Tangent Junction Between Solids

[kr7530]

I am still relatively new to NX, any help is greatly appreciated.
Is there an easy way to create a tangent transition between the face of one solid to the face of another?
Right now I create individual surfaces, sew them and unite the three solids together.
A function similar to what "Multi-sections Solid" does in Catia.

Thanks,
Kevin
NX8

 

[Xwheelguy]

Some of the "through curve" commands more well-known for surfacing can be coaxed into outputting solid bodies. Through Curves and Through Curve Mesh can accomplish this - you will still have to Unite the solids separately. Make sure you expand all the options and read the documentation when you're wanting to clarify what anything does. If you want tangency, your input curves will have to at minimum meet tangency prior to creating the solid body (transitional body).

Hope this helps.

Tim Flater
NX Designer
NX 9.0.2.5 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JohnRBaker]

Can you provide at least a picture of the two solids that you're attempt to 'transition' between? Of course the actual part file would be better.

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.

 

[kr7530]

John,

Sorry for the delay, I have attached a file. The red portion is what I am after, tangent and with minimum geometry. The attached file was created in catia, I only had to select the two faces to get what is shown. In NX I would do four "Bridge Curves", four "Through Curve Mesh" surfaces, two "Extract Body"(s), sew them together and unite the three.

Thanks,
Kevin

 

[JohnRBaker]

Attached is how I would do this using NX. There are actually two solutions, one using a simple Surface Thru Curves (the Blue body which is currently hidden) which technically meets your criteria of creating a transition solid which is 'Tangent' to the original solid blocks but the shape is not quite the same as your original Catia feature. For that I created a second body (the Green visible body) using the Swept function with a single Arc as the Guide Curve so as to assure that the result is a 'circular' section, which I suspect is what you're actually looking for.

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.

 

[kr7530]

Thanks John! That is a big help, I figured there had to be an easy way to do it.

Thanks again,
Kevin