How to get point names

Submitted by 218156 on Thu, 04/23/2020 - 04:19
Forums: 
Journaling / NXOpen API

I have created some Associative points and renamed like point1, point2 etc, and added in layer 10, below is my code

Option Strict Off
Imports System
Imports NXOpen
Imports NXOpenUI
Imports NXOpen.UF
Imports NXOpen.Utilities

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()
For Each myPoint As Point In workPart.Points

If myPoint.Layer = 10 Then
lw.WriteLine(myPoint.Name)
lw.WriteLine(myPoint.Coordinates.ToString)
End If

Next

End Sub

End Module

When I execute above code I am getting coordinates but not names of points
can you please let me know where is problem in my code and I need names of these points please help me

Thanks

NXJournaling - Thu, 04/23/2020 - 08:29

In NX, features (the entries you see in the part navigator) create and manage geometric objects. NX allows you to apply a name to the feature and/or the object. The code that you posted will report the name as applied to the object itself. Since you do not get any results, I'm going to assume that you have applied the names to the point features. Do your custom names show up in the part navigator? If so, those are feature names.

So, there are a few options here:

  • change the code to iterate through the features, look for point features and report the feature names
  • keep the code you have, but ask the point object which feature it belongs to and report the feature name
  • go back and assign the names to the point objects

Which you use will depend on your needs. I can help with any of the above if you have specific questions.

218156 - Thu, 04/23/2020 - 09:01

Hi.
Thanks for your quick reply,
Yes names are given to features and these names are appearing in part navigator;
I tried with another method, below is my code

Option Strict Off
Imports System
Imports NXOpen
Imports NXOpenUI
Imports NXOpen.UF
Imports NXOpen.Utilities
Imports NXOpen.Features

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()

Dim mypoint1 As PointFeature

For Each myFeature As Feature In workPart.Features
If TypeOf (myFeature) Is PointFeature Then
mypoint1 = myFeature
lw.WriteLine(mypoint1.Name)
End If

Next

End Sub

End Module

This time I am getting feature name but I am note getting layer and coordinate properties,

My requirement is to process all the points in specific layer say layer 10 and get name and coordinate of point

can you please help me

thanks In Advance

NXJournaling - Thu, 04/23/2020 - 09:25

The point feature (myPoint1, in your code) has a .Location property that returns a Point3D structure. This is one way to get the coordinates of your point. Try the following:

lw.writeline(myPoint1.Location.ToString)

Alternatively, you could use the point feature's .GetEntities method to gain access to the point object and query its .Coordinates property (also returns a Point3D structure).

218156 - Thu, 04/23/2020 - 10:26

Hello,
Thanks For Your reply,

when I am using location property I am Getting below Error

NXOpen.NXException: Feature has no Origin
at NXOpen.Feature.get Location()

since I need both Layer and coordinate properties I used GetEntities method but I am getting below error
System.IndexOutOfRangeException: Index was outside the bounds of the array

Below is my code

Option Strict Off
Imports System
Imports NXOpen
Imports NXOpenUI
Imports NXOpen.UF
Imports NXOpen.Utilities
Imports NXOpen.Features

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()

Dim mypoint1 As PointFeature

For Each myFeature As Feature In workPart.Features
If TypeOf (myFeature) Is PointFeature Then
mypoint1 = myFeature
lw.WriteLine(mypoint1.Name)

Dim myNxObject() As NXObject
myNxObject = mypoint1.GetEntities()
Dim pt As Point = CType(myNxObject(0), Point)
lw.WriteLine(pt.Coordinates.ToString)
lw.WriteLine(pt.Layer)

End If

Next

End Sub

End Module

can you please suggest what is problem in my code

NXJournaling - Thu, 04/23/2020 - 15:07

I created a simple part (3 point features) and ran your code; it completed successfully for me. What version of NX are you using? What features are contained in your part? Does your part have point sets or patterns of point features?

218156 - Fri, 04/24/2020 - 06:16

Earlier I was checking in lower version of NX, I was getting Error, Now I checked in higher version it is working fine

Thank you so much for your grate help

Thanks