Solved: Create Dimension between two points in idw - Page 2

iogurt1 · ‎01-04-2016

I am slowly getting into drawing automation with iLogic and I've already learned a lot just watching the video on http://www.symetri.co.uk/blog/details/automating-dimensions-with-ilogic

I copied their iLogic code to try it for myself and creating a linear dimension between two faces works great.

I also got the code to work if I want to place a diameter on a round object

What I am now struggling with, is to create a linear dimension between two work points that are set to "include" in the idw. I think it has something do with with the way I am defining the work points. For the faces, the code snippet that defines the edges looks like this:

'finds edges with a particular attributes then taks the first instance
Dim aoEdge3 as face
oObjs = oAssyDoc.AttributeManager.FindObjects("DIM", "RHS", "1")
aoEdge3 = oObjs.Item(1)

'Finds the drawing edge that represents the one with the attribute
Dim aoDrawCurves4 As DrawingCurve
oDrawViewCurves = oView.DrawingCurves(aoEdge4)
aoDrawCurves4 = oDrawViewCurves.Item(1)

What I don't know, is how to define the work points. I tried to define the aoDrawCurves4 As Point2d but that didn't work.

Any help is appreciated.

iogurt1 · ‎09-09-2016

Hey there. No worries, keep asking if you're stuck. I've had tons of help when I first got into it, just paying it forward. In a few months you'll be answering questions from people getting into drawing automation 🙂

As for the text on a new line I had to google it myself as well. All these codes are pretty much standard VBA codes, stuff that also works in excel and other applications. I found this: http://www.mrexcel.com/forum/excel-questions/66757-visual-basic-applications-code-creating-multiple-...

So it looks like your code would be

oDimText.FormattedText = "<DimensionValue/>" & vbLf & "Top Plate"

Anonymous · ‎09-13-2016

So with your help and learning more about iLogic I came up with this.... It changes the dimensions to our customer layer but I want the style to be put into inches, because it is on in mm now. Please help!

Format:HTML Format Version:1.0 StartHTML: 165 EndHTML: 9661 StartFragment: 314 EndFragment: 9629 StartSelection: 314 EndSelection: 314SyntaxEditor Code Snippet

ActiveSheet = ThisDrawing.Sheet("Sheet:1")

'References this document
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisDoc.Document

'References this drawing sheet
Dim oSheet As Sheet
oSheet = oDrawDoc.ActiveSheet

Dim oDim as DrawingDimension
Dim oDimStyle As DrawingStylesManager = oDrawDoc.StylesManager
For Each oDim In oSheet.DrawingDimensions
    If oDim.AttributeSets.Nameisused("iLogic_Created") = True Then
    oDim.Layer = ThisDrawing.Document.StylesManager.Layers("Customer")
    End If
    
Dim oStylesMgr As DrawingStylesManager = oDrawDoc.StylesManager
    
If oDimStyle = "Customer" Then
oDimStyle = ThisDrawing.Document.oStylesMgr.DimensionStyles.Item("KG-in")
    
End If

Next

Dim ODDoc as Inventor.Document
ODDoc=ThisApplication.ActiveDocument

ODDoc.AttributeManager.PurgeAttributeSets

iogurt1 · ‎09-13-2016

Without testing it myself, I think the problem is that the dimensions are assigned to a layer

oDim.Layer = ThisDrawing.Document.StylesManager.Layers("Customer")

and further down you call for

If oDimStyle = "Customer" Then

But oDimStyle is dimensioned as

DrawingStylesManager = oDrawDoc.StylesManager

and not a layer.

I'm not sure if you need your dimensions to be on a layer for future code but I've never done that myself. I assign my dimensions a new style, depending on what they were created as (most of them will be created as "By Standard (your dimstyle)". I usually create two rules, one called "MetricToImperial" and another called "ImperialToMetric"and run one or the other, depending on the units the customer wants to see:

SyntaxEditor Code Snippet

'---INITIAL SETUP---'References this document
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisDoc.Document

'Runs these rules on all sheets, instead of just the active sheet.
For Each oSheet In oDrawDoc.Sheets

'Reference the Styles Manager
Dim oStylesMgr As DrawingStylesManager
oStylesMgr = oDrawDoc.StylesManager

'get the reference to the target dimension style (by name)
Dim oDimStyle As DimensionStyle
oDimStyle = oStylesMgr.DimensionStyles.Item("OurDimStyle1")

'get the reference to the target dimension style (by name) for hole notes
Dim oDimStyleHoles As DimensionStyle
oDimStyleHoles = oStylesMgr.DimensionStyles.Item("OurDimStyle2")

'Reference the Dimensions
Dim oDims As DrawingDimensions
oDims = oSheet.DrawingDimensions

