \U+0305 \U+0305 \U+0305 \U+0305 \U+0305 \U+0305 \U+0305 \U+0305 " End If End If Next End Sub Function dist(y1 As Double, x1 As Double, y2 As Double, x2 As Double) dist = Sqrt((y1 - y2) ^ 2 + (x1 - x2) ^ 2) End Function

Vladimir Michl, www.arkance-systems.cz - www.cadforum.cz

Re: How to set in Inventor so that the dimension appears underline when there is a break

dusan.naus.trz — Mon, 10 Jun 2024 11:58:17 GMT

Unbelievable. That's very interesting. Thank you.

Re: How to set in Inventor so that the dimension appears underline when there is a break

dusan.naus.trz — Mon, 10 Jun 2024 13:18:14 GMT

@CGBenner and @johnsonshiue

After reading the current standard ISO 129-1, THE UNDERLINED DIMENSIONS ARE NOT INDICATED ANYWHERE after using Break in the view.
We do not require this functionality. It was a unique case with a customer. We won't use it anymore. The existing functionality contained in Inventor is correct.
The ČSN EN ISO 5456 - 2 standard only talks about the projection of component views. The information that was on the website is not listed anywhere.
Recommend discussion: If someone wants this functionality, let them supply additional documents.
I'm in favor of scrapping this idea and we won't be using it in future drawings.