When run, the following script will change the color of the face of simple holes to blue (color 211), and threaded holes to yellow (color 6). The journal has been tested with NX 7.5.
Imports System
Imports NXOpen
Imports NXOpen.UF
Imports NXOpen.Features
Module HoleColours
Sub Main()
Dim s As Session = Session.GetSession()
Dim ufs As UFSession = UFSession.GetUFSession()
Dim dp As Part = s.Parts.Work
Dim expstring As String = Nothing
Dim index2 As Integer = -1
Dim exps() As Expression
Dim holewiththread As Boolean = False
Dim holeexpstring As String = "Threaded"
Dim hole As BodyFeature
Dim faces() As Face
Dim nFaces As Integer = 0
Dim obj(-1) As DisplayableObject
Dim displayModification1 As DisplayModification
Dim featcoll As FeatureCollection = dp.Features
For Each f As Feature In featcoll
If f.FeatureType = "SIMPLE HOLE" Then
holewiththread = False
exps = f.GetExpressions()
index2 = exps(0).Description.IndexOf(holeexpstring)
If index2 > 0 Then
holewiththread = True
End If
If holewiththread = True Then
hole = DirectCast(f, BodyFeature)
faces = hole.GetFaces()
nFaces = faces.Length
ReDim obj(nFaces - 1)
For i As Integer = 0 To nFaces - 1
obj(i) = faces(i)
Next
displayModification1 = s.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = 6
displayModification1.Apply(obj)
Else 'holewiththread is false
hole = DirectCast(f, BodyFeature)
faces = hole.GetFaces()
nFaces = faces.Length
ReDim obj(nFaces - 1)
For i As Integer = 0 To nFaces - 1
obj(i) = faces(i)
Next
displayModification1 = s.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = 211
displayModification1.Apply(obj)
End If
End If
Next
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
Comments
I have painted Holes,
I have painted Holes, chamfers, blends, pockets, subtracted faces etc. But with one feature I have a problem. I am using NX 7.5, and for shells:
shell = DirectCast(f, Shell)
we don't have a method faces = shell.GetFaces()
there is a class ShellFace but I can't figure out how to use it.
Any ideas?
re: painted holes
Oddly, the NX7.5 documentation doesn't show the .GetFaces method for the Shell class, but the NX8 documentation does (and it notes it was added in NX3). Perhaps it is just an error in the documentation. Try to use the .GetFaces method and see what happens.
If you are still having problems, email your code to info@nxjournaling.com
re: painted holes
I cannot build the solution with the GetFaces() method. From Siemens NX Forum I know that in NX8
shell can be casted to BodyFeature class which contains GetFaces() method, but it also doesn't work under NX7.5. I will send my code to nxjournaling. Thanks for helping me.
re: shell.GetFaces
The Shell.GetFaces method seems to be broken in NX7.5. I would suggest you log a call with GTAC to report it; they are the only ones who are able to fix it.
Counterbored and Countersunk
How would i get this to work for counterbored and counter sunk holes as well?
re: Cbore & Csunk holes
Instead of looking for a feature type of "SIMPLE HOLE", you will want to look for "CBORE_HOLE" or "CSUNK_HOLE" as desired.
stil i am not getting indexof
stil i am not getting indexof ?
index of simplehole(i.e.=-1) & index of threaded(i.e.=1) are they fixed ?
re: indexOf
IndexOf is a string method. It searches for a substring within a string; if the substring is found, it will return the start position in the main string where the substring was found. If the substring cannot be found in the main string, it will return the value: -1. As an alternative, we could have used the string.Contains() method.
For some string code examples, see:
http://www.dotnetperls.com/indexof-vbnet
In this journal we are looking for the word "Threaded" within the expression description. If the return value is -1, we are dealing with a hole; if the return value is >= 0, we are dealing with a threaded hole.
thanks..got it.
thanks..got it.
all threaded holes
Is there a way to find out if a cylindrical face has thread?
We have many holes created by subtracted linked bodies, with thread.
Or can we find out the cylindrical face attached into symbolic thread?
I have found this in the nx.net reference, but I cannot make it work (in vb):
-----
UF_MODL_symb_thread_data_s
Also known as:
UF_MODL_symb_thread_data_t
UF_MODL_symb_thread_data_p_t
Overview
This structure is used in creating and inquiring symbolic threads.
