Slab Element in Staad

Re: Slab Element in Staad

SKLose — Thu, 05 May 2011 15:19:20 GMT

hmmbe,

You asked if it is realistic to release a beam at just one end. A release is simply a reflection of the connection details at that joint. So, there should be no problem with a release at one end, if the connection at that end represents a condition which is different from the default.

sureshprsharma,

Using master-slave to prevent axial deformation sounds like a logical approach, provided the member also is parallel to one of the global axes. This is because the master-slave feature in STAAD allows for linkages to be along the global axes only.

Re: Slab Element in Staad

sureshprsharma — Tue, 03 May 2011 03:52:46 GMT

Dear SKLOse,

I refer to your posting dtd. Mar 25 2011. Is it not possible to control the differential displacement of the two nodes of the beam in the local X direction with the help of Master Slave so that axial force is not developed in the beam?

Re: Slab Element in Staad

hmmbe — Tue, 26 Apr 2011 12:03:15 GMT

Is it realistic to release the beam at one end ?

Is it due to the method of reporting of STAAD ?

Re: Slab Element in Staad

SKLose — Fri, 25 Mar 2011 05:08:16 GMT

The reason a beam develops an axial force is, the two ends of a beam move by different distances resulting in a relative displacement along the local X axis between the 2 ends. So, if you can prevent or minimize this relative deformation, the axial force can be prevented.

To achieve this, you'll either have to release FX at one end, or provide a very large value for AX (the cross section area). You can find a discussion on a similar topic at

communities.bentley.com/.../166243.aspx

Re: Slab Element in Staad

hmmbe — Thu, 24 Mar 2011 22:49:36 GMT

Hi All,

When modeling like this, there is a large axial force in the beams, which is not realistic

How can we overcome this problem ?

Re: Slab Element in Staad

SKLose — Fri, 26 Nov 2010 19:53:32 GMT

The reason I didn't suggest ELEMENT RELEASES is because when you release an element, it is not just the transfer of forces/moments between that element and the beam it is attached to that is halted, but also between that element and other elements it is connected to at that node. Since the elements form part of a single slab, you don't want a release between adjoining elements.

The element design feature available through the DESIGN ELEMENT command in the STAAD command file has two drawbacks in my opinion. a) Design is done only for MX and MY. Important checks like one-way shear and punching shear are presently not done. b) In the case of an irregular mesh where the elements can have local X and Y pointing in various directions, there is no common line of reference about which design is done. Instead, design is done for MX and MY as they are obtained from each element with no transformation of axis.

Both these limitations are overcome by using the advanced slab designer which is a very targeted solution for folks doing slab design. For those who don't have RAM Concept, there is another way. In the Concrete Design tab, which most people think is just for beam and column design, there is a slab design component too, though not as comprehensive as RAM Concept.

Re: Slab Element in Staad

sureshprsharma — Wed, 24 Nov 2010 07:30:32 GMT

Dear Lose,

In paragraph 2 of your posting you have suggested to place the slab/plate in such a manner that top of slab and beam is at one level (global Y) with the nodes of beam and slab connected through master slave with appropriate rigidity so as to simulate the condition of simply supported. I do not find anything wrong with what you have suggested except that the modeling would be a bit complicated. In my view let the modeling be carried out on the lines of what has been advised by you in paragraph 1 of your posting and release the nodes connecting the beam and slab to simulate the condition of simply supported slab. If you do not agree with me, I would welcome your comments .

2. Is advanced slab design the only option to design slab? Staad is also designing slab as per some country code and giving output for reinforcement/steel for the sagging moment in the middle of the slab. It is also outputting moment at the nodes. What I feel the output generated by Staad in respect of RCC plate/slab almost satisfies 75% of the requirement of the designer to create quick design for the slab. I do not mean that further improvement in the design output for the slab is not required. As I have so far not come across advanced slab designer I am not in position to draw a comparison.

Re: Slab Element in Staad

SKLose — Sun, 21 Nov 2010 09:57:29 GMT

If by FIXED, you are referring to a monolithic connection between the beam and slab, here is a way to simulate that. Model the slab using a mesh of plates. Subdivide the beam into several segments. Ensure that those segments and elements are connected to each other at all those nodes which lie along the boundary between the beam and slab. The default connection between a beam segment and a plate element is treated by STAAD as one through which all three forces (FX, FY and FZ) and all 3 moments (MX, MY and MZ) are transmitted to each other which is what you would expect from a monolithic connection. Hence, other than the properties, material data and loads, there is nothing extra that you need to assign.

If the connection is not monolithic, meaning, if the slab is simply resting on the beam and does not transfer any moments to the beam, you could model the beam and slab at the elevations of their respective shear centers (or centerlines if that's what you prefer). This too requires that the slab is meshed and the beam is segmented. Then, use the master-slave feature to link the beam segment nodes to the element nodes along their boundary. The link will be just for FX, FY and FZ. By leaving out MX, MY and MZ, there will be no moment transfer. Without this additional step, the slab and beam would be identified as being physically separate entities with no connection, and no load transfer would be possible.

For designing the slab, the quickest way is to use the link between STAAD.Pro and RAM Concept. In the STAAD.Pro GUI's modeling mode, look for the tab called Advanced Slab Design. After the analysis, click on this page to launch the RAM Concept program if you have a license for it. If you don't have RAM Concept, you'll have to take the results from all those elements and design the slab manually, which can be quite tedious.

Re: Slab Element in Staad

Himmatlal Chavda — Fri, 19 Nov 2010 10:44:41 GMT

yes i know the said thing but in actual practice we have different conditions for plate such as simply supported, fixed etc. then in space frame with the model say 3*3 bay both sides and height of building say 20 meter then in that case if i am using the plate element and applying the pressure then how to assigned the different conditions of plate. i think i have to separately design it or what ? The building may be of composite type

Re: Slab Element in Staad

sureshprsharma — Fri, 19 Nov 2010 00:44:15 GMT

Your question is very brief and general. It is not posible to furnish the full particulars. Only few lines I can spell out is that you will have to assign thickness and material property to plate. I believe you are aware of creating plates. Apply pressure as per plate load item. But before applying the load, plate has to be meshed so that plate load is transferred to the beam through the common nodes between plate and beam. I will suggest you to take the help of Technial Reference Manual and Staad Graphical to clear your doubts. One more thing that I feel it is better to simulate plate with the floor load and Master slave .If you are not applying lateral loads Master slave also may be omitted. Meshing of plate leads to poor management with the model.

sureshprsharma