'Reference Linear Dimensions
Dim oLinearDim As GeneralDimension

'Reference Ordinate Dimensions
Dim oOrdDim As OrdinateDimension

'---CHANGE DIMENSIONS---'change Linear dimensions (not including Angular dims)
For Each oLinearDim In oDims.GeneralDimensions
    If TypeOf oLinearDim Is LinearGeneralDimension Then
        oLinearDim.Style = oDimStyle
    End If
Next

'change Ordinate dimensions
For Each oOrdDim In oDims.OrdinateDimensions
oOrdDim.Style = oDimStyle
Next

'change Hole and Thread Notes
Dim oThreadNote As HoleThreadNote
For Each oThreadNote In oSheet.DrawingNotes.HoleThreadNotes
oThreadNote.Style = oDimStyleHoles
Next
Next 'sheet

iLogicVb.UpdateWhenDone = True

Anonymous · ‎09-13-2016

So the issue is we have Shop level and customer level drawings, the shop level has dimensions on the shop layer and are in MM while the customer level dimensions are on the customer layer and need to be in IN, So I can the dimensions to go from customer to Shop layers but I can't get the dimensions to go into IN. 😞

iogurt1 · ‎09-13-2016

Oh I see. Interesting concept 🙂

Ok just guessing here again but try to change the line

If oDimStyle = "Customer" Then

to

If oDim.Layer = "Customer" Then

See if that works...

Anonymous · ‎09-13-2016

I changed that, It give me this error though....

Anonymous · ‎09-13-2016

And yes, Interesting but a pain in the butt hahaha

iogurt1 · ‎09-13-2016

So I got it to work with the below code. Instead of applying the layer to dimensions that have the attribute "iLogic_Created" and then further down look for

If oDimStyle = "Customer" Then

I do everything at the same time. Let me know if this works or not:

SyntaxEditor Code Snippet

'---INITIAL SETUP---'On Error Resume Next 'Instead of showing errors, the code will finish all the items it can

'References this document
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisDoc.Document

'Runs these rules on all sheets, instead of just the active sheet.
For Each oSheet In oDrawDoc.Sheets

'Reference the Styles Manager
Dim oStylesMgr As DrawingStylesManager
oStylesMgr = oDrawDoc.StylesManager

'get the reference to the target dimension style (by name)
Dim oDimStyle1 As DimensionStyle
oDimStyle1 = oStylesMgr.DimensionStyles.Item("YourDimStyle1")

'get the reference to the target dimension style (by name) for hole notes
Dim oDimStyle2 As DimensionStyle
oDimStyle2 = oStylesMgr.DimensionStyles.Item("YourDimStyle2")

'Reference the Dimensions
Dim oDims As DrawingDimensions
oDims = oSheet.DrawingDimensions

'Reference Linear Dimensions
Dim oLinearDim As GeneralDimension

'---CHANGE DIMENSIONS---
For Each oLinearDim In oDims.GeneralDimensions
    If TypeOf oLinearDim Is LinearGeneralDimension Then
              oLinearDim.Style = oDimStyle1
    End If
    If oLinearDim.AttributeSets.Nameisused("iLogic_Created") Then
       oLinearDim.Layer = ThisDrawing.Document.StylesManager.Layers("Border (ANSI)")
       oLinearDim.Style = oDimStyle2
    End If
Next
Next 'sheet
iLogicVb.UpdateWhenDone = True

Anonymous · ‎09-13-2016

You sir are a life saver!! 😄

Anonymous · ‎09-20-2016

Have you ever done anything with turning off/on work points in drawing views based on specific parameters?

iogurt1 · ‎09-20-2016

I actually haven't. I'm assuming you mean the visibility of the "included" work points that get turned into Centermarks?

But I just tried it and you could do something like this:

marks(3) = oSheet.Centermarks.AddByWorkFeature(WorkPoint4, oView)
If oPartDoc.ComponentDefinition.Parameters.Item("YourParameter").Value = "True" Then
marks(3).Visible = True
Else
marks(3).Visible = False
End If

or if your parameter is not a true/false, just fill in the value.

Anonymous · ‎09-26-2016

I have a huge favor to ask... All of my code works perfectly thank you! My only issue is that the size of my views change obviously the scaling of them aren't controlling it well enough. So I was wondering if there is a way to say no matter what have the views set to a certain size and so all of my dimensions and view labels won't jump.

iogurt1 · ‎09-26-2016

I am using this on pretty much all my drawings: http://adndevblog.typepad.com/manufacturing/2014/11/set-drawing-view-width.html

And then just put something like "Not to scale" in your title block.

Also check this out, might be helpful: http://forums.autodesk.com/t5/inventor-forum/dimension-text-position-as-dimension-changes/td-p/59797...