Data Members
cyl_face
tag_t
Cylindrical face to be threaded.
etc.
-------
-------
kukelyk
re: wave linked threaded holes
The following code will look for symbolic thread features in your work part. If/when one if found, it will assign the 'thread callout' as the name of the cylindrical face. Hopefully, it will serve as a starting point for your needs.
Option Strict Off
Imports System
Imports System.Collections.Generic
Imports NXOpen
Imports NXOpen.UF
Module Module1
Sub Main()
Dim theSession As Session = Session.GetSession()
Dim theUfSession As UFSession = UFSession.GetUFSession()
Dim workPart As Part = theSession.Parts.Work
Dim lw As ListingWindow = theSession.ListingWindow
lw.Open()
Dim threadFeatures As New List(Of Features.Feature)
For Each myFeature As Features.Feature In workPart.Features
If myFeature.FeatureType.ToUpper = "SYMBOLIC_THREAD" Then
threadFeatures.Add(myFeature)
End If
Next
Dim myThreadParameters As UFModl.SymbThreadData
For Each myFeature As Features.Feature In threadFeatures
theUfSession.Modl.AskSymbThreadParms(myFeature.Tag, myThreadParameters)
Dim threadedFace As Face
threadedFace = Utilities.NXObjectManager.Get(myThreadParameters.cyl_face)
'if you highlight the face with the following line, you must remove the highlighting
'with the part cleanup -> remove extraneous highlighting command
'threadedFace.Highlight()
'apply thread callout as face name
threadedFace.SetName(myThreadParameters.callout)
'change preferences to show names in work view
workPart.Preferences.NamesBorderVisualization.ObjectNameDisplay = Preferences.PartVisualizationNamesBorders.NameDisplay.WorkView
Next
lw.Close()
End Sub
Public Function GetUnloadOption(ByVal dummy As String) As Integer
'Unloads the image when the NX session terminates
GetUnloadOption = NXOpen.Session.LibraryUnloadOption.AtTermination
'----Other unload options-------
'Unloads the image immediately after execution within NX
'GetUnloadOption = NXOpen.Session.LibraryUnloadOption.Immediately
'Unloads the image explicitly, via an unload dialog
'GetUnloadOption = NXOpen.Session.LibraryUnloadOption.Explicitly
'-------------------------------
End Function
End Module
re: wave linked threaded holes
Thanks for Your response. Unfortunately I had no time dealing with it. I tried it, it works fine, but.
I added only this:
[code]
theUfSession.Obj.SetColor(threadedFace.Tag, 100)
[/code]
to the journal.
If I run the journal, it makes everything well, but if I delete a thread feature, the callout remains displayed. I have never used (and have not known) callout. Could You please give some more help?
-------
kukelyk
re: threaded holes
The following code will run through the part and remove any custom names from faces before looking for symbolic threads. The code will then assign the thread callout as the name of the threaded face.
If you assign custom names to other faces in the file, the code will need to be modified to avoid removing those...
Option Strict Off
Imports System
Imports System.Collections.Generic
Imports NXOpen
Imports NXOpen.UF
Module Module1
Dim theSession As Session = Session.GetSession()
Dim theUfSession As UFSession = UFSession.GetUFSession()
Dim workPart As Part = theSession.Parts.Work
Dim lw As ListingWindow = theSession.ListingWindow
Sub Main()
lw.Open()
RemoveNames()
Dim threadFeatures As New List(Of Features.Feature)
Dim threadFaces As New List(Of Face)
For Each myFeature As Features.Feature In workPart.Features
If myFeature.FeatureType.ToUpper = "SYMBOLIC_THREAD" Then
threadFeatures.Add(myFeature)
End If
Next
Dim myThreadParameters As UFModl.SymbThreadData
For Each myFeature As Features.Feature In threadFeatures
theUfSession.Modl.AskSymbThreadParms(myFeature.Tag, myThreadParameters)
Dim threadedFace As Face
threadedFace = Utilities.NXObjectManager.Get(myThreadParameters.cyl_face)
'if you highlight the face with the following line, you must remove the highlighting
'with the part cleanup -> remove extraneous highlighting command
'threadedFace.Highlight()
threadFaces.Add(threadedFace)
'apply thread callout as face name
threadedFace.SetName(myThreadParameters.callout)
Next
'change preferences to show names in work view
workPart.Preferences.NamesBorderVisualization.ObjectNameDisplay = Preferences.PartVisualizationNamesBorders.NameDisplay.WorkView
lw.Close()
End Sub
Sub RemoveNames()
Dim markId1 As Session.UndoMarkId
markId1 = theSession.SetUndoMark(Session.MarkVisibility.Invisible, "Start")
Dim tFaces() As Face
For Each tBody As Body In workPart.Bodies
tFaces = tBody.GetFaces
For Each tFace As Face In tFaces
tFace.SetName("")
Next
Array.Clear(tFaces, 0, tFaces.Length)
Next
theSession.UpdateManager.DoUpdate(markId1)
End Sub
End Module
Features Colors
I have created an application which paints every machined face of a model. It paints all feature faces (and each subtract)
which removes a material from a model. It works very good. But there is one condition: it only works for 1 part.
