topic Re: Retrieve dimensions in Inventor Programming Forum

Retrieve dimensions

theo_bot — Mon, 08 Oct 2012 13:45:53 GMT

Hi,

I want to retrieve dimensions in a drawing with ilogic. I found some code in de api help, but i can't figure out how to translate it into a ilogic code.

I always use assembly models in these drawing and all the parameters have unique names. So in my drawing i want to retrieve some specific dimensions in a view.

Can anyone point me in the right direction? maybe a small sample?

kind regards,

theo

Re: Retrieve dimensions

marco_suurlant — Wed, 10 Oct 2012 06:54:10 GMT

Hello Theo,

Here you have a little example how-to retrieve dimensions with a special parameter name in iLogic.

The workflow I use is:

1. Retrieve all dimensions.

2. Iterate through the dimensions.

3. Delete dimensions if not a special parameter.

The special parameter name has a prefix “RetD_” as model / userparameter.

Start code”

Dim oDrawDoc As DrawingDocument = ThisDoc.Document

Dim oSheet As Sheet = oDrawDoc.ActiveSheet

Dim oDrawView As DrawingView = oSheet.DrawingViews(1)

Dim oGeneralDimensionsEnum As GeneralDimensionsEnumerator

oGeneralDimensionsEnum = oSheet.DrawingDimensions.GeneralDimensions.Retrieve(oDrawView)

Dim PrefixStr As String = "RetD_"

Dim oGeneralDimension As GeneralDimension

For Each oGeneralDimension In oGeneralDimensionsEnum

Dim oParameter As Parameter

oParameter = oGeneralDimension.RetrievedFrom.Parameter

If oParameter.DrivenBy.count <> 0 Then

Dim oDrivenByParameter As Parameter

For Each oDrivenByParameter In oParameter.DrivenBy

If InStr(oDrivenByParameter.Name, PrefixStr) = 0 Then

oGeneralDimension.Delete

End If

Else

If InStr(oParameter.Name, PrefixStr) = 0 Then

oGeneralDimension.Delete

End If

“End Code

I hoop it was use full.

Best regards,

Re: Retrieve dimensions

Anonymous — Wed, 10 Oct 2012 20:18:44 GMT

Wow!!! That is the great code!!!!

Thank you so much!!!

Re: Retrieve dimensions

theo_bot — Thu, 11 Oct 2012 08:39:54 GMT

Marco,

Thanks, it works great!!

Houdoe,

gr Theo

Re: Retrieve dimensions

skyngu — Thu, 11 Oct 2012 12:17:45 GMT

will this rule delete dimensions by hole features?

it seems not going to work at that way.

thanks.

Re: Retrieve dimensions

xiaodong_liang — Tue, 16 Oct 2012 10:11:28 GMT

I'd suggest you provide a dataset to recreate the problem you met with. This will help the peers here to diagnose.

Re: Retrieve dimensions

skyngu — Tue, 16 Oct 2012 12:06:50 GMT

HI,

please check attachment. there will be an error when run ilogic rule.

the dimension by hole feature is not going to work.

it is 1/4--20 hole. the diameter of tap drill hole casues the error.

thanks a lot.

Re: Retrieve dimensions

marco_suurlant — Tue, 16 Oct 2012 14:17:42 GMT

Hi,

You were right the code stopped working because the Tapped Hole has no RetrievedFrom.Parameter.

Here you have the modified code.

