Creating tubular structures with loops ?? 1

[skanskan]

Hello.

Sometimes one needs to create a structure from a sketch (for example with sweep -> tube tube) and gets the error
"Gaps in string or multiple loops".

In order to avoid that error I must select one single line at a time but that could be very time consuming if we have many lines.
And it has a major drawback, the resulting corners are not rounded and it's quite complex to round all corners.

Is there any other way to accomplish this task easily?
I know there is a "routing mechanical" module but not all users have its license, and the result of that module it's not a "common" object, and it needs a special work method.

Imagine I have this simple structure.

Is there any method to choose only the horizontal lines?
(with a big selection square around all of them and some kind ot filter)
and later only the vertical ones.
Or in general, selecting all lines in a given direction.

 

[skanskan]

Or how can I quickly convert that sketch into a path to be used with the router mechanical module?

 

[Toost]

I only have an answer to your last question,
You can in one step convert a sketch such as the one above into "routing path" using the "Connected curves" command. ( drag rectangle around all)
Then in the attached image i applied "Space reservation" using rectangle selection around all in one step.
in this particular case NX then creates 16 Sweeps. Note that these features are not united and not blended.

Regards,
Tomas

 

[skanskan]

OK thanks, I'll try.

One more question.
If I pattern a curve (on the sketch interface)...
The result is a patterned curve but I can't see anything on the history.
How can I later modify the parameters of this pattern?
For example I create a pattern of a line that produces 10 lines with a spacing of 1cm. Later I change my mind and need the spacing equal to 1.5cm.

 

[Toost]

i agree, this is difficult to see in the sketcher, there are small symbols that tells that there is a pattern inside the sketch, see attached image.
If you know / see this, then double click any of these curves and you will bring back the patterning dialog and can change.
Image / symbols from NX9.

Regards,
Tomas

 

[skanskan]

And what about NX8.5 ?

 

[JohnRBaker]

Here's on alternative that dose not require anything other than Modeling.

Create a single sketch 'grid'. Now add the four tubes (of course you have to create them one-at-a-time, but you only need to do this once) and then create a 'Feature Group' of the tubes but do NOT include the Sketch nor the Datum CSYS (this step is really optional but it does help organize your model). Now using 'Pattern Feature', create a 'Linear' pattern in the X and Y directions using the 'Count and Pitch' Spacing method with the Count being whatever you wish it to be and the Pitch Distance to be the same as the 'Grid' size. Note that you must use the 'Variational' Pattern Method since you will be Patterning the Feature Group (even if you didn't use the Feature Group you'd still need to use the 'Variational' method as you'd now be picking the four tubes). Note that I took care of the 'corners' by adding a 20 mm Sphere at the origin and then creating a 2 x 2 Pattern of it at the extents of the overall grid pattern. Once the Pattern Features are created, Unite them all into a single solid and you're done. See the attached example of a 5 x 5 grid with 100 mm size grid and 20 mm tubes. If you go to the Part Navigator and expand the 'User Expressions' item you will find all the expressions that you'll need to create any size grid that you desire.

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

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

 

[Toost]

The functionality of the sketcher pattern feature is the same in 8.5, i.e double click the patterned curves to edit the pattern. There might be some other difference but the way of editing is the same.

Regards,
Tomas