Beam Coordinate Systems

The beam coordinate systems (x-y-z) are used for defining beam offsets and diametral temperature gradients.

No orientation node (default)

Using orientation node L

The x axis is always the axial direction pointing from node I to node J. The optional orientation node L, if used, defines a plane containing the x and z axes at node K. If this element is used in a large-deflection analysis, the location of the orientation node L is used only to initially orient the element.

When no orientation node is used, z is perpendicular to the curvature plane, uniquely determined by the I, J, and K nodes. If I, J, and K are co-linear, the y axis is automatically calculated to be parallel to the global X-Y plane. In cases where the element is parallel to the global Z axis (or within a 0.01 percent slope of the axis), the element y axis is oriented parallel to the global Y axis.

For information about orientation nodes and beam meshing, see Generating a Beam Mesh With Orientation Nodes in the Modeling and Meshing Guide. See Quadratic Elements (Midside Nodes) in the same document for information about midside nodes. For details about generating the optional orientation node L automatically, see the LMESH and LATT command descriptions.

Local Cylindrical Coordinate Systems

The cylindrical coordinate systems (A-R-T) are used for defining internal section motions (that is, axial-A, radial-R, and hoop-T displacements and rotations).

The cylindrical systems are always created from the default beam coordinate systems (beam system without orientation node L), with A being the same as beam axis x, and an angle α (0 < α < 360 degrees) from R to the beam axis y.

Element and Layer Coordinate Systems

The element coordinate systems (e1-e2-e3) are defined at the mid-surfaces of the pipe wall. The e1, e2, and e3 axes are parallel respectively to cylindrical axes A, T, and R in the undeformed configuration. Each element coordinate system is updated independently to account for large material rotation during a geometrically nonlinear analysis. Support is not available for user-defined element coordinate systems.

The layer coordinate systems (L1-L2-L3) are identical to the element coordinate system if no layer orientation angles are specified; otherwise, the layer coordinate system can be generated by rotating the corresponding element coordinate system about the shell normal (axis e3). Material properties are defined in the layer systems; therefore, the layer system is also called the material coordinate system.

ELBOW290 Structural Elbow Cross Sections

The element is a one-dimensional line element in space. The cross-section details are provided separately (via the SECDATA command). A section is associated with the element by specifying the section ID number (SECNUM). A section number is an independent element attribute.

ELBOW290 Structural Elbow can only be associated with the pipe cross section (SECTYPE,,PIPE). For elements with homogeneous materials, the material of the pipe is defined as an element attribute (MAT).

The layup of a composite pipe can be defined with a shell section (SECTYPE). Shell section commands provide the input options for specifying the thickness, material, orientation and number of integration points through the thickness of the layers. The program obtains the actual layer thicknesses used for ELBOW290 Structural Elbow element calculations (by scaling the input layer thickness) so that they are consistent with the total wall thickness given by the pipe section. A single-layer shell section definition is possible, allowing flexibility with regard to the number of integration points used and other options.

For shell section input, you can designate the number of integration points (1, 3, 5, 7, or 9) located through the thickness of each layer. When only one integration point is specified, the point is always located midway between the top and bottom surfaces. If three or more points are specified, one point is located on the top surface, one point is located on the bottom surface, and the remaining points are distributed at equal distances between the top and bottom points. The default number of integration points for each layer is 3. When a single layer is defined and plasticity is present, however, the number of integration points is changed to a minimum of five during solution.

In "Element and Layer Coordinate Systems", the layer coordinate system can be obtained by rotating the corresponding element coordinate system about the shell normal (axis e3) by angle θ (in degrees). The value of θ for each layer is given by the SECDATA command input for the shell section.

For details about associating a shell section with a pipe section, see the SECDATA command documentation.