Start code”

Dim oDrawDoc As DrawingDocument = ThisDoc.Document

Dim oSheet As Sheet = oDrawDoc.ActiveSheet

Dim oDrawView As DrawingView = oSheet.DrawingViews(1)

Dim oGeneralDimensionsEnum As GeneralDimensionsEnumerator
oGeneralDimensionsEnum = oSheet.DrawingDimensions.GeneralDimensions.Retrieve(oDrawView)

Dim oGeneralDimension As GeneralDimension
For Each oGeneralDimension In oGeneralDimensionsEnum
	Dim oParameter As Parameter

	Try
		oParameter = oGeneralDimension.RetrievedFrom.Parameter
	Catch
		' Error to set oParameter.
		' Go further to delete the dimension.
	End Try

    If oParameter.DrivenBy.count <> 0 Then
        Dim oDrivenByParameter As Parameter
        For Each oDrivenByParameter In oParameter.DrivenBy
            If InStr(oDrivenByParameter.Name, "RetD_") = 0 Then
                oGeneralDimension.Delete
            End If
        Next
    Else
        oGeneralDimension.Delete
    End If
Next

“End Code

I didn’t test it with your Part because I have now only version 2011.

Best regards,

Re: Retrieve dimensions

skyngu — Tue, 16 Oct 2012 17:18:04 GMT

hi,

at the near end of your code, you miss some parts. it should be like this,

If InStr(oParameter.Name, "test_") = 0 Then

oGeneralDimension.Delete
End If

otherwise, the code will delete all dimensions.

thanks for your information.

Re: Retrieve dimensions

marco_suurlant — Tue, 16 Oct 2012 17:46:03 GMT

Hi,

Something like this:

Dim oDrawDoc As DrawingDocument = ThisDoc.Document

Dim oSheet As Sheet = oDrawDoc.ActiveSheet

Dim oDrawView As DrawingView = oSheet.DrawingViews(1)

Dim oGeneralDimensionsEnum As GeneralDimensionsEnumerator
oGeneralDimensionsEnum = oSheet.DrawingDimensions.GeneralDimensions.Retrieve(oDrawView)

Dim PrefixStr As String = "RetD_"

Dim oGeneralDimension As GeneralDimension
For Each oGeneralDimension In oGeneralDimensionsEnum
    Dim oParameter As Parameter
	Try
		oParameter = oGeneralDimension.RetrievedFrom.Parameter
	Catch
		' Error to set oParameter.
		' Go further to delete the dimension.
	End Try

    If oParameter.DrivenBy.count <> 0 Then
        Dim oDrivenByParameter As Parameter
        For Each oDrivenByParameter In oParameter.DrivenBy
            If InStr(oDrivenByParameter.Name, PrefixStr) = 0 Then
                oGeneralDimension.Delete
            End If
        Next
	Else
        If InStr(oParameter.Name, PrefixStr) = 0 Then
            oGeneralDimension.Delete
        End If
    End If
Next

Re: Retrieve dimensions

Anonymous — Tue, 16 Oct 2012 20:03:27 GMT

Guys,

What if I have 3 views and I need to dimension OAL length on the front view, OAL width on the side view, and lets say a hole on the top view. How to modify the code. I tried to play with it, copiyng the part of the code and changing the view name, but it gives me an error.

Thanks in advance.

Re: Retrieve dimensions

marco_suurlant — Wed, 17 Oct 2012 09:39:22 GMT

Hi,

Here you have some code that can do that, only thing what you must have do is give the Drawing View a name and give the user / model parameter the right name.

Sub Main
    Dim oDrawDoc As DrawingDocument = ThisDoc.Document
    Dim oSheet As Sheet = oDrawDoc.ActiveSheet
    RetrieveDimByView(oSheet, "FrontView", "RetD_")
    RetrieveDimByView(oSheet, "RightView", "RetDRight_")
    RetrieveDimByView(oSheet, "TopView", "RetDTop_")
End Sub

