Document Type: FAQ
Original Author: Bentley Technical Support Group
Document Type: FAQ
Original Author: Bentley Technical Support Group
Presently, STAAD only reports the nodal stresses of the individual elements meeting at the node. In the Plate page of the post-processing mode, the lower table on the right hand side of the screen contains the element nodal stresses. However, the average value from all such plates connected to the node is not reported.Averaging is straightforward at joints that are only connected to one plane of plate elements and the loading is a normal pressure. However transverse shear will jump at a line if a line load is applied; so a single average would be inappropriate for that stress only. Similarly for stresses across a line of beams or walls or a line of bending moments; etc. If two walls and a floor meet at a joint there are 3 planes that should be treated separately. Also averaging should be separate for the same surface on either side of a wall to account for the stress discontinuity. At the common joint there would be 12 sets of stresses (4 plates on each of 3 surfaces).So averaging can be interrupted due to certain loadings, plates in other planes, and other members. Further complexity occurs for contours and corner stresses if a shallow curved surface is being averaged. Most likely the inplane stresses should be averaged separately from the bending stresses, without coordinate transformations, since the flat plate faceted surfaces are trying to simulate a smooth surface.The above considerations are not easily automated. REI hopes to implement at least some simple cases in a near future release.
TRESCA is 2.0 times TMAX. TMAX is the maximum inplane shear stress on a plate element. TMAX = 0.5 * max[abs((s1 - s2)) , abs((s2 - s3)) , abs((s3 - s1))] where s1 and s2 are the inplane principal stresses and the 3rd principal stress, s3, is zero at the surface. TRESCAT is the value for the top surface of the element. TRESCAB is on the bottom. Top and bottom are in accordance with the direction of the local Z axis. See the link http://www.reiworld.com/Search.asp?id=SP-1549for more information on the meaning of TOP and BOTTOM surfaces for plates. Example problem 18 in the examples manual shows the calculation of TMAX
For Mx, the unit width is a unit distance at the center of the element, parallel to the local Y axis. For My, the unit width is a unit distance at the center of the element, parallel to the local X axis. Attached is a diagram to clarify this. It is taken from section 1.6.1 of the Technical Reference manual.
SUPPORTS 1 TO 529 ELASTIC MAT DIRECT Y SUBGRADE 4
Your guess is a good one. You can model the support as an elastic mat foundation. To do that, you first need to know the subgrade modulus of concrete. One of the methods by which the modulus can be computed is using the following equation:Ks = Es / B ( 1 - PoissonRation * PoissonRatio ) ( Reference: Foundation Analysis and Design ( Fifth Edition ) by Joseph E. Bowels Page 503 , Equation 9-6a )In addition, if you want to make sure the concrete pedestal takes only compressive force, then specify the SPRING COMPRESSION command for those joints in the direction KFY.An example of this isSUPPORTS 1 TO 529 ELASTIC MAT YONLY SUBGRADE 987SPRING COMPRESSION 1 TO 529 KFYIf you have any anchor bolts attached to the baseplate, they can be modeled as spring supports (tension only).An example of this isSUPPORTS1000 TO 1004 FIXED BUT MX MY MZ KFY 5467SPRING TENSION1000 TO 1004 KFY
You do not have to assign any properties for solid elements. For solids, the only information required is their geometry (node numbers and their coordinates), and material constants (E, Poisson, etc.). You may refer to example problem 24 in the examples manual if you want details.
From the Select menu at the top, select the Plates Cursor. Then select the element for which you want the Z axis direction changed. From the Commands menu, select Geometric Constants followed by Plate Reference Point and give the coordinates of this point. Choose the Local Axis direction to point towards or away from the Reference Point. The Assign option should be set to "To Selection". Click on OK.
Yes, it is possible to do this. In Section 5.32.3 of the STAAD.Pro Technical Reference Manual, if you look at the syntax of the element pressure loading, you will find the following :element-list PRESSURE direction x1 y1 x2 y2In this syntax, (x1,y1) and (x2,y2) represent the corners of the region (on the element) over which the PRESSURE load is applied. However, if you omit the terms (x2,y2), the load will be treated as a concentrated force acting at the point (x1,y1), where x1 and y1 are measured as distances, from the centroid of the element, along the local X and Y axes, of the point of action of the load.Thus, if you want to apply a 580 pound force along the negative global Z direction at a distance away from the centroid of (1.3,2.5)feet along the local X & Y axes of element 73, you can specify the following commandsUNIT POUND FEETLOAD 1 CONCENTRATED LOAD ON WALLELEMENT LOAD73 PR GZ -580.0 1.3 2.5
Since there are several types of shear stress results we can get from STAAD, the expression "maximum shear stress" needs to be clarified. So, let us first see what the choices are :SXY - For any given element, this is the in-plane shear stress on the element and acts along the plate local X-Y axes directions.TMAX - This is the maximum inplane shear stress on the element and is a composite of SXY and the stress resulting from torsion MXY.SQX - This is the out-of-plane shear stress on the X face at the centroid of the element.SQY - This is the out-of-plane shear stress on the Y face at the centroid of the element.All of these results can be obtained in a report form, with additional options like sorting done in ascending or descending order for a user-defined set of elements and a user-defined set of load cases. As an example, do the following for getting a report of TMAX sorted in the order from maximum to minimum for all plates for load cases 4 and 5.Go to the post-processing mode. Select all plates. From the Report menu, select Plate Results - Principal stresses. Select TMAX, and set the sorting order from High to Low. Switch on "Absolute values" also to perform sorting based on Absolute values. Click on the Loading tab, and select just cases 4 and 5. Click on OK. A report will be displayed. Click the right mouse button inside the table, and select Print.