When I use this app on the assembly, where I have "PROMOTED" or "LINKED" bodies and added some features it changes the colors, But it is no permanent. When I save, close and reopen the assembly all changes are gone.
Can somebody give me some advice how can I keep the new colors permanently?
re: feature colors
In the "Edit Object Display" dialog box, in the "settings" section, there is an option: "Apply changes to owning part"; in your assembly, change the color of a face of a component with this option set. Save your parts, close them, and reopen to see if the change 'stuck'. If it works, record a journal of the actions to see what code you need to change/add.
Change e.g. dia. 11 holes color
I would like to change in my part color of holes but only holes e.g. dia. 11. Anybody can give me advice how to do it?
re: hole color
What version of NX are you using?
Are you working with a parameterized file (a native NX file with hole features) or a dumb solid (imported data or a 'body' object with no features)?
If you are working with a native NX file, you can search through the features for hole features and query the diameter of the hole.
I am using NX10 version and I
I am using NX10 version and I am working with parameterized file (with hole features).Anybody know what code should be added to on the existing journal ( on the beginning of this post ) ?
Thanks
Marcin
re: hole color
Here is a journal for changing colour for simple holes based on hole diameter. Note you need to edit the code for hole diameter and face colour.
Option Strict OffImports System
Imports NXOpen
Imports NXOpen.UF
Imports NXOpen.Features
Module HoleColours
Sub Main()
Dim s As Session = Session.GetSession()
Dim ufs As UFSession = UFSession.GetUFSession()
Dim wp As Part = s.Parts.Work
Dim exps() As Expression
Dim holeexpstring As String = "Diameter"
Dim hole As BodyFeature
Dim faces() As Face
Dim nFaces As Integer = 0
Dim obj(-1) As DisplayableObject
Dim displayModification1 As DisplayModification
Dim featcoll As FeatureCollection = wp.Features
Dim holedia As Double = Nothing
Dim facecolour As Integer = 3
Dim holediachange As Double = 1.0
For Each f As Feature In featcoll
If f.FeatureType = "SIMPLE HOLE" Then
hole = DirectCast(f, BodyFeature)
exps = f.GetExpressions()
For Each exp1 As Expression In exps
If exp1.Description.Contains(holeexpstring) Then
holedia = exp1.Value
End If
Next
If holedia = holediachange Then
faces = hole.GetFaces()
nFaces = faces.Length
ReDim obj(nFaces - 1)
For i As Integer = 0 To nFaces - 1
obj(i) = faces(i)
Next
End If
displayModification1 = s.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = facecolour
displayModification1.Apply(obj)
End If
Next
End Sub
End Module
Frank Swinkels
Change e.g. G 1/8" thread color
I would like to add on last Frank journal, code which change color e.g. G1/8" thread. I tried to do it base on "hole color" journel it means instead of "SIMPLE HOLE" feature typ add "THREADED HOLE" feature - is it correct value? Maybe should be "THREADED_HOLE" or "THREAD". Where can I find correct "FeatureType" name? - for simple hole is SIMPLE HOLE; for Counterbored hole is CBORE_HOLE; for Countersunk hole is CSUNK_HOLE; where I can find the others (e.g. threaded hole)?.
Anyway in
Dim holeexpstring As String = "Thread Size" ' Instead of "Diameter"
and
Dim holediachange As Double = G 1-8 ' Instead of e.g. 1.0
but G1/8 can not be "Double" so I changed it on String Dim holediachange As String = "G 1-8"
I feel that it is not correct way.