Sub RetrieveDimByView(ByVal oSheet As Sheet, ByVal ViewName As String, ByVal PrefixStr As String)
    Dim oDrawView As DrawingView
    For Each oDrawView In oSheet.DrawingViews
        If oDrawView.Name = ViewName Then
            Exit For
        End If
    Next
    Dim oGeneralDimensionsEnum As GeneralDimensionsEnumerator
    oGeneralDimensionsEnum = oSheet.DrawingDimensions.GeneralDimensions.Retrieve(oDrawView)
    Dim oGeneralDimension As GeneralDimension
    For Each oGeneralDimension In oGeneralDimensionsEnum
        Dim oParameter As Parameter
        Try
            oParameter = oGeneralDimension.RetrievedFrom.Parameter
        Catch
            ' Error to set oParameter.
            ' Go further to delete the dimension.
        End Try
        If oParameter.DrivenBy.count <> 0 Then
            Dim oDrivenByParameter As Parameter
            For Each oDrivenByParameter In oParameter.DrivenBy
                If InStr(oDrivenByParameter.Name, PrefixStr) = 0 Then
                    oGeneralDimension.Delete
                End If
            Next
        Else
            If InStr(oParameter.Name, PrefixStr) = 0 Then
                oGeneralDimension.Delete
            End If
        End If
    Next
    oSheet = Nothing
End Sub

Re: Retrieve dimensions

Anonymous — Fri, 19 Oct 2012 15:50:10 GMT

Excellent works just great.

One more question, is there any chance to offset the dimensions?

Thanks,

Re: Retrieve dimensions

theo_bot — Mon, 22 Oct 2012 09:46:52 GMT

Hi Marco,

It works fine, but my model is based on a multi body part.

So if i retrieve the dimensions, i get the dimensions from every part from my assembly.

in the standard interface, i can select a part thats part of the view, how can i do this thru the api?

the API help tells me that you can use a "demensionToRetrive":

Sub Retrieve(ViewOrSketch As IDispatch, ByRef DimensionsToRetrieve As [optional] VARIANT, Result As [out, retval] GeneralDimensionsEnumerator*)

I've tried some to create a ObjectCollection with the specific part, but i doesn't seem to work. Do you have any suggestion.

Kind regards,

Theo

Re: Retrieve dimensions

marco_suurlant — Mon, 22 Oct 2012 16:51:28 GMT

Hello achmidt,

What you can do is select all dimension and then arrange dimensions.

Start code"

    Dim oCommandMgr As CommandManager = _
    ThisApplication.CommandManager

    oCommandMgr.ControlDefinitions.item("DrawingSelectAllInventorDimsCmd").Execute
    oCommandMgr.ControlDefinitions.item("DrawingArrangeDimensionsCmd").Execute

"End code

Best regards,

Re: Retrieve dimensions

marco_suurlant — Tue, 23 Oct 2012 07:33:15 GMT

Hello Theo,

If you want to make a collection of a Part you can do something like this,

Dim oAssemblyDocument As Inventor.AssemblyDocument = _
	oDrawView.ReferencedDocumentDescriptor.ReferencedDocument

Dim oOcc As Inventor.ComponentOccurrence = _
	oAssemblyDocument.ComponentDefinition.occurrences.item(1)

Dim oGeneralDimensionsObj As ObjectCollection = _
	oSheet.DrawingDimensions.GeneralDimensions.GetRetrievableDimensions(oDrawView, oOcc)

The oGeneralDimensionsObj has now the retrieved dimensions form the first Part.

Best regards,

Re: Retrieve dimensions

Anonymous — Thu, 01 Nov 2012 20:03:01 GMT

Thanks!!!

Re: Retrieve dimensions

Anonymous — Fri, 02 Nov 2012 13:57:23 GMT

I`d like to share the code I assembled from different pieces (see attached). Configurator works great but I have few problems with the drawing dimensions.

I`m not sure how to place flat pattern OAL dim`s, can`t place bend dim`s, not sure how to modify flat pattern placement code so it shows bend extents.

oView4 = oSheet.DrawingViews.AddBaseView(oPartDoc,oPoint4, ViewScale,kDefaultViewOrientation, kHiddenLineDrawingViewStyle,,, oBaseViewOptions)

Also I`m not sure how to do ordinate dim`s for the holes (horizontal & vertical).

If you`d like to test it out don`t forget to change the template path and name in the code.

I have an external rule that I run after drawing creation (see below), it places the dimensions I need.

Sub Main
    Dim oDrawDoc As DrawingDocument = ThisDoc.Document
    Dim oSheet As Sheet = oDrawDoc.ActiveSheet
    RetrieveDimByView(oSheet, "VIEW1", "Fr_") ' front view
    RetrieveDimByView(oSheet, "VIEW3", "Rs_") ' right side view
	RetrieveDimByView(oSheet, "VIEW2", "Tv_") ' top view
    'RetrieveDimByView(oSheet, "View3", "RetDTop_")
End Sub

Sub RetrieveDimByView(ByVal oSheet As Sheet, ByVal ViewName As String, ByVal PrefixStr As String)
    Dim oDrawView As DrawingView
    For Each oDrawView In oSheet.DrawingViews
        If oDrawView.Name = ViewName Then
            Exit For
        End If
    Next
    Dim oGeneralDimensionsEnum As GeneralDimensionsEnumerator
    oGeneralDimensionsEnum = oSheet.DrawingDimensions.GeneralDimensions.Retrieve(oDrawView)
    Dim oGeneralDimension As GeneralDimension
    For Each oGeneralDimension In oGeneralDimensionsEnum
        Dim oParameter As Parameter
        Try
            oParameter = oGeneralDimension.RetrievedFrom.Parameter
        Catch
            ' Error to set oParameter.
            ' Go further to delete the dimension.
        End Try
        If oParameter.DrivenBy.count <> 0 Then
            Dim oDrivenByParameter As Parameter
            For Each oDrivenByParameter In oParameter.DrivenBy
                If InStr(oDrivenByParameter.Name, PrefixStr) = 0 Then
                    oGeneralDimension.Delete
                End If
            Next
        Else
            If InStr(oParameter.Name, PrefixStr) = 0 Then
                oGeneralDimension.Delete
            End If
        End If
    Next
    oSheet = Nothing
	
	
	Dim oCommandMgr As CommandManager = _
    ThisApplication.CommandManager

    oCommandMgr.ControlDefinitions.item("DrawingSelectAllInventorDimsCmd").Execute
    oCommandMgr.ControlDefinitions.item("DrawingArrangeDimensionsCmd").Execute
	
End Sub

Would be great to add a code that automatically scales up/down the views and places them on the sheet.

Any help appreciated. Thanks,

Re: Retrieve dimensions

Anonymous — Mon, 21 Jul 2014 09:40:09 GMT

The Following code suggested by you is performing the necessary action but ends with "Unexpected error".

Also it is retrieving the dimension without the special characters like "RteD_". Please guide me.

Dim oDrawDoc As DrawingDocument = ThisDoc.Document

Dim oSheet As Sheet = oDrawDoc.ActiveSheet

Dim oDrawView As DrawingView = oSheet.DrawingViews(1)

Dim oGeneralDimensionsEnum As GeneralDimensionsEnumerator
oGeneralDimensionsEnum = oSheet.DrawingDimensions.GeneralDimensions.Retrieve(oDrawView)

Dim PrefixStr As String = "RetD_"

Dim oGeneralDimension As GeneralDimension
For Each oGeneralDimension In oGeneralDimensionsEnum
    Dim oParameter As Parameter
Try
oParameter = oGeneralDimension.RetrievedFrom.Parameter
Catch
' Error to set oParameter.
' Go further to delete the dimension.
End Try

    If oParameter.DrivenBy.count <> 0 Then
        Dim oDrivenByParameter As Parameter
        For Each oDrivenByParameter In oParameter.DrivenBy
            If InStr(oDrivenByParameter.Name, PrefixStr) = 0 Then
                oGeneralDimension.Delete
            End If
        Next
Else
        If InStr(oParameter.Name, PrefixStr) = 0 Then
            oGeneralDimension.Delete
        End If
    End If
Next

Re: Retrieve dimensions

marco_suurlant — Tue, 22 Jul 2014 08:59:26 GMT

Hello,

I have tested the code on my side and it is working, the test part is included.

If it is still not working can you include the part.

Best regards,

Marco