Can't find the 2 last constraints in a closed spline sketch.

[stephlouv]

Hi there,

On NX 9.0.3.5
I am trying to constrain a closed spline within a sketch.
I added dimension for each thought point but they are always 2 constraint needed.
I usually really good a this but here I don't understand why NX require 2 more.

Even the "continuous Auto dimensioning" can't solve it.

It seems that the "closed" option add a last point above the first.
And because this last point is "virtual", it's impossible to constrain it.

See screenshot attached.

Thank you guys.

Stéphane



"My english is bad ? That's why i'am french."

 

[stephlouv]

The screenshot.

"My english is bad ? That's why i'am french."

 

[stephlouv]

OK.
I did a basic test.
A new part file, a new sketch, auto-dimensions, an open spline through 4 points.
All is constraint.

"My english is bad ? That's why i'am french."

 

[stephlouv]

Now I am closing the spline.
2 constraints needed.

Which is stupid as the last point is the first.
But maybe not for the sketch solving engine.

"My english is bad ? That's why i'am french."

 

[stephlouv]

OK. It goes deeper ....
From the closed spline
I enter values to the auto-dimensions.
Only one couple of dim is referencing datums.
The other dim will make the through points "rigid" between them.
Still 2 constraints needed.



"My english is bad ? That's why i'am french."

 

[stephlouv]

I now change p1 to 20 instead of 126.
To me, the all spline should translate 106mm to the left.
.... Well ... No ....

And they are p3 and p5 that are referencing a invisible point ???

"My english is bad ? That's why i'am french."

 

[stephlouv]

I'm now editing the spline and uncheck the "Closed" option.
P3 & p5 are now OK and I get the same shape at first.

I can close again the spline.

There is a problem with the closing point.
For GTAC ?



"My english is bad ? That's why i'am french."

 

[JohnRBaker]

OK, I've verified that this is happening in NX 9.0.3.4. That being said, I have some good news and bad news.

The bad news is that even using NX 10.0.3.1, this still has a problem with having two missing constraints, at least as far as the solver is concerned.

Now for the good news, this has been fixed in the next version of NX (not NX 10.0 but the version that we're just now in middle of beta testing and which will be available in the spring of next year).

Now in the mean time, the reality is that your spline IS fully constrained. After all if each point of the spline has been dimensioned it's fully constrained. True, the software will continue to tell you that it isn't and Check-Mate will flag it as being not being fully constrained, but the reality is that there is nothing more that you can do to constrain it. But that has all been fixed in the version that we're currently working on as a result of using some new solver options particularly when it comes to splines. And before you ask, no these improvements can't be ported back to NX 9.0 or NX 10.0.

Now the only other approach is to create your sketch of just the points that define the spline and then outside of the sketcher, create a closed spline through the sketch points.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[stephlouv]

Thank you John.

All make sense now.

But it's not easy to create a spline (from the curve menu) based on points from a sketch. They are hard to select and associativity not guaranty. ???
I instead create a poly-line sketch representing the future spline "poles".
It's then super easy to create the spline based on the lines end points and the associativity is perfect.

This spline is made to define a break out section boundary.
Can you please have a look to my other subject :

http://www.eng-tips.com/viewthread.cfm?qid=394472

"My english is bad ? That's why i'am french."