Frank any idea?
I use NX10 version and I am working with parameterized files.
Thanks
Marcin
re: change thread color
Are you specifying the thread in the "hole" feature? If so, you can look for "hole package" type features in the feature collection and query the thread type from the feature.
If you are using the "thread" feature to add the thread to an existing hole or boss, you will need to look for the corresponding feature type in the collection.
I can't seem to find a reference to a G1/8" thread anywhere. What thread standard does it belong to? Or is this a custom thread that you have added to your NX install?
re: change thread color
To be honest I forgot that G1/8" thread is not standard NX thread in custom NX installation. G threads were added in my NX installation. OK, forget about the thread G - instead of this kind of thread use M8 standard metric thread. Mayby this is reason why my scribble not working. Anyway I use "hole" feature where I chose thread holes (metric or inch standard).
So you suggest as below (basic on last Frank "hole color" journal):
Dim holeexpstring As String = "Thread Size"
Dim holediachange As String = "M8"
Dim holedia As Double = Nothing
For Each f As Feature In featcoll
If f.FeatureType = "HOLE PACKAGE" Then
hole = DirectCast(f, BodyFeature)
exps = f.GetExpressions()
For Each exp1 As Expression In exps
If exp1.Description.Contains(holeexpstring) Then
holedia = exp1.Value
End If
Next
If holedia = holediachange Then
faces = hole.GetFaces()
nFaces = faces.Length
ReDim obj(nFaces - 1)
For i As Integer = 0 To nFaces - 1
obj(i) = faces(i)
Next
End If
displayModification1 = s.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = facecolour
displayModification1.Apply(obj)
End If
Next
re: hole color
If you find a "HOLE PACKAGE" feature, you can use the appropriate builder object to see if the hole is threaded and if so what the thread size is. If the hole/thread is the size that you are looking for, you can get the hole faces and change their color.
Option Strict Off
Imports System
Imports NXOpen
Module change_hole_color_2
Sub Main()
Dim theSession As Session = Session.GetSession()
If IsNothing(theSession.Parts.Work) Then
'active part required
Return
End If
Dim workPart As Part = theSession.Parts.Work
Dim lw As ListingWindow = theSession.ListingWindow
lw.Open()
Const undoMarkName As String = "change hole color"
Dim markId1 As Session.UndoMarkId
markId1 = theSession.SetUndoMark(Session.MarkVisibility.Visible, undoMarkName)
'Const holeColor As Integer = 211
Const holeThreadedColor As Integer = 6
Dim newColor As Integer
For Each theFeature As Features.Feature In workPart.Features
If TypeOf (theFeature) Is NXOpen.Features.HolePackage Then
Dim theHolePackageBuilder As Features.HolePackageBuilder = workPart.Features.CreateHolePackageBuilder(theFeature)
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.ThreadedHole Then
newColor = holeThreadedColor
'lw.WriteLine("thread size: " & theHolePackageBuilder.ThreadSize)
'lw.WriteLine("thread standard: " & theHolePackageBuilder.ThreadStandard)
If theHolePackageBuilder.ThreadSize.Contains("M8") Then
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = newColor
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
End If
theHolePackageBuilder.Destroy()
End If
Next
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
re: hole color
Below journal which recognizes holes dia.8, 10 11, 11.5; C'bore holes dia.10, 12, 14 and thread holes M3, M6, M8 and changes their colors face - written on the basic on your code. I am happy with myself because I am learning slowly read VB.NET reference guide (net_ref.chm file). I put it because maybe someone come in handy.
