.png){kind=small}
icon from the top right pane. This will change the right hand pane to the FE results area. The layout of the FE results area is shown below.
The results of a finite element analysis include a wide range of force and displacements for each individual node. For the majority of models, the number of numerical results would be too large to directly process effectively. Therefore the results of an Finite Element analysis are presented graphically. The results can be displayed in a contour format, or in the form of section diagrams, using line, rectangular or circular sections. With both the contour and section diagram outputs, the software also provides options to display numerical values for results are various locations within the FE surfaces. The software also provides the option to apply peak smoothing of the FE results, or, alternatively, the section diagrams can be used with an averaging strip width.
It is a good idea to globally verify the results using a few hand calculations and checks so as to make sure the results are in the expected ballpark values.
To access the results for the FE surfaces, go to Results>Graphical Analysis Results and then select the icon from the top right pane. This will change the right hand pane to the FE results area. The layout of the FE results area is shown below.
.png)
.png)
In both the graphical and section diagram results, the following force and displacement or stress results can be displayed. In line with standard FE results conventions, tensile stress is displayed as a positive stress. Hence tensile forces are also displayed as a positive value. The forces and displacement results are as follows:
|
Max Error (%) |
Displays the percentage error in the results. |
|
Fx (kN/m) membrane |
the in-plane (axial) force in the local x-axis direction |
|
Fy (kN/m) membrane |
the in-plane (axial) force in the local y-axis direction |
|
Fxy (kN/m) membrane |
the in-plane shear force in the local xy-plane |
|
Fmax (kN/m) membrane |
the principal in-plane membrane force derived from the principal stress σ1 |
|
Fmin (kN/m) membrane |
the principal in-plane membrane force derived from the principal stress σ2 |
|
Mx (kNm.m) moment |
Moment in the local x axis of the surface. This is moment from bending in the x direction of the element, i.e. rotating about the local y axis. A positive value indicates compression on the positive local z axis side of the element. |
|
My (kNm/m) moment |
Moment in the local y axis of the surface. This is moment from bending in the y direction of the element, i.e. rotating about the local x axis. Sign convention as per Mx. |
|
Mxy (kNm/m) moment |
Twisting moment. Just as a two dimensional stress field has two direct stresses (x and y) and a shear stress (xy), the two dimensional system of moments is the same. Sign convention as per Mx. |
|
Mmax (kNm/m) principal |
The (max) principal moments in an element, determined by transforming the Mx, My and Mxy forces to the direction whereby the perpendicular forces Mmax and Mmin cause zero twisting moments Mxy. Sign convention as per Mx. |
|
Mmin (kNm/m) principal |
The (min) principal moments in an element, determined by transforming the Mx, My and Mxy forces to the direction whereby the perpendicular forces Mmax and Mmin cause zero twisting moments Mxy. Sign convention as per Mx. |
|
FVx (kN/m) shear |
Transverse shear force (through the thickness of the element) in a shear plane normal to the local x-axis. |
|
FVy (kN/m) shear |
Transverse shear force (through the thickness of the element) in a shear plane normal to the local y-axis. |
|
FVMax (kN/m) shear |
Vector sum ((Fvx² + Fvy² )^0.5) of the transverse shear forces Fvx and Fvy. |
|
Mrx - Wood & Armer |
The modified moment in the local x axis (i.e rotation about the local y-axis) of the surface modified using the Wood & Armer technique, taking into account the twisting moment Mxy. In reinforced concrete the ‘Wood & Armer’moments are normally used in the design and not the direct Mx and My moments. |
|
Mry - Wood & Armer |
The modified moment in the local y axis (i.e rotation about the local x-axis) of the surface modified using the Wood & Armer technique, which takes into account the effect of the twisting moment Mxy. |
|
X displ (mm) |
the displacement measured in the global X-axis direction |
