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# Degree of Freedom Arrows in Sketch

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?

Zsolt

13 REPLIES

# Re: Degree of Freedom Arrows in Sketch

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

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

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'.

Ganesh Kadole, QA Analyst (PLM), SQS
Testing: NX 11 | NX 12 | TCIN
TC 11.2 | TC Vis 11.3 | AWC 3.2

# Re: Degree of Freedom Arrows in Sketch

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

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

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

# Re: Degree of Freedom Arrows in Sketch

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

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.

Ganesh Kadole, QA Analyst (PLM), SQS
Testing: NX 11 | NX 12 | TCIN
TC 11.2 | TC Vis 11.3 | AWC 3.2

# Re: Degree of Freedom Arrows in Sketch

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