Option Strict Off
Imports System
Imports NXOpen
Module change_hole_color
Sub Main()
Dim theSession As Session = Session.GetSession()
If IsNothing(theSession.Parts.Work) Then
'active part required
Return
End If
Dim workPart As Part = theSession.Parts.Work
Dim lw As ListingWindow = theSession.ListingWindow
lw.Open()
Const undoMarkName As String = "change hole color"
Dim markId1 As Session.UndoMarkId
markId1 = theSession.SetUndoMark(Session.MarkVisibility.Visible, undoMarkName)
Const holeColor As Integer = 211
Const holeThreadedColor As Integer = 6
Dim newColor As Integer
Dim holedia() As Double = {8,10,11,11.5}
Dim cboredia() As Double = {10,12,14}
For Each theFeature As Features.Feature In workPart.Features
If theFeature.FeatureType = "HOLE PACKAGE" Then
'If TypeOf (theFeature) Is NXOpen.Features.HolePackage Then
Dim theHolePackageBuilder As Features.HolePackageBuilder = workPart.Features.CreateHolePackageBuilder(theFeature)
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.GeneralHole Then
newColor = holeColor
'lw.WriteLine("Diameter: " & theHolePackageBuilder.GeneralSimpleHoleDiameter.Value)
'lw.WriteLine("Counter Bore Diameter: " & theHolePackageBuilder.GeneralCounterboreDiameter.Value)
For i As Integer = 0 To holedia.GetUpperBound(0)
For j As Integer = 0 To cboredia.GetUpperBound(0)
If theHolePackageBuilder.GeneralSimpleHoleDiameter.Value = holedia(i) or theHolePackageBuilder.GeneralCounterboreDiameter.Value = cboredia(j) Then
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = newColor
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
Next
Next
End if
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.ThreadedHole Then
newColor = holeThreadedColor
'lw.WriteLine("thread size: " & theHolePackageBuilder.ThreadSize)
'lw.WriteLine("thread standard: " & theHolePackageBuilder.ThreadStandard)
If theHolePackageBuilder.ThreadSize.Contains("M3") or theHolePackageBuilder.ThreadSize.Contains("M6") or theHolePackageBuilder.ThreadSize.Contains("M8") Then
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = newColor
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
End if
theHolePackageBuilder.Destroy()
End If
Next
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
Hole Color
Hello Experts
In our model heaving 10 simple holes.
macro need to give colour to holes as per below instructions
(diameter 8,10,5,15,20) = yellow colour
(diameter 30,45,85,49,53)= cyan colour
Thank you
Reagrds
Naveen
Re: Hole Color
Below code which maybe will be helpful
Option Strict Off
Imports System
Imports NXOpen
Module change_hole_color
Sub Main()
Dim theSession As Session = Session.GetSession()
If IsNothing(theSession.Parts.Work) Then
'active part required
Return
End If
Dim workPart As Part = theSession.Parts.Work
Dim lw As ListingWindow = theSession.ListingWindow
lw.Open()
Const undoMarkName As String = "change hole color"
Dim markId1 As Session.UndoMarkId
markId1 = theSession.SetUndoMark(Session.MarkVisibility.Visible, undoMarkName)
Const holeColor As Integer = 211
Const holeThreadedColor As Integer = 6
Dim newColor As Integer
Dim holedia() As Double = {5,8,10,15,20,30,45,49,53,85}
Dim cboredia() As Double = {10,12,14}
For Each theFeature As Features.Feature In workPart.Features
If theFeature.FeatureType = "HOLE PACKAGE" Then
'If TypeOf (theFeature) Is NXOpen.Features.HolePackage Then
Dim theHolePackageBuilder As Features.HolePackageBuilder = workPart.Features.CreateHolePackageBuilder(theFeature)
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.GeneralHole Then
'newColor = holeColor
'lw.WriteLine("Diameter: " & theHolePackageBuilder.GeneralSimpleHoleDiameter.Value)
'lw.WriteLine("Counter Bore Diameter: " & theHolePackageBuilder.GeneralCounterboreDiameter.Value)
For i As Integer = 0 To holedia.GetUpperBound(0)
For j As Integer = 0 To cboredia.GetUpperBound(0)
If theHolePackageBuilder.GeneralSimpleHoleDiameter.Value = holedia(i) or theHolePackageBuilder.GeneralCounterboreDiameter.Value = cboredia(j) Then
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
Select Case theHolePackageBuilder.GeneralSimpleHoleDiameter.Value
Case is = 30
displayModification1.NewColor = 31 'cyan
Case is = 45
displayModification1.NewColor = 31 'cyan
Case is = 49
displayModification1.NewColor = 31 'cyan
Case is = 53
displayModification1.NewColor = 31 'cyan
Case is = 85
displayModification1.NewColor = 31 'cyan
Case else
displayModification1.NewColor = 6 ' yellow
End Select
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
Next
Next
End if
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.ThreadedHole Then
newColor = holeThreadedColor
'lw.WriteLine("thread size: " & theHolePackageBuilder.ThreadSize)
'lw.WriteLine("thread standard: " & theHolePackageBuilder.ThreadStandard)
If theHolePackageBuilder.ThreadSize.Contains("M3") or theHolePackageBuilder.ThreadSize.Contains("M6") or theHolePackageBuilder.ThreadSize.Contains("M8") Then
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = newColor
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
End if
theHolePackageBuilder.Destroy()
End If
Next
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
Hole Color
Thanks for your support
In our model we have used simple holes and thread holes so macro
need to change color of only simple holes and thread holes.
simple holes= in blue color
thread holes = in yellow colour
if part contain other than simple hole feature and tread feature it should be in red color.
