Siemens NX 10 - Basic surface trouble 1

[philukuk]

Hello all,

I am currently having some trouble with a surface which I am working on.

I was wondering if someone could put me out of my misery!?!

I have attached the sketches I am using and two results of my attempts.
I have a feeling this is something simple but for some reason I am struggling to get my head around it.
I would like to get the process of this shape right as I will be doing a lot more of a similar shape.

I have attached some screen shots below.

http://files.engineering.com/getfil...-7c74-4e35-bccd-7e83a180adb0&file=sketch.tiff

http://files.engineering.com/getfil...fc-4e9f-bac4-9a255dd6eabc&file=attempt_2.tiff

http://files.engineering.com/getfil...b5-4155-8398-112319c3c3de&file=attempt_3.tiff

Many Thanks in advance.

 

[JohnRBaker]

Could you provide use with the part, or at least cut-off the end of it and upload that?

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.

 

[philukuk]

Sure,

http://files.engineering.com/getfil...5f-9d82-18d492e919e6&file=surface_trouble.prt

Thanks

 

[JohnRBaker]

Well I looked at your part and while I was able to create what I think is a usable surface (see the attached model) using Surface Thru Curve Mesh where the first 'Primary Curve' is a Point, it could have been better if the original model had been better.

That being said, you really need to clean-up your sketches. In fact, I would start over making sure that as you create the various sketches so that they all line-up and connect so that they can be use to create proper surfaces.

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.

 

[philukuk]

Thank you John,

I appreciate it, I have just completed the training for CAD/NX but will take onboard what you have said.

Thanks again.

Phil

 

[Xwheelguy]

Phil,

Surfaces are a garbage in, garbage out type of process in NX and most freeform modeling in general. If the input curves are not good quality, then the surfaces output will more than likely not be of good quality. Taking care to create smooth, clean curves at the beginning of the process will at least give you some hope in ending up with smooth, clean surfaces (fewer imperfections and/or issues down the road).

Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[MSPBenson]

Phil,

Although NX can produce surfaces using a point as construction, I would advise avoiding this technique if at all possible.
Using a point in a Through Curve mesh can (and often) create surfaces with tiny 'ripples' in them.
These surfaces are extremely problematic if you then try to offset them (including thicken).
Even if the topology is perfect and does not contain ripples the curve is tending towards zero so will not be practical to offset in one direction.
Also if you try and use a common export format like iges the result can produce a 'bow tie' effect where the output becomes un-trimmed.
My advice where you encounter 3 sides is to always create a fourth (usually by adding a trim of some sort). Also try to keep the angles between primary and cross above 45 deg (so don't try and split a tangent continuous edge into 2 to create an extra edge)
See the example part for the technique I would use to create the corner detail.

Mark Benson
Aerodynamic Model Designer

To a Designer, the glass was right on CAD.

 

[philukuk]

Thank you everyone,

MSPBenson wow! Thanks I have been trying to work through the process and can follow you up until Bridge Curve (19).

Could you possibly talk me through how and why you use the bridge curves and trim sheets??

Thanks

 

[MSPBenson]

Phil,

I'm not sure if you are aware, but you can step back through the model tree to see how the model is built.
If you right click on a feature in the part navigator you will see, about half way down, 'make current feature'.
If you make the bridge curve the current feature and then one by one follow the feature tree down by making the next feature the current one you will see the model being built 1 feature at a time (spline 20 is not required, I just forgot to delete it)
Alternatively you can use Edit>Feature>playback (from the main menu)
As mentioned in my post above the bridge and trims are added to split 1 edge into 2 edges. These are trimmed sympathetically to the other 2 edges to make a nice neat 4 sided patch.

Hope that helps.


Mark Benson
Aerodynamic Model Designer

To a Designer, the glass was right on CAD.