Cross-Section Constraints

The constraints on the elbow cross-section can be applied at the element nodes I, J, and K with the following section degrees of freedom labels:

SE – section radial motion (as occurs during expansion or ovalization, for example)

SO – section tangential motion (as occurs during ovalization, for example)

SW – section axial motion (as occurs during warping, for example)

SRA – local shell normal rotation about cylindrical axis A

SRT – local shell normal rotation about cylindrical axis T

SECT – all section deformation

Only fixed cross-section constraints are allowed via the D command. Delete section constraints via the DDELE command. For example, to constrain the warping and ovalization of the cross-section at node n, issue this command:

D,n,SW,,,,,SO

To allow only the radial expansion of the cross-section, use the following commands:

D,n,SECT

DDELE,n,SE

It is not practical to maintain the continuity of cross-section deformation between two adjacent elements joined at a sharp angle. For such cases, Ansys, Inc. recommends coupling the nodal displacements and rotations but leaving the cross-section deformation uncoupled. The ELBOW command can automate the process by uncoupling the cross-section deformation for any adjacent elements with cross-sections intersecting at an angle greater than 20 degrees.

ELBOW290 Structural Elbow Transverse Shear Stiffness

ELBOW290 Structural Elbow includes the effects of transverse shear deformation through the pipe wall. The transverse shear stiffness of the element is a 2 x 2 matrix, as shown:

For a single-layer elbow with isotropic material, default transverse shear stiffnesses are as follows:

where k = 5/6, G = shear modulus, and h = pipe wall thickness.

You can override the default transverse shear stiffness values by assigning different values via the SECCONTROL command for the shell section.

ELBOW290 Structural Elbow Loads

Element loads are described in Element Loading. Forces are applied at the nodes. By default, ELBOW290 Structural Elbow element nodes are located at the center of the cross-section. Use the SECOFFSET command's OFFSETY and OFFSETZ arguments for the pipe section to define locations other than the centroid for force application.

Pressure Input

Internal and external pressures are input on an average basis over the element. Lateral pressures are input as force per unit length. End "pressures" are input as forces.

To input surface-load information on the element faces, issue the SFE command

On faces 1 and 2, internal and external pressures are input, respectively, on an average basis over the element.

On face 3, the input (VAL1) is the global Z coordinate of the free surface of the internal fluid of the pipe. Specify this value with ACEL,0,0,ACEL_Z, where ACEL_Z is a positive number. The free surface coordinate is used for the internal mass and pressure effects. If VAL1 on the SFE command is zero, no fluid inside of the pipe is considered. If the internal fluid free surface should be at Z = 0, use a very small number instead. The pressure calculation presumes that the fluid density above an element to the free surface is constant. For cases where the internal fluid consists of more than one type of fluid (such as oil over water), the free surface coordinate of the elements in the fluids below the top fluid need to be adjusted (lowered) to account for the less dense fluid(s) above them.

The internal fluid mass is assumed to be lumped along the centerline of the pipe, so as the centerline of a horizontal pipe moves across the free surface, the mass changes in step-function fashion. The free surface location is stepped, even if you specify ramped loading (KBC,0).

Pressures may be input as surface loads on the element faces as shown by the circled numbers in the following illustration. Positive pressures act into the pipe wall.

The end-cap pressure effect is included by default. The end-cap effect on one or both ends of the element can be deactivated via KEYOPT(6). When subjected to internal and external pressures, ELBOW290 Structural Elbow with end caps (KEYOPT(6) = 0) is always in equilibrium; that is, no net forces are produced. Without end caps (KEYOPT(6) = 1), the element is also in equilibrium except for the case when the element is curved. With end caps only at one end (KEYOPT(6) = 2 or 3), the element is obviously not in equilibrium.

Temperatures

When KEYOPT(1) = 0, a layer-wise pattern is used. T1 and T2 are temperatures at inner wall, T3 and T4 and the interface temperatures between layer 1 and layer 2, ending with temperatures at the exterior of the pipe. All undefined temperatures are default to TUNIF. If exactly (NL + 1) temperatures are given (where NL is the number of layers), then one temperature is taken as the uniform temperature at the bottom of each layer, with the last temperature for the exterior of the pipe.

When KEYOPT(1) = 1, temperatures can be input as element body loads at three locations at both end nodes of the element so that the temperature varies linearly in the beam y axis and z axis directions. At both ends, the element temperatures are input at the section centroid (TAVG), at the outer radius from the centroid in the element y direction (Ty), and at the outer radius from the centroid in the element z direction (Tz). The first coordinate temperature TAVG defaults to TUNIF. If all temperatures after the first are unspecified, they default to the first. If all temperatures at node I are input, and all temperatures at node J are unspecified, the node J temperatures default to the corresponding node I temperatures. For any other input pattern, unspecified temperatures default to TUNIF. The following graphic illustrates temperature input when KEYOPT(1) = 1:

ELBOW290 Structural Elbow Input Summary

Integration Stations

Integration stations along the length and within the cross-section of the elbow are shown in Figure 290.2: ELBOW290 Structural Elbow Element Integration Stations.

