Applies To 
   
  Product(s): STAAD.Pro
  Version(s): All
  Environment:  N/A
  Area:  Modeling & Postprocessing
  Subarea:  Plates and Solids
  Original Author: Bentley Technical Support Group
   

 

 

 

 

 

 

 

  

  1. Is there a way to obtain the average stress at a node where several plate elements meet?
  2. In the plate element stress results, what do the terms TRESCAT and TRESTAB stand for? How are they calculated?
  3. I am modelling a concrete slab using plate elements. I am looking for the moments in the slab at the center of each element. I noticed that the output gives the bending moments per unit width. What is the per unit width? Would that be the thickness of the plate element?
  4. I have modeled a 40" x 40" column base plate with (4) 12" dia. pipe columns on it (equally spaced in both directions). How do I tell STAAD that the base plate will be on a concrete pedestal (f'c = 4.0 ksi)?
  5. How do you assign properties to solids?
  6. I would like to change the direction of the local Z axis of an element so that it points in the opposite direction. How do I do it?
  7. Is it possible to apply a concentrated force on the surface of an element? The point where the load acts is not one of the nodes of the element, as a result of which I cannot use the JOINT LOAD option.
  8. How can I find the maximum shear stress on my plate element model?
  9. The plate element results contain a term called TMAX. Is TMAX the best representation of the total stresses resulting from the torsion on the element?
  10. In the post processing mode - Results menu - Plate Stress Contour, there are two options called Max Top and Max Bottom. Are these direct stresses or flexural stresses?
  11. Can STAAD.Pro be used in designing a mat foundation?
  12. When modelling plate elements, should the individual elements satisfy any minimum requirements for the ratio of the length of their side to their thickness?
  13. I have a model where supports are defined at the nodes of some of the plate elements in the structure. If I divide the support reaction values by the thickness, length etc., of the side of the elements adjacent to the support, shouldn't the values match the ELEMENT NODAL STRESSES?
  14. Why shear stresses are not included in the Von Mises stresses for solid elements?
  15. How to change the local axis orientation X and Y for plates ?
  16. What is the difference between Plate element , Shell element and Surface?
  17. How to model an orthotropic plate so that it would have a smaller stiffness in one direction than in another?
  18. Is it possible to obtain the element stresses/ moments at a certain location within a plate ?
  19. I have modeled a T beam using quad plates. I am trying to find out the bending stress in the flange. How can I get that ?

1. Is there a way to obtain the average stress at a node where several plate elements meet?

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. We hope to implement at least some simple cases in future.

2. In the plate element stress results, what do the terms TRESCAT and TRESTAB stand for? How are they calculated?

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.

Example problem 18 in the examples manual shows the calculation of TMAX

3. I am modelling a concrete slab using plate elements. I am looking for the moments in the slab at the center of each element. I noticed that the output gives the bending moments per unit width. What is the per unit width? Would that be the thickness of the plate element?

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. 

Diagrams explaining the various plates forces, moments and streses are available at section 1.6.1 of the Technical Reference manual.

4. I have modeled a 40" x 40" column base plate with (4) 12" dia. pipe columns on it (equally spaced in both directions). How do I tell STAAD that the base plate will be on a concrete pedestal (f'c = 4.0 ksi)? My first guess is to assign supports at the mesh intersections:

SUPPORTS 1 TO 529 ELASTIC MAT DIRECT Y SUBGRADE 4

Any suggestions?

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 is

SUPPORTS
1 TO 529 ELASTIC MAT YONLY SUBGRADE 987

SPRING COMPRESSION
1 TO 529 KFY

If you have any anchor bolts attached to the baseplate, they can be modeled as spring supports (tension only).

An example of this is

SUPPORTS
1000 TO 1004 FIXED BUT MX MY MZ KFY 5467

SPRING TENSION
1000 TO 1004 KFY

5. How do you assign properties to solids?

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.

6. I would like to change the direction of the local Z axis of an element so that it points in the opposite direction. How do I do it?

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.

7. Is it possible to apply a concentrated force on the surface of an element? The point where the load acts is not one of the nodes of the element, as a result of which I cannot use the JOINT LOAD option.

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 y2

In 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 commands

UNIT POUND FEET
LOAD 1 CONCENTRATED LOAD ON WALL
ELEMENT LOAD
73 PR GZ -580.0 1.3 2.5

8. How can I find the maximum shear stress on my plate element model?

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.

9. The plate element results contain a term called TMAX. Is TMAX the best representation of the total stresses resulting from the torsion on the element?

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.

10. In the post processing mode - Results menu - Plate Stress Contour, there are two options called Max Top and Max Bottom. Are these direct stresses or flexural stresses?

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.

11. Can STAAD.Pro be used in designing a mat foundation?

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 analyzed. 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.

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.

Note : A better option is to use STAAD.foundation software for design of mat. Mat modeled and analyzed in STAAD.Pro can be imported into STAAD.foundation will all results data and it can be subseqently designed in STAAD.foundation. One can also model and design mats directly in STAAD.Foundation.

12. When modelling plate elements, should the individual elements satisfy any minimum requirements for the ratio of the length of their side to their thickness?

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.

