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
Solved! Go to Solution.
Solved by vladimir_michl. Go to Solution.
Solved by CGBenner. Go to Solution.
@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.
Chris Benner
Industry Community Manager – Design & Manufacturing
If a response answers your question, please use ACCEPT SOLUTION to assist other users later.
Also be generous with Likes! Thank you and enjoy!
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-br...
If I modify the Dimension. The underline will not appear. Please fix it, it's a bug. What do you think?
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!
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
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.
Can't find what you're looking for? Ask the community or share your knowledge.