|
Y displ (mm) |
the displacement measured in the global Y-axis direction |
|
Z disp (mm) |
the displacement measured in the global Z-axis direction |
|
Tx rotation (deg) |
The rotation about the global X-axis, measured in degrees |
|
Ty rotation (deg) |
The rotation about the global Y-axis, measured in degrees |
|
Tz rotation (deg) |
The rotation about the global Z-axis, measured in degrees |
|
As req Top XX |
the reinforcement required for the Mrx moment i.e. bars running parallel to the local x-axis, located at the positive local z-axis side (top) of the section |
|
As req Top YY |
the reinforcement required for the Mry moment i.e. bars running parallel to the local y-axis, located at the positive local z-axis side (top) of the section |
|
As req Bot XX |
the reinforcement required for the Mrx moment i.e. bars running parallel to the local x-axis, located at the negative local z-axis side (bottom) of the section |
|
As req Bot YY |
the reinforcement required for the Mry moment i.e. bars running parallel to the local y-axis, located at the negative local z-axis side (bottom) of the section |
|
Spring support reaction (kN/m²) |
for horizontal FE surfaces where a surface area spring has been defined, the support reactions are displayed as kN/m² |
The stress results are as follows:
|
σx (N/mm²) |
the stress on a face normal to the local x-axis, given in N/mm² |
|
σy (N/mm²) |
the stress on a face normal to the local y-axis, given in N/mm² |
|
τxy (N/mm²) |
the shear stress in the plane of the FE surface. |
|
σ max (N/mm²) |
The principal stress σ1 = 1/2((σx+σy) + √[(σx - σy)² + 4τxy²] |
|
σ min (N/mm²) |
The principal stress σ2 = 1/2((σx+σy) - √[(σx - σy)² + 4τxy²] |
|
τxz (N/mm²) |
The shear stress on the local xz plane |
|
τyz (N/mm²) |
The shear stress on the local yz plane |
|
σ von Mises (N/mm²) |
displays the von Mises stress |
|
σ Tresca (N/mm²) |
displays the Tresca stress |
|
σ Drucker-Prager (N/mm²) |
displays the Drucker-Prager stress |
|
σ Mohr Coloumb (N/mm²) |
displays the Mohr-Coloumb stress |
For the stress outputs, the stresses are calculated for the top, mid-plane and bottom of the FE surface. The 'side' of the FE surface is chosen using the drop down to the right of the stress results drop down. In addition to the side selection, the maximum (absolute) value of the stress results can also be selected.
Where the principal stresses (or the bending moments resulting from the principal stresses) are selected, an additional display option is activated. This indicates the direction of the principal stresses. This option is enabled by clicking on the .png){kind=small}
icon.
To take into account non-uniaxial stress conditions, the stress results for an FE surface include four common elastic yield criteria. For ductile materials where the yield stress is the same in tension as in compression, the Tresca or von Mises stress output would be used. Where a material is brittle, so that the tensile yield stress is lower than the compressive yield stress, then the Drucker-Prager or Mohr Coloumb stress results would be used. For brittle materials, the stress is displayed relative to the compressive yield stress σyc. For the Drucker-Prager or Mohr-Coloumb results, it is necessary to input the Fyt and Fyc values in the FE surface material properties.
For further information on the elastic yield criterion, reference should be made to a suitable resource. The following Wikipedia page may also be of use - https://en.wikipedia.org/wiki/Yield_surface
When viewing the contour outputs, a number of viewing features are available to assist in using the contour plots to view the magnitude of the results. These options are:
Colour map flat - displays the contours as flat surfaces. The contours are displayed over the plane of each FE surface.
Colour map 3D - the contours are offset from the plane of the FE surface in proportion to their value, producing a 3D results surface. With the 3D plot option selected, the offset of the plot can be controlled using the scale value.
A typical example of a 3D contour plot is shown below. This shows the peak value of the bending moment underneath to supported column which is applying a large point load to the FE surface. 3D contour plots are often useful when considering peak values in the FE results.