Thank you
Hole Color
Currently i did for part contain simple holes and tread holes.
macro will change the color of simple holes as per hole diameters.
Example
hole dia = 50,60 should be in blue color
hole dia = 30,40 should be in cyan color
All tread holes in yellow color
Option Strict Off
Imports System
Imports NXOpen
Module change_hole_color
Sub Main()
Dim theSession As Session = Session.GetSession()
If IsNothing(theSession.Parts.Work) Then
'active part required
Return
End If
Dim workPart As Part = theSession.Parts.Work
Dim lw As ListingWindow = theSession.ListingWindow
lw.Open()
Const undoMarkName As String = "change hole color"
Dim markId1 As Session.UndoMarkId
markId1 = theSession.SetUndoMark(Session.MarkVisibility.Visible, undoMarkName)
Const holeColor As Integer = 211
Const holeColor2 As Integer = 31
Const holeThreadedColor As Integer = 6
Dim newColor As Integer
For Each theFeature As Features.Feature In workPart.Features
If theFeature.FeatureType = "HOLE PACKAGE" Then
Dim theHolePackageBuilder As Features.HolePackageBuilder = workPart.Features.CreateHolePackageBuilder(theFeature)
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.GeneralHole Then
newColor = holeColor
If theHolePackageBuilder.GeneralSimpleHoleDiameter.Value = 60 or theHolePackageBuilder.GeneralSimpleHoleDiameter.Value = 50 Then
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = newColor
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
If theHolePackageBuilder.GeneralSimpleHoleDiameter.Value = 40 or theHolePackageBuilder.GeneralSimpleHoleDiameter.Value = 35 Then
newColor = holeColor2
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = newColor
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
End if
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.ThreadedHole Then
newColor = holeThreadedColor
If theHolePackageBuilder.ThreadSize.Contains("M30") or theHolePackageBuilder.ThreadSize.Contains("M6") or theHolePackageBuilder.ThreadSize.Contains("M8") Then
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = newColor
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
End if
theHolePackageBuilder.Destroy()
End If
Next
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
Please support on below points
I need create the two arrays like
Dim holedia1() As Double = {50,60}
Dim holedia2() As Double = {30,40}
holedia1 for blue color
holedia2 for cyan color
all tread holes should be in yellow color(for all sizes)
other holes in red color
RE: Hole Color
Regarding to simple hole you can use select case method as shown on previous post
https://docs.microsoft.com/en-us/dotnet/visual-basic/language-reference/...
Below code changing all threaded color.
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.ThreadedHole Then
'lw.WriteLine("thread size: " & theHolePackageBuilder.ThreadSize)
'lw.WriteLine("thread standard: " & theHolePackageBuilder.ThreadStandard)
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = 6
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End if
RGB values
Hello Experts
Please help on my requirements
My requirements are
Through RGB values i need to control the macro
1) All threaded holes in yellow color = its solved
2) 8 dia ,6dia,10dia,17dia =blue color
Thank you
Hole Color
Thanks for reply
Below code apply the blue colour and cyan color for simple holes.
blue color and cyan colour divided on basis of hole diameters.
user will mention diameters in two arrays like.
Dim holedia() As Double = {5,6,8,10,12}
Dim cboredia() As Double = {4.8,5.8,6.6,9,11,14,17.5,22}
need support on
In a model having simple hole but hole dia not mentioned above two arrays means
it should be in red colour and model contains conterbore or other type holes means macro needs apply red color.
