Not that I am aware of.
That said, I thought they displayed, and disappeared as you applied constraints, back when I first started using Unigraphics, ie circa UG v8. I could be mistaken though.
It is OK when you apply constraints and dimensions the arrows disappear. My problem is that I have to open the Rapid Dim. or the Contraints to see where should I put constraints or dimension.
Yes I know when the Auto Dimensioning is on the arrows are not even visible neither in the Rapid D. or Geometric Constraints. I am just trying to get know my possibilities
"Yes I know when the Auto Dimensioning is on the arrows are not even visible neither in the Rapid D. or Geometric Constraints."
This is because when auto dimensioning is on, your sketch is fully constrained (NX adds auto dimensions to constrain the sketch). So in this case, the arrows are not visible because they are not needed.
NX can say 1 or 1000 degree of freedom, but the user can't see in the sketch which entities must contrained without starts command indicated by @Crypto.
Correct and you have already mentioned that it can be a ER to the existing behaviour (as designed behaviour). Probably such ER may exists already.
Testing: NX 11 | NX 12 | TCIN
TC 11.2 | TC Vis 11.3 | AWC 3.2
Below is a quick journal that will toggle the DOF display of the active sketch. If you add a dimension and close the dimension dialog, NX will automatically turn off the DOF display (you can run the journal again to turn it back on, if desired).
Not thoroughly tested. If you run into an issue, post it here and I'll see if I can fix it.
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, "toggle active sketch DOF") lw.Open() For Each temp As Sketch In theSession.Parts.Work.Sketches If temp.IsActive Then temp.DOFDisplay = Not temp.DOFDisplay 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 '----Other unload options------- 'Unloads the image when the NX session terminates 'GetUnloadOption = NXOpen.Session.LibraryUnloadOption.AtTermination 'Unloads the image explicitly, via an unload dialog 'GetUnloadOption = NXOpen.Session.LibraryUnloadOption.Explicitly '------------------------------- End Function End Module