Figure 290.2: ELBOW290 Structural Elbow Element Integration Stations

Element solution is available at all integration points through element printout (OUTPR). Solution via the POST1 postprocessor is available at element nodes and selected section integration locations (see KEYOPT(8) settings for more details).

Stress Output

Several items are illustrated in Figure 290.3: ELBOW290 Structural Elbow Stress Output:

Figure 290.3: ELBOW290 Structural Elbow Stress Output

KEYOPT(8) controls the amount of data output to the results file for processing with the LAYER command. Interlaminar shear stress is available at the layer interfaces. KEYOPT(8) must be set to either 1 or 2 to output these stresses in the POST1 postprocessor. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to review results.

KEYOPT(10) = 1 outputs normal stress component Sz, where z is shell normal direction. The element uses a plane-stress formulation that always leads to zero thickness normal stress. With KEYOPT(10) = 1, Sz is independently recovered during the element solution output from the applied pressure load.

The element shell stress resultants (N11, M11, Q13, etc.) are parallel to the element coordinate system (e1-e2-e3), as are the shell membrane strains and curvatures (ε₁₁, κ₁₁, γ₁₃, etc.) of the element. Shell stress resultants and generalized shell strains are available via the SMISC option at the element end nodes I and J only.

ELBOW290 Structural Elbow also outputs beam-related stress resultants (Fx, My, TQ, etc) and linearized stresses (SDIR, SByT, SByB, etc) at two element end nodes I and J to SMISC records. Beam stress resultants and linearized stresses are parallel to the beam coordinate system (x-y-z).

Linearized Stress

It is customary in pipe design to employ components of axial stress that contribute to axial loads and bending in each direction separately. Therefore, ELBOW290 Structural Elbow provides a linearized stress output as part of its SMISC output record, as indicated in the following definitions:

SDIR is the stress component due to axial load.

SDIR = Fx/A, where Fx is the axial load (SMISC quantities 1 and 36) and A is the area of the cross section (SMISC quantities 7 and 42).

SByT and SByB are bending stress components.

where My, Mz are bending moments (SMISC quantities 2,37,3,38). Coordinates y_max, y_min, z_max, and z_min are the maximum and minimum y, z coordinates in the cross section measured from the centroid. Values Iyy and Izz are moments of inertia of the cross section.

The reported stresses are strictly valid only for elastic behavior of members. ELBOW290 Structural Elbow always employs combined stresses in order to support nonlinear material behavior. When the elements are associated with nonlinear materials, the component stresses can at best be regarded as linearized approximations and should be interpreted with caution.

ELBOW290 does not provide extensive element printout. Because the POST1 postprocessor provides more comprehensive output processing tools, Ansys, Inc. suggests issuing the OUTRES command to ensure that the required results are stored in the database. To view 3D deformed shapes for ELBOW290, issue an OUTRES,MISC or OUTRES,ALL command for static or transient analyses. To view 3D mode shapes for a modal or eigenvalue buckling analysis, expand the modes with element results calculation active via the MXPAND command's Elcalc = YES option.

ELBOW290 Structural Elbow Output Definitions

In the table below, the O column indicates the availability of the items in the file Jobname.out. The R column indicates the availability of the items in the results file.

In either the O or R columns, “Y” indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

For the stress and strain components, x-y-z constitutes the element solution coordinate system, where x refers to axial, y refers to hoop, and z refers to radial. Unlike other line elements, ELBOW290 allows for transformation of stresses and strains to other coordinate systems in postprocessing (RSYS). By default, the element stresses and strains are displayed or listed in the Global Cartesian coordinate system.

More output is described via the PRESOL and *GET,,SECR commands in POST1.

