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Reg.surface to solid 2
- Thread starter sudhakarn
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This procedure can at times be confusing/involved if you're not familiar with basic practices typically used for surface modeling. The following are the general steps to follow as each model can be a little different, depending on how the surfaces are modeled prior to converting the surface model to a solid model. It's also a good idea to be aware there are usually more ways than one to get from point A to point B using NX.
Create and, if necessary, trim surfaces to completely enclose a volume (meaning the surfaces are water tight) then use the Sew command to sew the surfaces together. In order for this to be successful, the surface edges must be less than or equal to the modeling distance tolerance. NX will typically flash "Solid Body created" in the Cue/Status line if the Sew successfully converts the surfaces to a solid body. Alternatively, you can set your preselection filter to Solid Body and hover your mouse over the surfaces - if they highlight, you know you have a solid. You can also hover over the body and wait for the 3 dots to appear, select the body and see if Solid Body appears in the Quick Pick menu that pops up.
Tips:
[ul]
[li]When performing the Sew command, if you click Apply rather than OK, NX will highlight all non-sewn edges which makes it a bit easier to see if you have any unwanted gaps between surface edges.[/li]
[li]Examine Geometry will also display gaps between surface edges after using Sew (Sheet Boundaries -> check Highlight Results).[/li]
[li]I recommend running Examine Geometry (Set All -> Window select around your entire surface model but do not include any curves or other construction geometry) before using Sew to check all of your surfaces in case you may need to fix any issues with the surfaces before creating a solid body. Repeat Examine Geometry as needed and at least when the model is 100% completed and fix any major issues (Misaligned, Consistency, Self-Intersection, Spikes/Cuts).[/li]
[/ul]
Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.4.2
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M
Create and, if necessary, trim surfaces to completely enclose a volume (meaning the surfaces are water tight) then use the Sew command to sew the surfaces together. In order for this to be successful, the surface edges must be less than or equal to the modeling distance tolerance. NX will typically flash "Solid Body created" in the Cue/Status line if the Sew successfully converts the surfaces to a solid body. Alternatively, you can set your preselection filter to Solid Body and hover your mouse over the surfaces - if they highlight, you know you have a solid. You can also hover over the body and wait for the 3 dots to appear, select the body and see if Solid Body appears in the Quick Pick menu that pops up.
Tips:
[ul]
[li]When performing the Sew command, if you click Apply rather than OK, NX will highlight all non-sewn edges which makes it a bit easier to see if you have any unwanted gaps between surface edges.[/li]
[li]Examine Geometry will also display gaps between surface edges after using Sew (Sheet Boundaries -> check Highlight Results).[/li]
[li]I recommend running Examine Geometry (Set All -> Window select around your entire surface model but do not include any curves or other construction geometry) before using Sew to check all of your surfaces in case you may need to fix any issues with the surfaces before creating a solid body. Repeat Examine Geometry as needed and at least when the model is 100% completed and fix any major issues (Misaligned, Consistency, Self-Intersection, Spikes/Cuts).[/li]
[/ul]
Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.4.2
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M
I am not sure i understand the question.
A "solid body" is in fact a shell of surfaces.
The "solid" definition is that these surfaces, from now on "faces", are connected in a schema such that the solid modeler (the cad system) knows which faces are adjacent,
it knows which faces share a common edge, and in the opposite direction, the edge knows what faces it belongs to. - when you pick an edge to apply a blend, the cad system will because of this select the faces that should be tangent and should be trimmed to the new blend surface, the new blend face should produce new edges where it meets the existing faces. etc etc.
But, there is nothing inside the solid.
The difference between a "sheet body" and a "solid body" is that there is no volume inside a sheet body because there is no such thing as "inside". A solid body encloses a volume.
the definition of the volume is that all surfaces / faces has an in-side and an out-side. ( a normal which is + in one direction and - in the opposite direction.)
On a solid body, all faces have the normal + out from the volume. This way the system can calculate the enclosed volume.
Is this relevant to the question ?
Regards,
Tomas
A "solid body" is in fact a shell of surfaces.
The "solid" definition is that these surfaces, from now on "faces", are connected in a schema such that the solid modeler (the cad system) knows which faces are adjacent,
it knows which faces share a common edge, and in the opposite direction, the edge knows what faces it belongs to. - when you pick an edge to apply a blend, the cad system will because of this select the faces that should be tangent and should be trimmed to the new blend surface, the new blend face should produce new edges where it meets the existing faces. etc etc.
But, there is nothing inside the solid.
The difference between a "sheet body" and a "solid body" is that there is no volume inside a sheet body because there is no such thing as "inside". A solid body encloses a volume.
the definition of the volume is that all surfaces / faces has an in-side and an out-side. ( a normal which is + in one direction and - in the opposite direction.)
On a solid body, all faces have the normal + out from the volume. This way the system can calculate the enclosed volume.
Is this relevant to the question ?
Regards,
Tomas
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- #4
Just to be clear and nothing against what Tomas posted above, but "sheet body" can be used in reference to either a single surface or multiple surfaces that have been Sewn (stitched) together to form a larger surface body which will appear as a single connected body to the software. Terms used by experienced modelers can sometimes be confusing to those that may not be as experienced.
Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.4.2
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M
Tim Flater
NX Designer
NX 11.0.1.11 MP8
GM GPDL 11-A.3.4.2
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M
- Thread starter
- #5
What version of NX?
Search for 'make solid' in the command finder. If you have a watertight sheet body, this command will convert it to a solid. I know it is available in NX 11, might also be in NX 10.
www.nxjournaling.com
Search for 'make solid' in the command finder. If you have a watertight sheet body, this command will convert it to a solid. I know it is available in NX 11, might also be in NX 10.
www.nxjournaling.com
If I understand correctly,You have a model which is build up out of surfaces (Maybe imported step or Iges?) Which is not a real Body.
You can try following;
"Unsew" one of the faces and then "Sew" it back again (both commands you can find in the combine group where you will also find Unite etc..)
Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
Building new PLM environment from Scratch using NX12 / TC11
You can try following;
"Unsew" one of the faces and then "Sew" it back again (both commands you can find in the combine group where you will also find Unite etc..)
Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2
Building new PLM environment from Scratch using NX12 / TC11
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