If I run this iLogic program it aligns them incorrectly. If I use a Chain Set, that dimension does not respond to alignment
Is it possible to automatically arrange Chain dimensions
If you have a chain dimension set, please try the ChainDimensionSet.Arrange method. That should give better results.
The help says that the general DrawingDimensions.Arrange method doesn't work for dimensions that are members of chain dimension sets. (However you should be able to arrange the whole set if you provide the set object itself as an argument to that function.)
Mike Deck
Software Developer
Autodesk, Inc.
I think he's talking about this:
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kDrawingDocumentObject Then
MsgBox("This rule only works for Drawing Documents.",vbOKOnly, "WRONG DOCUMENT TYPE")
Exit Sub
End If
Dim oDDoc As DrawingDocument = ThisDrawing.Document
Dim oSheet As Inventor.Sheet = oDDoc.ActiveSheet
Dim oChainDimSet As ChainDimensionSet
For Each oChainDimSet In oSheet.DrawingDimensions.ChainDimensionSets
oChainDimSet.Arrange(oChainDimSet.Members.Item(1))
NextThe ChainDimensionSet object has its own Arrange method. When calling this method, it wants you to specify a base (LinearGeneralDimension) as input, so it can use that dimension as the basis to arrange all the other 'Members' of the set. In my example code, I'm simply specifying the first 'Member' of the set as the input general dimension to base the Arrange method on. Here's the link to the Help page for this.
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Wesley Crihfield
(Not an Autodesk Employee)
There is also a similar method for BaselineDimensionSet shown here.
Wesley Crihfield
(Not an Autodesk Employee)
That last code would have only worked on real ChainDimensionSets that were created as chain dimension sets when created. Here is an iLogic rule that attempts to combine all the different types of dimension types and all their different methods for arranging them. This should catch pretty much any type of dimension you created on your drawing. Try this:
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kDrawingDocumentObject Then
MsgBox("This rule only works for Drawing Documents.",vbOKOnly, "WRONG DOCUMENT TYPE")
Exit Sub
End If
Dim oDDoc As DrawingDocument = ThisDrawing.Document
Dim oSheet As Inventor.Sheet = oDDoc.ActiveSheet
Dim oDDims As DrawingDimensions = oSheet.DrawingDimensions
For Each oDDim As DrawingDimension In oDDims
If TypeOf oDDim Is LinearGeneralDimension Or _
TypeOf oDDim Is AngularGeneralDimension Then
oDDim.CenterText
End If
Next
For Each oBaselineDimSet As BaselineDimensionSet In oDDims.BaselineDimensionSets
oBaselineDimSet.ArrangeText
Next
For Each oChainDimSet As ChainDimensionSet In oDDims.ChainDimensionSets
oChainDimSet.Arrange(oChainDimSet.Members.Item(1))
Next
Dim oCollection As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection
Dim oLinGenDim As LinearGeneralDimension
For Each oGenDim As GeneralDimension In oDDims.GeneralDimensions
If TypeOf oGenDim Is LinearGeneralDimension Then
oCollection.Add(oGenDim)
End If
Next
oDDims.Arrange(oCollection)If this solved your problem, or answered your question, please click ACCEPT SOLUTION.
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Wesley Crihfield
(Not an Autodesk Employee)
I also find it very interesting that the "CenterText" method works, even though there doesn't appear to be any mention of it within the online help page for the DrawingDimension Object. But it is being used within the sample code.
Wesley Crihfield
(Not an Autodesk Employee)
@WCrihfield , not all dimensions have a CenterText method. But LinearGeneralDimension and AngularGeneralDimension do. Those are both derived from DrawingDimension.
Mike Deck
Software Developer
Autodesk, Inc.
Ah, I see now. Apparently I didn't dig deep enough when looking into that point before. Thanks for the helpful links.
Wesley Crihfield
(Not an Autodesk Employee)
That last code I posted worked just fine for me, so I'm not sure why it's not working just as good for you. I created a screen cast video of me dimensioning one side of a part using regular General dimensions, then dimensioning another side of it using Baseline dimensions, and another side using Chain dimensions. Then I move the text and positioning of all these dimensions around to create a little chaos for the rule to deal with. Then I show you the contents of the iLogic rule before I run it. Then I run the rule, to show you how it acts on my computer.
The video is attached:
And here is the link to the ScreenCast.
Wesley Crihfield
(Not an Autodesk Employee)
I see what you mean now. That scenario of having multiple chain dimension sets on the same side and using the usual iLogic arrange methods definitely leads to unfortunate and unwanted results. Seems this is one of those things that maybe Autodesk needs to look into further, and possibly offer an update for sometime in the future. Though it would likely be pretty low on their priorities, since there may not really be that many folks out there attempting to achieve this exact scenario.
An iLogic solution for this scenario would likely have to go into much more detail than those standard Arrange functions offer, if it is possible at all.
Wesley Crihfield
(Not an Autodesk Employee)
@robertast , are you looking only for improvements in the Inventor API and iLogic?
Or do you also need improvements in the way the Arrange command on the ribbon works?
In other words, does the Arrange command to everything you need, with no programming required?
Mike Deck
Software Developer
Autodesk, Inc.
It would probably be best to do an extra command "arrange all" right in the program. The current one should remain as an option. But it has to work right.
Until such is the case, I was hoping to solve this with the help of iLogic. And if that succeeds, offer Autodesk a ready-made solution.
I was interested in @JhoelForshav decision SOLUTION.
When it resolves dimension centering when text does not fit between dimension lines.
So I’m looking for any quick way to properly arrange the dimensions. This will be very relevant in the new version of 2022 as well, as the annotations in the tarpaulins will run out and have to be handled.
