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face types in NX 1
- Thread starter helperug
- Start date
Are you just tring to find, in which command this Detail Filter is?
The Detail Filtering for faces will show everytime, you will use Class Selection.
[ul]
[li]For example, create a body. Then select edit->object display command. Just don't select anything prior selcting this command.[/li]
[li]Now, the Class selection window will appear.[/li]
[li]In the Filters group, you will see the Type Filter option. Click on the icon for Type Filter.[/li]
[li]Now, new dialogbox will appear. Select Face in this dialogbox.[/li]
[li]Below, you will have the option for Detail Filtering. Click on this button.[/li]
[li]In new dialogbox, you will have those face types, that you are tring to find.[/li]
[/ul]
This Class Selection dialogbox will appear in many commnads, like Object Display, Move to Layer, etc.
The Detail Filtering for faces will show everytime, you will use Class Selection.
[ul]
[li]For example, create a body. Then select edit->object display command. Just don't select anything prior selcting this command.[/li]
[li]Now, the Class selection window will appear.[/li]
[li]In the Filters group, you will see the Type Filter option. Click on the icon for Type Filter.[/li]
[li]Now, new dialogbox will appear. Select Face in this dialogbox.[/li]
[li]Below, you will have the option for Detail Filtering. Click on this button.[/li]
[li]In new dialogbox, you will have those face types, that you are tring to find.[/li]
[/ul]
This Class Selection dialogbox will appear in many commnads, like Object Display, Move to Layer, etc.
- Thread starter
- #3
@svenbom,
thanks on reply, I am familar with filtering by geometrietypes in Nx.
Im looking for deeper information
- structure
- how to handle
- what is good for
- differences of these face types.
the help tells nothing
sorry new in NX
regards
Erwin
thanks on reply, I am familar with filtering by geometrietypes in Nx.
Im looking for deeper information
- structure
- how to handle
- what is good for
- differences of these face types.
the help tells nothing
sorry new in NX
regards
Erwin
JohnRBaker
Mechanical
Why exactly do you need that sort of information? I'm not aware of anything in the documentation which will give you a 'course of instruction in Geometric math-forms' used by NX. However, if you wish to learn something about a specific face on your model, go to...
Information -> Object...
...set the filter to 'Face' and select the Face(s) of interest and you will get information about the type of face selected and any dimensional parameters associated to that particular face based on the math-form of the geometry that the face was created using be it some canonical form or if it were a more general B-surface.
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.
Information -> Object...
...set the filter to 'Face' and select the Face(s) of interest and you will get information about the type of face selected and any dimensional parameters associated to that particular face based on the math-form of the geometry that the face was created using be it some canonical form or if it were a more general B-surface.
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.
- Thread starter
- #5
thank you John on reply,
there are some cases where for example
the analysis->shape->show pole command not working on face extruded from a complex 3d spline.
On the extracted face with another face type show pole works???
sorry new in NX
regards
Erwin
there are some cases where for example
the analysis->shape->show pole command not working on face extruded from a complex 3d spline.
On the extracted face with another face type show pole works???
sorry new in NX
regards
Erwin
JohnRBaker
Mechanical
Have you tried...
Information -> B-surface...
...and then toggle ON all of the options and select the face(s) of interest?
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.
Information -> B-surface...
...and then toggle ON all of the options and select the face(s) of interest?
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.
- Thread starter
- #7
-
1
- #8
JohnRBaker
Mechanical
These faces are what's known as TABCYL's or 'Tabulated Cylinders'. They are one of several so-called 'canonical forms'. Others types include Planar, Spherical, Conical, Cylindrical, etc. In NX, faces are given names based on a combination of how they are created and what their math-forms are. And contrary to what you might think, the faces of your model are NOT B-surfaces and to say that they are free-form would be incorrect as well. Now we COULD have designed NX so that faces like this were created as B-Surfaces but it's not necessary and it would result in a model much more complicated than it needs to be. For mosts types of operations there are closed-solutions when working with faces which are represented as a 'canonical form' which means that no approximations have to be made, unlike what happens virtuallyt ALL the time when working with B-surfaces.
This is just the way NX works, we never create geometry that's more complicated than it NEEDS to be and we do this for several reasons. One, it just makes part files smaller. Second, they update faster since there are no complex approximation routines which have to converge on a solution since in most cases there is an algebratic/analytic solution which will give you an exact answer immediately. Third, this means that the code will run faster and use less system resource (i.e. memory) to perform computations using canonical geometry. BTW, the same thing would happen if you were use one of those splines to create a Revolve feature, the face would be another 'canonical form' known as a 'Surface of Revolution'.
Now don't worry, if for some reason an operation that you use later on, like X-Form to change the shape of one of the faces of your model, will only work if the face was actually a B-Surface (something that WAS a limitation until NX 7.5), NX will internally create the necessary B-Surface data needed so that you could use X-Form to modify the shape of the 'Extruded' face. And it will do this without actually changing the original Extrude feature which means that it can still be edited by simply modify either the referenced profile curves or by editing the parameters of the Extrude feature itself.
Let me give you some advise; don't worry too much about exactly what math-forms NX is using when creating geometry as it will take care of any of the internal machinations that needs to be done when that geometry is acted upon by some downstream application. If the internal math-form needs to be altered, NX if quite capable of doing that without either any special intervention or actions by the user and in most cases, without having to destroy the original design intent of the features which the user created.
For some more information about Tabulated Cylinders and other common math forms used in CAD systems, click on the link below and when the PDF document opens, search for "tabulated Cylinder". An interesting point here is that the 'example' figure that they use to show what a 'tabulated cylinder' shape would look like bears a striking resemblance to the shape of the 'Extrude' faces of your 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.
This is just the way NX works, we never create geometry that's more complicated than it NEEDS to be and we do this for several reasons. One, it just makes part files smaller. Second, they update faster since there are no complex approximation routines which have to converge on a solution since in most cases there is an algebratic/analytic solution which will give you an exact answer immediately. Third, this means that the code will run faster and use less system resource (i.e. memory) to perform computations using canonical geometry. BTW, the same thing would happen if you were use one of those splines to create a Revolve feature, the face would be another 'canonical form' known as a 'Surface of Revolution'.
Now don't worry, if for some reason an operation that you use later on, like X-Form to change the shape of one of the faces of your model, will only work if the face was actually a B-Surface (something that WAS a limitation until NX 7.5), NX will internally create the necessary B-Surface data needed so that you could use X-Form to modify the shape of the 'Extruded' face. And it will do this without actually changing the original Extrude feature which means that it can still be edited by simply modify either the referenced profile curves or by editing the parameters of the Extrude feature itself.
Let me give you some advise; don't worry too much about exactly what math-forms NX is using when creating geometry as it will take care of any of the internal machinations that needs to be done when that geometry is acted upon by some downstream application. If the internal math-form needs to be altered, NX if quite capable of doing that without either any special intervention or actions by the user and in most cases, without having to destroy the original design intent of the features which the user created.
For some more information about Tabulated Cylinders and other common math forms used in CAD systems, click on the link below and when the PDF document opens, search for "tabulated Cylinder". An interesting point here is that the 'example' figure that they use to show what a 'tabulated cylinder' shape would look like bears a striking resemblance to the shape of the 'Extrude' faces of your 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.
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