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How to Add Dimension to sketch without the user prompt

Question asked by Jared Ticotin on Jun 17, 2020
Latest reply on Jun 17, 2020 by Jared Ticotin

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I have this simple code that was generated from record macro:

Dim swApp As Object
Dim Part As Object
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long
Sub main()
Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
boolstatus = Part.Extension.SelectByID2("Arc1", "SKETCHSEGMENT", 3.7150296065182E-03, 2.27937040626695E-02, 0.271824680271828, False, 0, Nothing, 0)
Dim myDisplayDim As Object
Set myDisplayDim = Part.AddDimension2(2.92954224961134E-02, -9.04798883599746E-03, 0.338308576024644)
Part.ClearSelection2 True
Dim myDimension As Object
Set myDimension = Part.Parameter("D1@Sketch3")
myDimension.SystemValue = 0.00635
End Sub

When I run this, I get a popup which requires the user to click "ok" to close, then it sets it's value. How can I add a dimension to a circle in a sketch without this popup? Or at least in a way that doesn't require the user to do anything?

Jared Ticotin Jun 17, 2020 2:11 PM

Correct Answer

This put me on the right track. For anyone interested, I had to do this:

Option Explicit
Sub main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDisplayDim As SldWorks.DisplayDimension
Dim swDim As SldWorks.Dimension
Dim boolstatus As Boolean
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False
boolstatus = swModel.Extension.SelectByID2("Arc1", "SKETCHSEGMENT", 3.7150296065182E-03, 2.27937040626695E-02, 0.271824680271828, False, 0, Nothing, 0)
Set swDisplayDim = swModel.AddDimension2(2.92954224961134E-02, -9.04798883599746E-03, 0.338308576024644)
Set swDim = swModel.Parameter(swDisplayDim.GetNameForSelection)
swDim.SystemValue = 0.00635
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, True
End Sub

I put in bold the important lines that were needed which macro record doesn't generate.

Thanks for the help.

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Josh Brady Jun 17, 2020 9:47 AM

Please read the Remarks section

2016 SOLIDWORKS API Help - AddDimension2 Method (IModelDoc2)

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Fifi Riri Jun 17, 2020 11:24 AM

Hello. Try this:

Option Explicit
Sub main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDisplayDim As SldWorks.DisplayDimension
Dim swDim As SldWorks.Dimension
Dim boolstatus As Boolean
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False
boolstatus = swModel.Extension.SelectByID2("Arc1", "SKETCHSEGMENT", 3.7150296065182E-03, 2.27937040626695E-02, 0.271824680271828, False, 0, Nothing, 0)
Set swDisplayDim = swModel.AddDimension2(2.92954224961134E-02, -9.04798883599746E-03, 0.338308576024644)
Set swDim = swDisplayDim.GetDimension
swDim.SystemValue = 0.00635
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, True
End Sub

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Jared Ticotin @ Fifi Riri on Jun 17, 2020 2:11 PM

This put me on the right track. For anyone interested, I had to do this:

Option Explicit
Sub main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDisplayDim As SldWorks.DisplayDimension
Dim swDim As SldWorks.Dimension
Dim boolstatus As Boolean
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False
boolstatus = swModel.Extension.SelectByID2("Arc1", "SKETCHSEGMENT", 3.7150296065182E-03, 2.27937040626695E-02, 0.271824680271828, False, 0, Nothing, 0)
Set swDisplayDim = swModel.AddDimension2(2.92954224961134E-02, -9.04798883599746E-03, 0.338308576024644)
Set swDim = swModel.Parameter(swDisplayDim.GetNameForSelection)
swDim.SystemValue = 0.00635
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, True
End Sub

I put in bold the important lines that were needed which macro record doesn't generate.

Thanks for the help.

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Josh Brady @ Jared Ticotin on Jun 17, 2020 2:22 PM

Jared Ticotin wrote:

Set swDim = swModel.Parameter(swDisplayDim.GetNameForSelection)

This is like asking your neighbor to ship you a package via UPS.

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Jared Ticotin @ Josh Brady on Jun 17, 2020 3:34 PM

I did not realize this would take longer. I tried it using Fifi's code but I kept getting an error on this line:

Set swDim = swDisplayDim.GetDimension

Honestly my script works really fast though. If there's any difference it is probably a fraction of a second and not noticeable.

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5 Replies

Josh Brady Jun 17, 2020 9:47 AM
Mark Correct
Correct Answer
Please read the Remarks section

2016 SOLIDWORKS API Help - AddDimension2 Method (IModelDoc2)
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Fifi Riri Jun 17, 2020 11:24 AM
Mark Correct
Correct Answer
Hello. Try this:
Option Explicit
Sub main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDisplayDim As SldWorks.DisplayDimension
Dim swDim As SldWorks.Dimension
Dim boolstatus As Boolean
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False
boolstatus = swModel.Extension.SelectByID2("Arc1", "SKETCHSEGMENT", 3.7150296065182E-03, 2.27937040626695E-02, 0.271824680271828, False, 0, Nothing, 0)
Set swDisplayDim = swModel.AddDimension2(2.92954224961134E-02, -9.04798883599746E-03, 0.338308576024644)
Set swDim = swDisplayDim.GetDimension
swDim.SystemValue = 0.00635
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, True
End Sub
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- Jared Ticotin @ Fifi Riri on Jun 17, 2020 2:11 PM
  Unmark Correct
  Correct Answer
  This put me on the right track. For anyone interested, I had to do this:
  Option Explicit
  Sub main()
  Dim swApp As SldWorks.SldWorks
  Dim swModel As SldWorks.ModelDoc2
  Dim swDisplayDim As SldWorks.DisplayDimension
  Dim swDim As SldWorks.Dimension
  Dim boolstatus As Boolean
  Set swApp = Application.SldWorks
  Set swModel = swApp.ActiveDoc
  swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False
  boolstatus = swModel.Extension.SelectByID2("Arc1", "SKETCHSEGMENT", 3.7150296065182E-03, 2.27937040626695E-02, 0.271824680271828, False, 0, Nothing, 0)
  Set swDisplayDim = swModel.AddDimension2(2.92954224961134E-02, -9.04798883599746E-03, 0.338308576024644)
  Set swDim = swModel.Parameter(swDisplayDim.GetNameForSelection)
  swDim.SystemValue = 0.00635
  swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, True
  End Sub
  I put in bold the important lines that were needed which macro record doesn't generate.
  Thanks for the help.
  Like • Show 0 Likes0
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  - Josh Brady @ Jared Ticotin on Jun 17, 2020 2:22 PM
    Mark Correct
    Correct Answer
    Jared Ticotin wrote:
    
    Set swDim = swModel.Parameter(swDisplayDim.GetNameForSelection)
    This is like asking your neighbor to ship you a package via UPS.
    Like • Show 1 Like1
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    - Jared Ticotin @ Josh Brady on Jun 17, 2020 3:34 PM
      Mark Correct
      Correct Answer
      I did not realize this would take longer. I tried it using Fifi's code but I kept getting an error on this line:
      Set swDim = swDisplayDim.GetDimension
      Honestly my script works really fast though. If there's any difference it is probably a fraction of a second and not noticeable.
      Like • Show 0 Likes0
      Actions

How to Add Dimension to sketch without the user prompt

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