.png)
Colour Contour Lines - this produces a flat map with the contour lines colour coded to the values. This option also allows for the results to be exported as a dxf file, which can be obtained by clicking on the .png){kind=small}
icon. This output uses only coloured contour lines to reduce the amount of coloured ink that would be required to print a full colour flat contour map.
Contours - the number of computer generated contours to be displayed. The software uses the maximum and minimum values of the results to determine the range of the results and then divides this range into the number of selected contours.
Where peak values dominate the results this can leave areas of an FE surface where the resulting contour output is covered by a few, or even just one, contours. The software provides options to control or refine the contours to allow for the results range to be adjusted to investigate areas in more detail. These options are:
Max value - input a maximum value for the software to use in the calculation of the range of results and restrict the contours to be below this maximum. Areas where the results are outside the maximum value will be displayed in grey.
Min value - similar to the maximum value, but defines the lower end of the range. Values less than the minimum value will be displayed in grey.
User values - multiple contour values can be input, separated by a semi-colon. Contours of these values will be displayed in addition to those generated by the software using the range of the results (including the max and/or min values, if input) and the number of contours.
Additional results display options are:
Show contour legend - display a contour key indicating the range of values for each colour coded contour.
Place value at point - allows the values at each node in the FE surface to be displayed. The point(s) to be picked are selected using the mouse pointer.
Show characteristic values - displays values at software determined characteristic points within each FE surface.
Show peak values - displays the result values at software determined peak points.
When viewing results graphically, the contour values and range are determined by the range of values being displayed graphically. Therefore, when viewing the whole model, this will give the maximum range of the results over which the number of contours are calculated. Therefore, greater resolution can be gained by using the viewing options to view portions of the structure, which will then give the same number of contours but the range of results may be reduced. The use of the viewing filters and frame views are detailed in the MasterFrame manual.
When viewing contour plot results, the under lying FE mesh will still be visible, which may to some degree obscure some of the graphics. The FE mesh can be hidden from view using the display options. Clicking on the .png){kind=small}
icon and expanding the Finite Element Display Options, the "Don't Draw FE Mesh (outside editor)" option can be used to turn the FE mesh on and off.
Section diagrams provide a useful facility to investigate the results from an FE analysis along a line, on a rectangular perimeter or on a circular perimeter. Section diagrams can be particularly useful for investigating the bending moment distribution in slabs when looking for the bending moments in 'column' and 'middle' strips, or for investigating the axial force in walls.
To add a section diagram, select the required section type from the .png){kind=small}
icons. Once the icon clicked, the section name will be automatically filled in, denoting the type of section diagram and the section number.
For a line section diagram, the position of the line is defined by either nodes or by coordinates. Nodes can be selected graphically, using the mouse pointer. When a node is selected, the coordinate information will be automatically filled in. The "Pick basic nodes" option restricts the selected nodes to be those present in the Masterframe 'wireframe' model. To select nodes which are part of the FE mesh, the "Pick basic nodes" checkbox needs to unchecked. If the "Pick Basic nodes" option is selected, if the node numbering of the model is changed, then the section diagram will move with the nodes; otherwise, the coordinates of the line diagram will be the determining setting-out factor and re-meshing the model will not cause the line diagram to change position.
The rectangular and circular section diagrams work in a similar manner, except they are defined on a central point, which is defined by either a node point or by coordinates. In the case of a rectangular section, the section size is defined by the length and breadth of the section perimeter while a circular section is defined by the radius of the perimeter.
The scale of the section diagram is controlled by using the scale drop down.
The interval drop down controls the number of segments the scale diagram is divided into. Increasing the number of segments can help when viewing the digram. it also affects the number of numerical results which are displayed.
