How to model a non standard composite section?

Are you planning to model the arch as a series of straight line members?

Since the rules for designing this non-standard section are not implemented in STAAD, specify the properties needed for the analysis and do the analysis. Once you get the member end forces and section forces, you'll have to do the design on your own.

For calculating and assigning the properties, here are 2 ways.

1) Using a program such as Section Wizard, calculate the section properties. The four basic properties the program needs are

AX = Area of cross section

IX = Torsional Constant

IY = Moment of inertia for bending about principal Y axis

IZ = Moment of inertia for bending about principal Z axis

If you wish to consider shear deformation also, you have to calculate AY and AZ also, which are the areas for shear deformation along the principal Y and Z axes respectively.

2) After you have calculated these properties, you can do one of the following to assign them in STAAD.

a) the manual method

Assign the property using the PRISMATIC option, as explained in section 5.20.2 of the Technical Reference manual. The command syntax for this is

UNIT .. ..

MEMBER PROPERTY

member-list PRISMATIC AX f1 IX f2 IY f3 IZ f4 AY f5 AZ f6

where f1 through f6 are the values you calculated in the previous step.

For example,

UNIT CMS

MEMBER PROPERTY

14 TO 23 PRIS AX 36 AY 23 AZ 24 IX 179 IY 653 IZ 875

b) If you are using section wizard to calculate the properties, those properties can be exported to a User Table file. That user table file can then be imported into STAAD and the property assigned from that user table. The property may be exported either as a PRISMATIC section, or a GENERAL section

Dear SKLose, Thank you for your helpful comments.

Yes, I am trying to do grid analysis with the main portal as series of straight line forming an arch.

Let say I will calculate the properties of the section for bending and shear analysis (Ax, Ix, Iy, Iz, Ay & Az) and put these parameter with Prismatic or General Section command. What I want to know more does the Staad require us to define the material properties (i.g. elasticity) to be able to perform the analysis? if yes, which properties for this composite section should be used? (concrete or steel)

I notice in the "section wizard" tool that the sectional coordinate has different sign convention with what is used in Staad General or Prismatic sectional coordinate. In case I want to import an irregular section with a complex shape, will this importing process will automatically converts this different sign convention?

Demy

DEMY,

You asked :

What I want to know more does the Staad require us to define the material properties (i.g. elasticity) to be able to perform the analysis?

Answer:

Yes. Every member, plate element and solid element must have a material assigned to it.

-------------------------------------

You asked :

if yes, which properties for this composite section should be used? (concrete or steel)

Answer:

When you compute the properties of the composite section, and if there are 2 materials (say A and B), structural mechanics theory says that for the component made of the second material, the dimensions need to be transformed to the first material by dividing the "width" by the modular ratio (Ea/Eb). This will result in the gross section being represented through a single material (material A I think) When you do that, you are going to get the properties based on a single material.

So, to ensure consistency between the properties assigned to a member, and the material assigned to that member, the material must be the same as the one you chose during that transformation I mentioned in the above paragraph. For example, if it is a section made of concrete and steel, and you calculate the properties by transforming the concrete component to an equivalent steel component, the material that you assign too must be that of steel.

Here is another way of looking at it. Axial stiffness is represented by EA/L where E is Young's modulus and A is the cross section area. Flexural stiffness is represented using terms like 12EI/L^3, 6EI/L^2, 4EI/L, 2EI/L, etc., where E is the Young's modulus and I is the moment of inertia. Hence,for a composite section, the E and the I must be based on the same single material. If you calculate A and I based on concrete, you must assign it the E of concrete. If you calculate A and I based on steel, you must assign it the E of steel.

----------------------------------

You asked :

I notice in the "section wizard" tool that the sectional coordinate has different sign convention with what is used in Staad General or Prismatic sectional coordinate. In case I want to import an irregular section with a complex shape, will this importing process will automatically converts this different sign convention?

Answer :

See the answer at the following thread

communities.bentley.com/.../187381.aspx

Hi Kris,

Thank you, I got your point for the equivalent section properties

I post my case with the Section Wizard in the above thread, please put some solution.