turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Femap Forum
- 1D elements Cross-Section Additional Properties

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

11-23-2015 09:01 AM

Hi,

I wanted to know how to obtain additional info for beam cross-section such as location of centroid, shear center etc in FEMAP. I am unable to get the above info from Property->Shape Section.

Patran has ability to provide the above (image 2) info as well as additonal information I needed.

Thanks...

7 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

11-24-2015 05:16 AM

Dear VN

With FEMAP the life is more easy, simply run command "**Tools > Section Property > Surface Property**" and select any surface cross section, then FEMAP will measure the cross-section properties of the selected surface. Inputs required for this command are the surface ID and the Y-Axis vector. The first point selected in the Y-Axis (or orientation vector) will also define the origin. FEMAP will then internally mesh the surface and use the Y-Axis vector and the Beam Cross-Section Generator to calculate the section properties. A typical result is the folloiwng:

Surface Section Properties Preparing Cross Section... Meshing Surface 10... Meshing Surface 10... Computing Properties... Orientation of Section Properties: Origin: X= 0. Y= 0. Z= 0. Y Axis: X= 0. Y= 1. Z= 0. Z Axis: X= 1. Y= 0. Z= 0. Section Properties: Area A= 12. Centroid (from Origin): Cy= 2.99999 Cz= 1.5 Moment of Inertia: Iyy= 16.9999 Izz= 55.9996 Iyz= 0. Principal Moment of Inertia: I1= 55.9996 I2= 16.9999 Radius of Gyration: Ry= 1.19024 Rz= 2.16024 Angle to Principal Axes: Ang= -4.05026E-12 Polar Moment of Inertia: Ip= 72.9994 Shear Center (from Origin): SCy= 2.99999 SCz= -0.75428 Shear Center (from Centroid): SCy= 0. SCz= -2.25427 Shear Area: Asy= 4.41981 Asz= 6.3263 Torsional Constant: J= 3.96134 Warping Constant: W= 80.881

The result includes reference to the chosen orientation as well as the section properties. FEMAP calculates the standard section properties such as area, moments of inertia, torsional constant, and shear area. In addition, principal moments of inertia, radius of gyration, angle to principal axes, and warping constant are output.

This command uses the same Beam Cross-Section Generator available under Model, Property (type Beam) Shape.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

11-24-2015 01:56 PM

Blas,

Thanks for replying. Is it possible to illustrate how to issue Section Properties command with 1D element? I am getting a prompt to select a surface but if I have just line elements, how can I proceed with the above command?

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

11-24-2015 02:14 PM

Hello!,

If you have the cross section dimensions then simply draw the geometry of the cross section in FEMAP (or import as solid from any CAD system):

- Draw the cross section profile with curve lines & arcs: use commands like
**GEOMETRY > CURVE - LINE > CONTINUOUS**, or click the**F9**key and draw line by line - Next define a boundary surface with curves using command
**GEOMETRY > BOUNDARY SURFACE > FROM CURVES**, - Finally convert the boundary surface in a PARASOLID surface using
**GEOMETRY > SURFACE > CONVERT**.

Once you have the surface geometry of the beam cross section created then issue command **TOOLS > SECTION PROPERTIES > SURFACE PROPERTIES**.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

11-26-2015 11:57 AM

Hi Blas,

Thanks for replying. It seems like the section needs to be created and the command used to obtain geometrical properties. At this moment, it seems like the method is tedious but over time it may turn out to be otherwise.

Anyways, I appreciate your response and help.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-05-2015 04:02 AM

Dear VN,

A great feature of future version of **FEMAP V11.3** for **BEAM CROSS SECTIONS** will be the additional information that will appear in the picture of the defined beam cross-section, placing the section properties in the window to the left of the picture, well done for the FEMAP guys!!.

Also, to help to understand how to input the dimensions of the beam cross section definition the new release of FEMAP V11.3 will include explicitly the dimension marks like in the following picture, great!!.

The same philosophy for the beam nastran sections:

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-06-2015 09:40 AM

Hello.**Blas** whether there is an opportunity to add to the standart profiles a new type of cross-section like this:

Adding and changing section by means *General Section-Surface* not always convenient

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

12-07-2015 08:49 AM

Great to find that v11.3 gonna include additional Beam C/S info. If FEMAP folks are reading this, please do consider including Shear Center information as well. It would be really helpful.

Any idea on ETA of v11.3?

Blas, thanks for letting us know. I am now excited about the next release

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc