Layer setting checklist for drawing file

Submitted by policep on Tue, 01/09/2018 - 03:30
Forums: 
Journaling / NXOpen API

Hi All

I am working on layer setting checklist for drawing file

User will run the macro,macro has to move the objects as per below mentioned requirements

datum feature = should be in 100th layer
balloon feature = should be in 101 layer
datum target = should be in 102 layer
surface symbol = should be in 103 layer
welding symbol = should be in 104 layer

I did for sketches and fcfs & notes its working fine
please support on other objects mentioned in above.

Thank you
Reagrds
patil

policep - Thu, 01/11/2018 - 23:16

Please any support on this

Below code for notes

foreach (Note note in workPart.Notes)
{
DisplayableObject[] objects1 = new DisplayableObject[1];
objects1[0] = note;
DisplayModification displayModification1;
displayModification1 =
theSession.DisplayManager.NewDisplayModification();
displayModification1.NewLayer = 242;
displayModification1.Apply(objects1);
displayModification1.Dispose();
}

Thank you
Reagrds
Patil

NXJournaling - Fri, 01/12/2018 - 06:31

The code below shows how to access the other object types.

Option Strict Off
Imports System
Imports NXOpen
Imports NXOpen.UF

Module Module1

Dim theSession As Session = Session.GetSession()
Dim theUfSession As UFSession = UFSession.GetUFSession()

Dim theUI As UI = UI.GetUI()
Dim lw As ListingWindow = theSession.ListingWindow

Sub Main()

Dim markId1 As Session.UndoMarkId
markId1 = theSession.SetUndoMark(Session.MarkVisibility.Visible, "NXJ")

lw.Open()

lw.WriteLine("number of datums: " & theSession.Parts.Work.Annotations.Datums.ToArray.Length.ToString)

lw.WriteLine("number of datum targets: " & theSession.Parts.Work.Annotations.DatumTargets.ToArray.Length.ToString)

lw.WriteLine("number of drafting datum targets: " & theSession.Parts.Work.Annotations.DraftingDatumTargets.ToArray.Length.ToString)

lw.WriteLine("number of feature control frames: " & theSession.Parts.Work.Annotations.Fcfs.ToArray.Length.ToString)

lw.WriteLine("number of GDT's: " & theSession.Parts.Work.Gdts.ToArray.Length.ToString)
For Each temp As NXObject In theSession.Parts.Work.Gdts
lw.WriteLine(" type: " & temp.GetType.ToString)
Next

lw.WriteLine("number of ID symbols: " & theSession.Parts.Work.Annotations.IdSymbols.ToArray.Length.ToString)

lw.WriteLine("number of surface finish symbols: " & theSession.Parts.Work.Annotations.DraftingSurfaceFinishSymbols.ToArray.Length.ToString)

lw.WriteLine("number of weld symbols: " & theSession.Parts.Work.Annotations.Welds.ToArray.Length.ToString)

lw.Close()

End Sub

Public Function GetUnloadOption(ByVal dummy As String) As Integer

'Unloads the image immediately after execution within NX
GetUnloadOption = NXOpen.Session.LibraryUnloadOption.Immediately

End Function

End Module

Also note that the display modification object's .Apply method will accept an array of objects, so you could simplify your code as below:


DisplayModification displayModification1;
displayModification1 =
theSession.DisplayManager.NewDisplayModification();
displayModification1.NewLayer = 242;
displayModification1.Apply(workPart.Notes.ToArray);
displayModification1.Dispose();

policep - Fri, 01/12/2018 - 09:25

Thanks for your support

policep - Fri, 01/12/2018 - 10:26

Hello Experts

Please support on this

All manual edited dimensions should be in 108 layer & manual edited dimensions are in yellow colour.

Thank you

NXJournaling - Fri, 01/12/2018 - 10:34

The code at the following link will find manual dimensions; it writes some info to the listing window, but you can modify it to do as you like.

http://nxjournaling.com/content/report-dimensions-manual-text

policep - Fri, 01/12/2018 - 10:35

Thank you