ELBOW290 Structural Elbow Item and Sequence Numbers

Table 290.2: ELBOW290 Structural Elbow Item and Sequence Numbers lists output available for the ETABLE and ESOL commands using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this reference for more information. The table uses the following notation:

Beam Coordinate Systems

The beam coordinate systems (x-y-z) are used for orienting the generalized tube section. The beam coordinate systems are used also for defining beam offsets (see SECOFFSET command) and diametral temperature gradients.

No orientation node (default)

Using orientation node L

The x axis is always the axial direction pointing from node I to node J. The optional orientation node L, if used, defines a plane containing the x and z axes at node K. If this element is used in a large-deflection analysis, the location of the orientation node L is used only to initially orient the element.

When no orientation node is used, z is perpendicular to the curvature plane, uniquely determined by the I, J, and K nodes. If I, J, and K are co-linear, the y axis is automatically calculated to be parallel to the global X-Y plane. In cases where the element is parallel to the global Z axis (or within a 0.01 percent slope of the axis), the element y axis is oriented parallel to the global Y axis.

For information about orientation nodes and beam meshing, see Generating a Beam Mesh With Orientation Nodes in the Modeling and Meshing Guide. See Quadratic Elements (Midside Nodes) in the same document for information about midside nodes. For details about generating the optional orientation node L automatically, see the LMESH and LATT command descriptions.

Local Cylindrical Coordinate Systems

The cylindrical coordinate systems (A-R-T) are used for defining internal section motions (that is, axial-A, radial-R, and hoop-T displacements and rotations).

The cylindrical systems are always created from the default beam coordinate systems (beam system without orientation node L), with A being the same as beam axis x, and an angle α (0 < α < 360 degrees) from R to the beam axis y.

Element and Layer Coordinate Systems

The element coordinate systems (e1-e2-e3) are defined at the mid-surfaces of the pipe wall. The e1, e2, and e3 axes are parallel respectively to cylindrical axes A, T, and R in the undeformed configuration. Each element coordinate system is updated independently to account for large material rotation during a geometrically nonlinear analysis. Support is not available for user-defined element coordinate systems.

The layer coordinate systems (L1-L2-L3) are identical to the element coordinate system if no layer orientation angles are specified; otherwise, the layer coordinate system can be generated by rotating the corresponding element coordinate system about the shell normal (axis e3). Material properties are defined in the layer systems; therefore, the layer system is also called the material coordinate system.

ELBOW290 Generalized Tube Cross Sections

The element is a one-dimensional line element in space. The cross-section details are provided separately (via the SECDATA command). A section is associated with the element by specifying the section ID number (SECNUM). A section number is an independent element attribute.

ELBOW290 Generalized Tube can be associated with the pipe cross section (SECTYPE,,PIPE) or tapered pipe cross section (SECTYPE,,TAPER). For details about creating generalized tube sections, see Defining a Tapered Beam or Pipe and Defining a Noncircular Pipe in the Structural Analysis Guide.

The layup of a composite pipe can be defined with a shell section (SECTYPE). Shell section commands provide the input options for specifying the thickness, material, orientation and number of integration points through the thickness of the layers. The program obtains the actual layer thicknesses used for ELBOW290 Generalized Tube element calculations (by scaling the input layer thickness) so that they are consistent with the total wall thickness given by the pipe section. A single-layer shell section definition is possible, allowing flexibility with regard to the number of integration points used and other options.

For shell section input, you can designate the number of integration points (1, 3, 5, 7, or 9) located through the thickness of each layer. When only one integration point is specified, the point is always located midway between the top and bottom surfaces. If three or more points are specified, one point is located on the top surface, one point is located on the bottom surface, and the remaining points are distributed at equal distances between the top and bottom points. The default number of integration points for each layer is 3. When a single layer is defined and plasticity is present, however, the number of integration points is changed to a minimum of five during solution.

In "Element and Layer Coordinate Systems", the layer coordinate system can be obtained by rotating the corresponding element coordinate system about the shell normal (axis e3) by angle θ (in degrees). The value of θ for each layer is given by the SECDATA command input for the shell section.

For details about associating a shell section with a pipe section, see the SECDATA command documentation.

For elements with homogeneous materials, the material of the pipe is defined as an element attribute (MAT).

