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