Anonymous · ‎09-26-2016

You normally select the view manually too?

iogurt1 · ‎09-26-2016

Oh I see, this code is still with the selecting of the view. No, I changed mine and it looks like this:

'---INITIAL SETUP---
Dim oFront As DrawingView
oFront = ActiveSheet.View("FRONT").View

'---FRONT VIEW SIZE---

' Current width
Dim oCurrentFront As Double
oCurrentFront = oFront.Width

' New width we want (set in cm)
Dim oNewFront As Double
oNewFront = 14

' New scale
Dim oScaleFront As Double
oScaleFront = oNewFront / oCurrentFront * oFront.Scale

oFront.[Scale] = oScaleFront

'---VIEW POSITIONS---
'distances are in inches, not cm (because the sheet is defined in inches)
ActiveSheet.View("FRONT").SetSpacingToCorner(5.375 , 1.75, SheetCorner.TopLeft)

The bottom part is pretty sweet. you can lock down your views on the sheet so they are always in the same spot.

Anonymous · ‎09-26-2016

Ok, Yeah I re-wrote mine too haha I just didn't know if you were just manually using yours. 🙂

Anonymous · ‎09-26-2016

So this is my issue. I am using the iLogic attribute dims as well as the view code as well.

The dimensions still "jump" I don't know why exactly.... Is it because of the scale?

iogurt1 · ‎09-26-2016

Can you place the dimensions after the views have been scaled? Not sure how to fix this issue otherwise...

I usually run a "reset" rule that runs my different rules in order. First is the scaling and positioning of the views, and then add the dimensions and sort the BOM and stuff like that. Maybe that would help you as well? Just list them with

iLogicVb.RunRule(“ruleName1”)

iLogicVb.RunRule(“ruleName2”)

iLogicVb.RunRule(“ruleName3”)

Anonymous · ‎09-30-2016

First, thank you for all of your help its been great!!

Now, I have something that will be interesting to do.... 😛

I would like to have the project file to be shown after the question Ex: 123456789.ipj (or something along that line)

Also, if no was to be pressed I would like a browser to show up that would allow the user to manually map the file location.

Any ideas!?

I have the code stated below:

Sub Main iLogicVb.RunRule("CustOn")

'query user
MessageBox.Show("Would you like to print to the current Project File?: ", "iLogic Question",MessageBoxButtons.YesNo,MessageBoxIcon.Question)
'set condition based on answer
If question = vbYes Then
    oFileName = ThisDoc.FileName(False) 'without extension
    oRevNum = iProperties.Value("Project", "Revision Number")

    Else

    End If



    ' Get the PDF translator Add-In.
    Dim PDFAddIn As TranslatorAddIn
    PDFAddIn = ThisApplication.ApplicationAddIns.ItemById _
                            ("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}")

    'Set a reference to the active document (the document to be published).
    Dim oDocument As Document
    oDocument = ThisApplication.ActiveDocument
     Dim oContext As TranslationContext
    oContext = ThisApplication.TransientObjects.CreateTranslationContext
    oContext.Type = kFileBrowseIOMechanism
    'Create a NameValueMap object
    Dim oOptions As NameValueMap
     oOptions = ThisApplication.TransientObjects.CreateNameValueMap
    ' Create a DataMedium object
    Dim oDataMedium As DataMedium
    oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
    ' Check whether the translator has 'SaveCopyAs' options
    If PDFAddIn.HasSaveCopyAsOptions(oDocument, oContext, oOptions) Then

        ' Options for drawings...
        'oOptions.Value("Launch_Viewer") = launchviewer
        oOptions.Value("All_Color_AS_Black") = 1
        'oOptions.Value("Sheet_Range") = ThisApplication.PrintRangeEnum.kPrintAllSheets
        oOptions.Value("Sheet_Range") = Inventor.PrintRangeEnum.kPrintAllSheets

        'oOptions.Value("Remove_Line_Weights") = 0
        'oOptions.Value("Vector_Resolution") = 400

        'oOptions.Value("Custom_Begin_Sheet") = 2
        'oOptions.Value("Custom_End_Sheet") = 4
    End If
    'get PDF target folder path
    oFolder = Left(ThisDoc.Path, InStrRev(oPath, "\")) & "PDF"
    'Check for the PDF folder and create it if it does not exist
        If Not System.IO.Directory.Exists(oFolder) Then
            System.IO.Directory.CreateDirectory(oFolder)
        End If

     'Set the PDF target file name
    Dim fname As String
    fname = oFolder & "\" & oFileName & " Rev" & oRevNum & "-CUST.pdf"
    oDataMedium.FileName = fname
    'Publish document.
    If System.IO.Directory.Exists(fname) Then
        System.IO.File.Delete(fname)
        MessageBox.Show("Earlier PDF deleted! ", "Inventor")
    End If
    PDFAddIn.SaveCopyAs(oDocument, oContext, oOptions, oDataMedium)
    MessageBox.Show("Print Created in default Projects - " & fname, "Inventor")

End Sub

iogurt1 · ‎09-30-2016

Hmm I've never done anything like this. Maybe you can find something on the forums. If not I'd suggest making a post in this forum.

Sorry, no help this time

If you do figure it out, I'd be interested in the solution as well as this might have a useful application for me in the future

Create Dimension between two points in idw

Create Dimension between two points in idw

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