Cross-Section Constraints

The constraints on the elbow cross-section can be applied at the element nodes I, J, and K with the following section degrees of freedom labels:

SE – section radial motion (as occurs during expansion or ovalization, for example)

SO – section tangential motion (as occurs during ovalization, for example)

SW – section axial motion (as occurs during warping, for example)

SRA – local shell normal rotation about cylindrical axis A

SRT – local shell normal rotation about cylindrical axis T

SECT – all section deformation

Only fixed cross-section constraints are allowed via the D command. Delete section constraints via the DDELE command. For example, to constrain the warping and ovalization of the cross-section at node n, issue this command:

D,n,SW,,,,,SO

To allow only the radial expansion of the cross-section, use the following commands:

D,n,SECT

DDELE,n,SE

It is not practical to maintain the continuity of cross-section deformation between two adjacent elements joined at a sharp angle. For such cases, Ansys, Inc. recommends coupling the nodal displacements and rotations but leaving the cross-section deformation uncoupled. The ELBOW command can automate the process by uncoupling the cross-section deformation for any adjacent elements with cross-sections intersecting at an angle greater than 20 degrees.

ELBOW290 Generalized Tube Transverse Shear Stiffness

ELBOW290 Generalized Tube includes the effects of transverse shear deformation through the pipe wall. The transverse shear stiffness of the element is a 2 x 2 matrix, as shown:

For a single-layer elbow with isotropic material, default transverse shear stiffnesses are as follows:

where k = 5/6, G = shear modulus, and h = pipe wall thickness.

You can override the default transverse shear stiffness values by assigning different values via the SECCONTROL command for the shell section.

ELBOW290 Generalized Tube Loads

Element loads are described in Element Loading. Forces are applied at the nodes. By default, ELBOW290 Generalized Tube element nodes are located at the center of the cross-section. Use the SECOFFSET command's OFFSETY and OFFSETZ arguments for the pipe section to define locations other than the centroid for force application.

Pressure Input

Internal and external pressures are input on an average basis over the element. Lateral pressures are input as force per unit length. End "pressures" are input as forces.

To input surface-load information on the element faces, issue the SFE command

On faces 1 and 2, internal and external pressures are input, respectively, on an average basis over the element.

On face 3, the input (VAL1) is the global Z coordinate of the free surface of the internal fluid of the pipe. Specify this value with ACEL,0,0,ACEL_Z, where ACEL_Z is a positive number. The free surface coordinate is used for the internal mass and pressure effects. If VAL1 on the SFE command is zero, no fluid inside of the pipe is considered. If the internal fluid free surface should be at Z = 0, use a very small number instead. The pressure calculation presumes that the fluid density above an element to the free surface is constant. For cases where the internal fluid consists of more than one type of fluid (such as oil over water), the free surface coordinate of the elements in the fluids below the top fluid need to be adjusted (lowered) to account for the less dense fluid(s) above them.

The internal fluid mass is assumed to be lumped along the centerline of the pipe, so as the centerline of a horizontal pipe moves across the free surface, the mass changes in step-function fashion. The free surface location is stepped, even if you specify ramped loading (KBC,0).

Pressures may be input as surface loads on the element faces as shown by the circled numbers in the following illustration. Positive pressures act into the pipe wall.

The end-cap pressure effect is included by default. The end-cap effect on one or both ends of the element can be deactivated via KEYOPT(6). When subjected to internal and external pressures, ELBOW290 Generalized Tube with end caps (KEYOPT(6) = 0) is always in equilibrium; that is, no net forces are produced. Without end caps (KEYOPT(6) = 1), the element is also in equilibrium except for the case when the element is curved. With end caps only at one end (KEYOPT(6) = 2 or 3), the element is obviously not in equilibrium.

Temperatures

When KEYOPT(1) = 0, a layer-wise pattern is used. T1 and T2 are temperatures at inner wall, T3 and T4 and the interface temperatures between layer 1 and layer 2, ending with temperatures at the exterior of the pipe. All undefined temperatures are default to TUNIF. If exactly (NL + 1) temperatures are given (where NL is the number of layers), then one temperature is taken as the uniform temperature at the bottom of each layer, with the last temperature for the exterior of the pipe.