To display numerical values on section diagrams, select the .png){kind=small}
icon. Where results are shown can be controlled using the .png)
.png){kind=small}
- displays the distance along the line diagram that the result value occurs
.png){kind=small}
- indicates the distance along the line diagram that zero values occur
.png){kind=small}
- this drop down controls the interval at which results are displayed. The Auto option displays the results at point where the results at maximum hogging and sagging values at also at points where step changes occur. Alternatively, the drop down can be used to show results are interval points. The options are 1-5, where 1 shows results at every selected interval point, while 5 shows results at every 5th interval point.
As well as controlling the scale, the direction the results diagram is displayed in can be controlled using the .png){kind=small}
drop down. This does not affect the results axes, only the direction the diagram is displayed in.
By default, the software will display one line diagram at a time, with the displayed section being selected from the Section drop down. All section diagrams can be displayed at once by clicking on the .png){kind=small}
icon.
Further grouping of section diagrams can be achieved by using the Section Diagram Sets feature. A Section Diagram Set is effectively a grouping of section diagrams that are to be displayed at once. To add a Diagram Set, click on the .png){kind=small}
icon. The digram set name will increment by one, but this can be deleted and a user-defined name added. Adding new section diagrams will now be in this new Section Diagram set.
Line Diagram can be used in conjunction with the Average Strip feature. This allows for a width over which the results of the line diagram are to be averaged. The software carries out an integration over the strip width to calculate the average value. For edge strips, the software detects the region over which the results lie outside the FE surface and these are excluded ; that is, the averaging process only takes place over the width within the FE surface.
Note: An average strip width should only be used over an appropriate strip width. Using large width strips may produce overly low average results values since the sign of the results are included in the averaging process. For Flat Slabs, reference should be made the rules for Flat Slabs in either BS 8110 or BS EN 1992-1-1 or, alternatively, the Concrete Centre publication "How to design concrete flat slabs using Finite Element Analysis".
Where 1D line elements or point loads act on an FE surface, the results are liable to result in a peak value occurring, due to a singularity in the results. A singularity occurs where a force or restraint occurs at a point. Since a point has position but no size, theoretically the stress at the point is infinite. One methodology to dealing with these peaks in the results is to use peak smoothing. Peak smoothing is defined over a radius around the peak values. The software takes the results at the perimeter of the peak radius and uses the maximum of these values to represent the results inside the perimeter. Thus peak smoothing can be used to reduce the impact of the singularity. Where the results varying significantly around the peak perimeter, then no one value is representative of the results inside the perimeter and in this case, the software ignores the values within the peak smoothing perimeter and the contours inside the peak perimeter are shown in grey.
Since the software is either attempting to calculate a representative value for a peak, or ignoring the values within the peak smoothing area, care must be exercised when determining an appropriate peak smoothing perimeter. For columns, it would be inadvisable to select a radius which would lie outside the column cross section.
Where column/wall stiff regions have been applied, peak smoothing is not effective. This is because the stiffness of the mesh has been modified to account for the stiffness of the wall or column cross section and so carrying out a peak smoothing in addition to this is not appropriate, since the results will already be modified.
The Results Axis area is common to both contour and line diagrams. This area provide tools to control the results which are being displayed. These options are as follows:
Local axis - the results are displayed in terms of the surface local x- and y-axes.
Section Line - when using section lines, the results can be displayed as if the section line is the local x axis. This can be useful for looking at the distribution of bending moments in slabs, where bending moments Mrx results can be displayed for section lines even where the section lines intersect at right angles. A typical example is shown below.
.png)
User Coordinate System - the orientation of each FE surface can be rotated by a user specified input (in degrees). The local z-axis orientation is not modified. If no input is defined for a surface then the local axis remains unmodified. This feature can be used to align the coordinate system of various FE surfaces. This can be useful where slabs have been created using multiple FE surfaces.
Highlight current surface - this option is used in conjunction with the User Coordinate system
Show axis for each surface - this turns on a local axis coordinate axis indicator for each FE surface.