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Degree of Freedom Arrows in Sketch

Creator
Creator

Hello,

 

In Sketch, the degree of freedom arrows are visible only when the Geometric Constraints or Rapid Dimension command is active. Is it possible to show them all the time when the sketch is being edited?

 

Thanks for your help,
Zsolt

13 REPLIES

Re: Degree of Freedom Arrows in Sketch

Phenom
Phenom

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.

-Dave
NX 11 | Teamcenter 11 | Windows 8.1

Re: Degree of Freedom Arrows in Sketch

Creator
Creator

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.

Re: Degree of Freedom Arrows in Sketch

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi @Crypto,

If you turn off 'Continuous Auto Dimensioning', basically number of DOF can be seen at the status bar where it shows like 'Sketch needs 3 constraints'.

Regards,
Ganesh

Re: Degree of Freedom Arrows in Sketch

Phenom
Phenom

Hi @Crypto,

it's not possible. You have to open en ER for this, like me. More users ask the same, more probability Siemens PLM implement it.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: Degree of Freedom Arrows in Sketch

Phenom
Phenom

Hi @GaneshKadole,

your answer it's not for what was asked. 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.

Thank you...

Using NX 11 / RuleDesigner PDM

Re: Degree of Freedom Arrows in Sketch

Creator
Creator

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 Smiley Wink

Re: Degree of Freedom Arrows in Sketch

Honored Contributor
Honored Contributor

"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.

Re: Degree of Freedom Arrows in Sketch

Siemens Phenom Siemens Phenom
Siemens Phenom


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.

@cubalibre00

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.

Regards,
Ganesh

Re: Degree of Freedom Arrows in Sketch

Honored Contributor
Honored Contributor

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