Among the various stresses resulting from the torsional moment MXY, the only stress which is considered in TMAX is the shear stress. There are other stresses such as warping normal stresses which do not get represented in TMAX.TMAX is the maximum inplane shear stress on an element for a given load case. It represents inplane shear stresses only. It contains contributions from the direct inplane shear stress SXY as well as the shear stress caused by the torsional moment MXY. Example 18 in the examples manual shows the derivation of TMAX from SXY and MXY.While on the subject of shear stresses, one must note that the plate is also subjected to out-of-plane shear stresses SQX and SQY, which do not have any representation in TMAX.
These are the principal stresses SMAX and SMIN. Principal stresses are a blend of axial stresses (also known as membrane stresses SX and SY), bending stresses (caused by MX and MY) and inplane shear stresses (SXY). Since the bending stresses have distinct signs for the top and bottom surfaces of the element, the principal stresses too are distinct for top and bottom. The derivation for principal stresses is shown in example 18 of the STAAD Examples manual.
The answer to the question is Yes. The following are the major steps involved in the modelling and design of mat foundations using STAAD. 1) The mat foundation has to be modelled using finite elements. If the length and width of the mat are atleast 10 times larger than its thickness, plate elements can be used. If not, one may use 8 noded solid elements. The remainder of the structure involving the beams, columns and slabs also has to be modelled along with the mat. If beams share a common boundary with the mat and slabs, to ensure the proper transfer of load between the beams and the mat & slabs, the mat & slabs have to be divided into several elements, the beams have to be divided into several members, and the elements and members must share common nodes. 2) Generally, the supports for the mat are derived from the subgrade reaction of the soil. Using this attribute, and the influence area of each node of the mat, the spring constant for the supports may be derived. STAAD contains an automatic spring support generation facility for mat foundations. One may refer to Section 5.27.3 of the STAAD.Pro Technical Reference Manual for details on this type of support generation.3) Soil spring supports generally tend to be effective against resisting compressive forces only. They are ineffective in resisting uplift. This type of a unidirectional support requires those springs to be assigned an attribute call SPRING COMPRESSION.4) The loads on the mat and the rest of the model have to be specified. Then, the structure has to be analysed. This will generate the plate stresses and corner forces needed to design the mat. 5) You can then use the program's concrete design ability to design the individual elements which make up the mat. The only tedious aspect of this is that the program can presently design individual elements only. The task of taking the reinforcement values from each element and assembling the reinforcement picture of the overall mat has to be done by you manually. You may wish to look the information posted at the following links for details on the issues involved in designing individual elements. http://www.reiworld.com/Search.asp?id=SP-1549 http://www.reiworld.com/Search.asp?id=SP-1791 http://www.reiworld.com/Search.asp?id=SP-1792 We suggest you take a look at example problem number 27 in the STAAD.Pro examples manual for guidance on analysing mat foundations. In that example, the aspects explained in steps 1,2, 3 and 4 above are illustrated. Example problems 9 and 10 discuss concrete design of individual plate elements.
No, they do not have to. However, for the overall slab or wall, if the span in either direction is less than 10 times its thickness, then the slab or wall becomes more like a solid than like a plate; and thick plate theory may not be adequate. In that case, 8-noded solid elements may be necessary.
The element nodal stresses are obtained as the value of the stress polynomial at the coordinates of those joints. Stresses in an element are most accurately determined only at the center of the element (in the middle of the joint displacement locations used in calculating that stress). The stress values calculated at the nodes will only be approximate (only the displacements of the joints from this one element are used in calculating the stress). Stresses at a joint would be improved if the stresses from the other elements at the joint (on the same surface) were averaged. Consequently, the comparison you suggest is not feasible.A better alternative would be to compare the forces at the node rather than the stresses at the node. However, to do so, you will require version 2001 of STAAD.Pro.In STAAD.Pro 2001, the output for the commandPRINT ELEMENT FORCESconsists of the 3 forces and 3 moments at each of the nodes of the elements, reported in the global axis system. Thus, the output will consist of FX,FY,FZ,MX,MY,MZ with the 3 forces having units of force (not stress) and the 3 moments have units of moment (not moment per unit width). If you add up the values at the nodes of those elements which are connected to the support, those values must be equal to the support reaction.Another consideration is the way in which element loads are evaluated and used. Staad computes the equivalent forces at the corner joints (same total force, center of force, and direction). The remainder of the analysis and results are as if you had applied the loads as joint loads rather than as element loads. Two exceptions, temperature loads are applied internally to the element and plate releases will affect the load distribution to the joints.Say you have a wall with uniform pressure. Half of the load on the elements along the base will be applied directly to the base, the other half is applied to the line of joints at the top of these elements. So the internal transverse shears are too high at the top of the element. The transverse shears are OK at the center and too small at the base. The same will be true for the element force output of transverse forces. However, the reactions will have the entire force. A finer mesh in general, and near the base in particular, will improve the element stress and load distribution.
Product TechNotes and FAQs
Structural Product TechNotes And FAQs
Bentley Technical Support KnowledgeBase
Bentley LEARN Server
Bentley's Technical Support Group requests that you please confine any comments you have on this Wiki entry to this "Comments or Corrections?" section. THANK YOU!