13. I have a model where supports are defined at the nodes of some of the plate elements in the structure. If I divide the support reaction values by the thickness, length etc., of the side of the elements adjacent to the support, shouldn't the values match the ELEMENT NODAL STRESSES? I am aware of the fact that element stresses are in the local axis system of the element, and support reactions are in the global axis system, and am making the required transformations before making the comparison.

 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.


The output for the command

PRINT ELEMENT FORCES

consists 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.

14. Why shear stresses are not included in the Von Mises stresses for solid elements?

Have a look at the attached figure which is from the following link: http://en.wikipedia.org/wiki/Von_Mises_yield_criterion

There are 2 equations for calculating Von Mises stresses.

The first equation uses the STAAD.Pro terms SXX, SYY, SZZ, SXY, SYZ and SZX.

The second equation uses the terms S1, S2 and S3. These are the principal stresses. There are no shear terms in this equation. This is the one implemented in STAAD.Pro.

The Von Mises stress should be the same from both equations.

15. How to change the local axis orientation X and Y for plates ?

Although it is very easy to flip the direction of the local Z axis for the plates by using the Commands > Geometric Constants > Plate Reference Point option, unfortunately there is no easy way to change the local X and Y for plates as needed. For example, if one needs to re-orient the local x for the plate to be parallel to the global X direction, one has to redefine the incidence of the plates by going to the STAAD editor and changing the ELEMENT INCIDENCE data manually. The local X would be a vector from the center of the plate, drawn in a direction from node1 to node2 and is hence dependent on the element incidences data. In other words the element incidences need to be such that node1 to node2 should be the direction of the global X. The rule which governs how the plate local axes are oriented, is explained under section 1.6.1 of the Technical Reference Manual..

 

16 . What is the difference between Plate element , Shell element and Surface?

 

Plate element and shell element

Both terms represent the same thing in the STAAD context, which is, a 3-noded (triangular) or a 4-noded (quadrilateral) element to which a thickness has to be assigned as a property.

In STAAD, this element has both attributes - membrane (in-plane effect) and bending (out-of-plane effect). The bending effect can be shut off by declaring it as ELEMENT PLANE STRESS. The in-plane effect can't be shut off.

 

Plate Element and Surface

If you want to model a structure which contains a wall, slab or panel type component, you have two choices in STAAD :

 

a) Model that panel using a collection of individual elements. This is called a finite element mesh. This is an assembly of the 2d triangular and/or quadrilateral elements described above.

 

b) Model that as a single physical object called a Surface.

Option (a) is achieved using the mesh generation facilities in STAAD.

In option (b), (surface object), what happens under the hood is that, during the analysis, STAAD transforms the surface into a finite element mesh. The type of mesh (number of elements, type of elements, size of elements, etc.) that is generated from the surface is based on the parameters that you provide at the time of defining the surface.The details of the mesh thus generated are to a large extent, masked from the user. Results are presented for that surface, not for the individual elements that it is made up of.

 In other words, a surface is merely an object that represents a collection of elements. When the program goes through the analysis phase, it subdivides the surface into a plate elements . From analysis point of view, both plate and surface are the same thing . The difference is in the interpretation of results . For plates , the stresses are reported while for Surface the force is reported.

 

 17. How to model an orthotropic plate so that it would have a smaller stiffness in one direction than in another?

You can create the orthotropic 2D material, which would have a different Young's Modulus in X and Y direction (hence different stiffness in both directions). To do so, please go to General -> Materials vertical tab, then in the Material table on the right bottom corner select Orthotropic 2D tab and click Create button. In the opened window provide the required information and then assign this material to the plates.

18. Is it possible to obtain the element stresses/ moments at a certain location within a plate ?

There is a print command that lets you print the element stress at any location within a plate. The syntax for the print command is  

PRINT ELEMENT JOINT STRESSES AT f1 f2 LIST elements-list where f1 and f2 represent the distances along local X and local Y of the plate measured from the plate origin in current units.

For example if the current length units is set to “feet” and to one wants to print the moments/stresses at 0.5 ft from the center of a plate # 47, the print command would be  

PRINT ELEMENT JOINT STRESSES AT 0.5 0.5 LIST 47

You may refer to the section 5.42 of the Technical Reference for more details.

19. I have modeled a T beam using quad plates. I am trying to find out the bending stress in the flange. How can I get that ?

STAAD.Pro reports the bending moments for plates and not bending stresses. However one can find the bending stress without much effort from the data available. First one has to pick a plate close to where the stress is required. Mx (or My ) moments are reported as part of the Plate Center Stress table within the Plate page in the Postprocessing mode. The moment is reported per unit width. One may calculate the Section modulus S ( = 1/6x w x t2 , where w = width of flange plate over which moment is reported, t = thickness of flange plate ). The bending stress would then be M/S.

Alternately STAAD.Pro does report the combined stress for plates. This is available within the Combined Stress tab inside the Plate Center stress table. For the selected plate, note the Top combined stress ( Comb Sx or Comb Sy as appropriate ). The combined stress is the P/A + M/S value. From within the Shear Membrane and Bending tab of the same table, note the SX or the SY which would be the P/A component. One can then find the M/S component by taking out the P/A part from the combined stress. 

See Also

Product TechNotes and FAQs

Structural Product TechNotes And FAQs

External Links

Bentley Technical Support KnowledgeBase

Bentley LEARN Server

Comments or Corrections?

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!