Option Strict Off
Imports System
Imports NXOpen
Module change_hole_color
Sub Main()
Dim theSession As Session = Session.GetSession()
If IsNothing(theSession.Parts.Work) Then
Return
End If
Dim workPart As Part = theSession.Parts.Work
Dim lw As ListingWindow = theSession.ListingWindow
lw.Open()
Const undoMarkName As String = "change hole color"
Dim markId1 As Session.UndoMarkId
markId1 = theSession.SetUndoMark(Session.MarkVisibility.Visible, undoMarkName)
Const holeColor As Integer = 211
Const holeColor1 As Integer = 31
Const holeThreadedColor As Integer = 6
Dim newColor As Integer
Dim holedia() As Double = {5,6,8,10,12}
Dim cboredia() As Double = {4.8,5.8,6.6,9,11,14,17.5,22}
For Each theFeature As Features.Feature In workPart.Features
If theFeature.FeatureType = "HOLE PACKAGE" Then
Dim theHolePackageBuilder As Features.HolePackageBuilder = workPart.Features.CreateHolePackageBuilder(theFeature)
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.GeneralHole Then
For i As Integer = 0 To holedia.GetUpperBound(0)
For j As Integer = 0 To cboredia.GetUpperBound(0)
If theHolePackageBuilder.GeneralSimpleHoleDiameter.Value = holedia(i) or theHolePackageBuilder.GeneralSimpleHoleDiameter.Value = cboredia(j) Then
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
Select Case theHolePackageBuilder.GeneralSimpleHoleDiameter.Value
Case is = 5
displayModification1.NewColor = 211
Case is = 6
displayModification1.NewColor = 211
Case is = 8
displayModification1.NewColor = 211
Case is = 10
displayModification1.NewColor = 211
Case is = 12
displayModification1.NewColor = 211
Case is = 4.8
displayModification1.NewColor = 31
Case is = 5.8
displayModification1.NewColor = 31
Case is = 6.6
displayModification1.NewColor = 31
Case is = 9
displayModification1.NewColor = 31
Case is = 11
displayModification1.NewColor = 31
Case is = 14
displayModification1.NewColor = 31
Case is = 17.5
displayModification1.NewColor = 31
Case is = 22
displayModification1.NewColor = 31
Case else
displayModification1.NewColor = 6
End Select
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
Next
Next
End if
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.ThreadedHole Then
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = holeThreadedColor
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
theHolePackageBuilder.Destroy()
End If
Next
lw.Close()
End Sub
Public Function GetUnloadOption(ByVal dummy As String) As Integer
GetUnloadOption = NXOpen.Session.LibraryUnloadOption.Immediately
End Function
End Module
apply color to all subtracted face
Hello everyone, does someone have any code for applying face color to all subtracted faces. Found several useful codes for hole color update. Couldn't find any for subtracted faces. Thanks, B
Balaji
re: face color
There are 2 options in NX that may help.
Based on your question, I'd guess the first option is closer to what you want. Record a journal while applying a feature color to see what is required. After that, it should be fairly easy to iterate through the feature tree and apply a feature color to all the subtract features.
Assign Color to subtracted faces
Hi NX Journaling, managed to make the Below journal which assigns 'Yellow' color to all the subtracted faces. Used few codes of other journals from this forum.(apply feature color to the hole feature).
' NX 12.0.1.7
' Journal created by Balaji_Sampath03 on Mon Jul 13 11:15:56 2020 India Standard Time
'
'**************************************************************************************
'This Macro Assigns 'Yellow' colour to represent the machined feature
'to the features (extrude/revolve) with the operation type subtract
'to the boolean feature of type 'subtract'
'to all the hole features
'And Chamfer/trim/EdgeBlend
'***************************************************************************************
Imports System
Imports NXOpen
Module NXJournal
Sub Main (ByVal args() As String)
Dim theSession As NXOpen.Session = NXOpen.Session.GetSession()
Dim workPart As NXOpen.Part = theSession.Parts.Work
Dim displayPart As NXOpen.Part = theSession.Parts.Display
Dim markId1 As NXOpen.Session.UndoMarkId = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Visible, "Start")
theSession.SetUndoMarkName(markId1, "Assign Feature Face Color")
Const holeColor As Integer = 6
Const holeThreadedColor As Integer = 6
Dim newColor As Integer
Dim colorFeatureBuilder1 As NXOpen.Features.ColorFeatureBuilder = Nothing
colorFeatureBuilder1 = workPart.Features.CreateColorFeatureBuilder()
colorFeatureBuilder1.Color = workPart.Colors.Find("Yellow")
For Each theFeature As Features.Feature In workPart.Features
If TypeOf (theFeature) Is NXOpen.Features.Extrude Then
Dim extBuilder As NXOpen.Features.ExtrudeBuilder = workPart.Features.CreateExtrudeBuilder(theFeature)
If extBuilder.BooleanOperation.Type = NXOpen.GeometricUtilities.BooleanOperation.BooleanType.Subtract Then
Dim objects1(0) As NXOpen.Features.Feature
objects1(0) = theFeature
Dim added1 As Boolean = Nothing
added1 = colorFeatureBuilder1.SelectFeature.Add(objects1)
Dim nXObject1 As NXOpen.NXObject = Nothing
nXObject1 = colorFeatureBuilder1.Commit()
End If
End If
If TypeOf (theFeature) Is NXOpen.Features.Revolve Then
Dim revolveBuilder As NXOpen.Features.RevolveBuilder = workPart.Features.CreateRevolveBuilder(theFeature)
If revolveBuilder.BooleanOperation.Type = NXOpen.GeometricUtilities.BooleanOperation.BooleanType.Subtract Then
Dim objects1(0) As NXOpen.Features.Feature
objects1(0) = theFeature
Dim added1 As Boolean = Nothing
added1 = colorFeatureBuilder1.SelectFeature.Add(objects1)
Dim nXObject1 As NXOpen.NXObject = Nothing
nXObject1 = colorFeatureBuilder1.Commit()
End If
End If
If TypeOf (theFeature) Is NXOpen.Features.BooleanFeature Then
Dim booleanBuilder As NXOpen.Features.BooleanBuilder = workPart.Features.CreateBooleanBuilderUsingCollector(theFeature)
If booleanBuilder.Operation = NXOpen.Features.Feature.BooleanType.Subtract Then
Dim objects1(0) As NXOpen.Features.Feature
objects1(0) = theFeature
Dim added1 As Boolean = Nothing
added1 = colorFeatureBuilder1.SelectFeature.Add(objects1)
Dim nXObject1 As NXOpen.NXObject = Nothing
nXObject1 = colorFeatureBuilder1.Commit()
End If
End If
If TypeOf (theFeature) Is NXOpen.Features.Chamfer Then
Dim objects1(0) As NXOpen.Features.Feature
objects1(0) = theFeature
Dim added1 As Boolean = Nothing
added1 = colorFeatureBuilder1.SelectFeature.Add(objects1)
Dim nXObject1 As NXOpen.NXObject = Nothing
nXObject1 = colorFeatureBuilder1.Commit()
End If
If TypeOf (theFeature) Is NXOpen.Features.TrimBody2 Then
Dim objects1(0) As NXOpen.Features.Feature
objects1(0) = theFeature
Dim added1 As Boolean = Nothing
added1 = colorFeatureBuilder1.SelectFeature.Add(objects1)
Dim nXObject1 As NXOpen.NXObject = Nothing
nXObject1 = colorFeatureBuilder1.Commit()
End If
If TypeOf (theFeature) Is NXOpen.Features.EdgeBlend Then
Dim objects1(0) As NXOpen.Features.Feature
objects1(0) = theFeature
Dim added1 As Boolean = Nothing
added1 = colorFeatureBuilder1.SelectFeature.Add(objects1)
Dim nXObject1 As NXOpen.NXObject = Nothing
nXObject1 = colorFeatureBuilder1.Commit()
End If
If TypeOf (theFeature) Is NXOpen.Features.HolePackage Then
Dim theHolePackageBuilder As Features.HolePackageBuilder = workPart.Features.CreateHolePackageBuilder(theFeature)
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.ThreadedHole Then
newColor = holeThreadedColor
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = newColor
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
If theHolePackageBuilder.Type = Features.HolePackageBuilder.Types.GeneralHole Then
newColor = holeColor
Dim displayModification1 As DisplayModification
displayModification1 = theSession.DisplayManager.NewDisplayModification()
displayModification1.ApplyToAllFaces = False
displayModification1.NewColor = newColor
displayModification1.Apply(CType(theFeature, Features.HolePackage).GetFaces)
displayModification1.Dispose()
End If
theHolePackageBuilder.Destroy()
End If
Next
colorFeatureBuilder1.Destroy()
End Sub
End Module
Balaji