Units

When dealing with any CAD program, it is vital to know what system of units you are currently working in. Without a system of units it would be impossible to know how large the object is that you are designing. What is the estimated weight of the object? What is the estimated inertia about the drive axis? Is the design within a balance specification? These questions would be difficult, if not impossible, to answer without knowing the unit system in the current part. As such, unit systems are very important when modeling. With NX, working with units can largely be a "set it and forget it" operation; you specify either "inches" or "millimeters" when creating a new part and for the most part you don't have to worry about it after that.

When programming NX, you will encounter situations where you must specify the desired units (measurement functions, expressions with units, etc). Fortunately, the NXOpen API provides us with what we need.

Part Units

As stated above, there are only two choices for units when creating a new NX part file: inches or millimeters. Every existing part has a .PartUnits property that you can query to determine the overall unit system for the part. The NXOpen API defines the BasePart.Units enumeration to hold the possible values and display them in a human-friendly form. Knowing the unit system of the part that the journal is currently working with can be important when changing preferences such as modeling tolerance or text height. To make our journals flexible and robust, we should check the part units before setting any preferences that are unit dependent.

Option Strict Off
Imports System
Imports NXOpen

Module partUnits

Sub Main()

Dim theSession As Session = Session.GetSession()
If IsNothing(theSession.Parts.BaseWork) Then
'active part required
Return
End If

Dim workPart As Part = theSession.Parts.Work
Dim lw As ListingWindow = theSession.ListingWindow
lw.Open()

Dim textHeight As Double

If workPart.PartUnits = BasePart.Units.Inches Then
textHeight = 0.12
lw.WriteLine("Inch part file, textHeight = " & textHeight.ToString)
Else
textHeight = 3
lw.WriteLine("Millimeter part file, textHeight = " & textHeight.ToString)
End If

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

The code above simply checks the workPart's .PartUnits property; if the value is equal to the enumeration member: BasePart.Units.Inches, the test returns True and we know that we are dealing with an inch file. If the test results in a False value, it must be a millimeter file.

The available units

Of course there is much more to it than just knowing if the part is using "inch" or "millimeter" units. The expression system allows you to use a number of different unit types for your engineering calculations and the FEA and motion simulation applications require the use of units for their calculations. This means that NX has to be aware of quantities such as angular acceleration, thermal energy, dynamic viscosity, mass flow rate, frequency, and many more.

To see the full range of units available to you in NX, run the following journal. All of the available units will be output to the information window, grouped by type.

Option Strict Off
Imports System
Imports NXOpen

Module units

Sub Main()

Dim theSession As Session = Session.GetSession()
If IsNothing(theSession.Parts.BaseWork) Then
'active part required
Return
End If

Dim workPart As Part = theSession.Parts.Work
Dim lw As ListingWindow = theSession.ListingWindow
lw.Open()

Dim theMeasures() As String = workPart.UnitCollection.GetMeasures

For Each unitMeasure As String In theMeasures
Dim partBaseUnit As Unit = workPart.UnitCollection.GetBase(unitMeasure)
Dim unitMeasureTypes() As Unit
unitMeasureTypes = workPart.UnitCollection.GetMeasureTypes(unitMeasure)

lw.WriteLine(unitMeasure & " [part base unit: " & partBaseUnit.Name & "]")
lw.WriteLine("")
For Each unitType As Unit In unitMeasureTypes
lw.WriteLine(" name: " & unitType.Name)
lw.WriteLine(" abbreviation: " & unitType.Abbreviation)
lw.WriteLine("")
Next
lw.WriteLine("")
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

Finding units, converting units

The best way to create a unit object (in fact, the only way that I'm currently aware of) is to use the {part object reference}.UnitCollection.FindObject("unit name") method. By specifying the name of the unit, the UnitCollection will return the proper type. The journal above lists all the available units in NX. This is a good reference to have on hand if/when you are working with unit objects in NX. To successfully find the proper unit in the UnitCollection, the name must be specified exactly as NX expects (both correct spelling and capitalization are important).

The UnitCollection also provides us with a .Convert() method which will allow us to convert values from one unit to another. The units must both belong to the same measurement type, of course. Trying to convert a length in miles to a temperature in degrees Celcius doesn't make any sense, and NX will not hesitate to tell you so.

The journal code below will create an "inch" unit and a "centimeter" unit then it will convert a value from inches to centimeters.

Option Strict Off
Imports System
Imports NXOpen

Module GetUnit

Sub Main()

Dim theSession As Session = Session.GetSession()
If IsNothing(theSession.Parts.BaseWork) Then
'active part required
Return
End If

Dim workPart As Part = theSession.Parts.Work
Dim lw As ListingWindow = theSession.ListingWindow
lw.Open()

Dim inchUnit As Unit = workPart.UnitCollection.FindObject("Inch")
Dim centimeterUnit As Unit = workPart.UnitCollection.FindObject("CentiMeter")

'convert value from inches to centimeters
Dim lengthInInches As Double = 12
Dim lengthInCm As Double

'{part ref}.UnitCollection.Convert(initialUnits, targetUnits, initialValue)
'returns Double value representing the equivalent value in the target units
lengthInCm = workPart.UnitCollection.Convert(inchUnit, centimeterUnit, lengthInInches)

lw.WriteLine(lengthInInches.ToString & " inches = " & lengthInCm.ToString & " cm")

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

Conclusion

Units are very important to any CAD file. Make sure that you know the units of the current part before making changes to unit sensitive values (e.g. the part list maximum section height). Creating and using unit objects will be especially important when working with measurement functions and expressions.