problem through curve mesh surface 2

[skanskan]

Hi.

I'm trying to create this hook with a through curve mesh,
selecting first the primary curves (adding new sets)
and later the cross curves.

But I can't get it.
what's my problem?

It says the curves don't intersect but they seem to do it.
What are the red points?
This is a simplified version with splines, the original one was with circles and exact dimensions, but it didn't work either.

regards.

 

[skanskan]

And the file.

 

[skanskan]

OK, I got it, changing the tolerance.
Anyway, any advise would be wellcome.
And it just generates half of the model.

 

[skanskan]

Another related question...
How do you select only a part of curve?
Imagine you created on a sketch an arc, straight line or a spline, and you need to select (to create a mesh or anything else, from outside the sketch) only part of that arc, just till it's intersection with another curve (maybe in a different sketch).

 

[JohnRBaker]

OK, I assume that the two long splines are your 'cross curves', correct?

If so, simply pick one for the 'first' curve, the other curve for the 'second' curve and then RESELCT the first curve so that it also becomes the 'THIRD' curve so that it closes the volume. If you pick just two curves you've really only gone 'half-way around' the model.

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.

 

[skanskan]

Yes, I pick all the curves.
When I mean it only makes half of the surface I mean it's halved "through" the plane ZX, and I need to mirror it. I don't know if this is the expected behaviour if I'm selecting whole "circles" as a primary curves and not only a half.


I don't know if I should say through or along or...

 

[JohnRBaker]

This is what I got doing it the way I described (see attached).

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.

 

[SvenBom]

To get the full solid body, it Works exactly as JohnRBaker has described.
1. in through curve mesh, select all the circles as your Primary Curves
2. as first Cross curve, select one long spline.
3. for the second Cross curve, select the other long spline. Now, you will have only the half of the body.
4. now, for the third Cross curve, select the first one again (the one from the second step). Now, you will get the full body.

And about selecting only the part of the spline/curve (from intersection to intersection).
1. when in command (extrude, revolve, through curve mesh, etc.), click on the 'Stop at Intersection' command. The command is right to the 'Curve Rule' menu in the Selection Bar.
2. now click on the curve. Only the part of the curve will be selected. From one intersection to another intersection point.

I have attached your model, as I did it.
The first 'Through Curve Mesh (6)' is for the first question. I guess, it is the same as JohnRBaker already described.
The second 'Through Curve Mesh (7)' is for your second question. You can see, that I have been using 'Stop at Intersection' command with all Cross Curves.

 

[Toost]

Here's the reason for your issues, All the highlighted intersections are above the default tolerance.
The largest deviation is in the sketch of the two long splines.( not visible in the attached image) there is a 0.2 dimension between the arc and the spline.

Tighten the intersections between the curves rather than opening up the tolerance.
If you open up the tolerance to say 1.0 mm, then the resulting surface can at any location be plus/minus 1 mm from the curves used.- Depending on how you build your model you can have a 2 mm gap between adjoining surfaces.
Imagine you have an arc which is used for two surfaces , one surface to the left and one to the right of that arc, the left surface is interpolated such that it becomes minus 1 and the right becomes plus 1.

In the sketch of the two long splines, the splines are, when i edit them defined by poles. In this case a definition by points would have been better since you could have snapped all the intersection points.


Regards,
Tomas

 

[skanskan]

A last question.
While being on a sketch you can select end points at lines from straight other sketches (to create an intersection).
But if you want to slect the extreme of a circle or arc you can't select it because is not an end point.
I use to create the "project curve" from the sketch to get it.
Is there any other way?

 

[JohnRBaker]

Are we talking about something like the sketch in the attached file?

I have an arc where I've constrained the end point of a Line to always be at the highest point on an Arc. I did this by created a horizontal Line (reference status) tangent to the Arc, I then created a Point at the intersection of the reference Line and the Arc and then constrained the end of the Line to be coincident with the Point. If you move the Arc or change it's size the end of the Line remains at the 'extreme' point of Arc.

Note that there is also a new (NX 8.5) function for doing this same thing outside a sketch, in fact using any object, 2D or 3D and getting a so-called 'extreme' Point relative to any frame of reference. It's an item found on the Analysis menu titled 'Measure Extremes'.

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.