When KEYOPT(1) = 1, temperatures can be input as element body loads at three locations at both end nodes of the element so that the temperature varies linearly in the beam y axis and z axis directions. At both ends, the element temperatures are input at the section centroid (TAVG), at the outer radius from the centroid in the element y direction (Ty), and at the outer radius from the centroid in the element z direction (Tz). The first coordinate temperature TAVG defaults to TUNIF. If all temperatures after the first are unspecified, they default to the first. If all temperatures at node I are input, and all temperatures at node J are unspecified, the node J temperatures default to the corresponding node I temperatures. For any other input pattern, unspecified temperatures default to TUNIF. The following graphic illustrates temperature input when KEYOPT(1) = 1:

ELBOW290 Generalized Tube Input Summary

Integration Stations

Integration stations along the length and within the cross-section of the elbow are shown in Figure 290.5: ELBOW290 Generalized Tube Element Integration Stations.

Figure 290.5: ELBOW290 Generalized Tube Element Integration Stations

Element solution is available at all integration points through element printout (OUTPR). Solution via the POST1 postprocessor is available at element nodes and selected section integration locations (see KEYOPT(8) settings for more details).

Stress Output

Several items are illustrated in Figure 290.6: ELBOW290 Generalized Tube Stress Output:

Figure 290.6: ELBOW290 Generalized Tube Stress Output

KEYOPT(8) controls the amount of data output to the results file for processing with the LAYER command. Interlaminar shear stress is available at the layer interfaces. KEYOPT(8) must be set to either 1 or 2 to output these stresses in the POST1 postprocessor. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to review results.

KEYOPT(10) = 1 outputs normal stress component Sz, where z is shell normal direction. The element uses a plane-stress formulation that always leads to zero thickness normal stress. With KEYOPT(10) = 1, Sz is independently recovered during the element solution output from the applied pressure load.

The element shell stress resultants (N11, M11, Q13, etc.) are parallel to the element coordinate system (e1-e2-e3), as are the shell membrane strains and curvatures (ε₁₁, κ₁₁, γ₁₃, etc.) of the element. Shell stress resultants and generalized shell strains are available via the SMISC option at the element end nodes I and J only.

ELBOW290 Generalized Tube also outputs beam-related stress resultants (Fx, My, TQ, etc) and linearized stresses (SDIR, SByT, SByB, etc) at two element end nodes I and J to SMISC records. Beam stress resultants and linearized stresses are parallel to the beam coordinate system (x-y-z).

Linearized Stress

It is customary in pipe design to employ components of axial stress that contribute to axial loads and bending in each direction separately. Therefore, ELBOW290 Generalized Tube provides a linearized stress output as part of its SMISC output record, as indicated in the following definitions:

SDIR is the stress component due to axial load.

SDIR = Fx/A, where Fx is the axial load (SMISC quantities 1 and 36) and A is the area of the cross section (SMISC quantities 7 and 42).

SByT and SByB are bending stress components.

where My, Mz are bending moments (SMISC quantities 2,37,3,38). Coordinates y_max, y_min, z_max, and z_min are the maximum and minimum y, z coordinates in the cross section measured from the centroid. Values Iyy and Izz are moments of inertia of the cross section.

The reported stresses are strictly valid only for elastic behavior of members. ELBOW290 Generalized Tube always employs combined stresses in order to support nonlinear material behavior. When the elements are associated with nonlinear materials, the component stresses can at best be regarded as linearized approximations and should be interpreted with caution.

ELBOW290 Generalized Tube does not provide extensive element printout. Because the POST1 postprocessor provides more comprehensive output processing tools, Ansys, Inc. suggests issuing the OUTRES command to ensure that the required results are stored in the database. To view 3D deformed shapes for ELBOW290 Generalized Tube, issue an OUTRES,MISC or OUTRES,ALL command for static or transient analyses. To view 3D mode shapes for a modal or eigenvalue buckling analysis, expand the modes with element results calculation active via the MXPAND command's Elcalc = YES option.

ELBOW290 Generalized Tube Output Definitions

The Element Output Definitions table uses the following notation:

More output is described via the PRESOL and *GET,,SECR commands in POST1.

ELBOW290 Generalized Tube Item and Sequence Numbers

Table 290.4: ELBOW290 Generalized Tube Item and Sequence Numbers lists output available for the ETABLE command using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this document for more information. The output tables use the following notation: