Bond-slip Reinforcements and Pile Foundations

Transcription

1 Bond-slip Reinforcements and Pile Foundations Gerd-Jan Schreppers, January 2015 Abstract: This paper explains the concept and application of bond-slip reinforcements and pile foundations in DIANA. Basic assumptions and definitions will be discussed, as well as the pre-processing for bars in combination with different element types, specific loads, properties and material models. Introduction In the embedded reinforcement concept in DIANA the reinforcement particles share the displacement degrees of freedom with the continuum elements in which they are located. As a consequence no relative displacement between reinforcement and continuum element is allowed. For applications such as pull-out of anchors, post-tensioning of cables in concrete and even pile foundations, the frictional slip between bar and concrete or pile and soil is essential. Therefore, the concept of slipping reinforcements has been developed in DIANA as an alternative to the embedded reinforcement concept. In this paper the concept of slipping reinforcements is defined, which combines the efficient use of defining line reinforcements independent from the continuum elements connectivity, with slip between the line reinforcement and the continuum element. There are two main applications for slipping reinforcements: Bond-slip of a steel reinforcement bar in concrete continuum Concrete pile in soil For reading this paper it is recommended to read the white paper about Embedded reinfor-cements first. Basic Assumptions and Definitions Slip reinforcements are only available for lines in the following continuum elements: 2D plane stress elements 3D curved shell elements 3D solid elements The location of the slip reinforcements is defined similar to embedded reinforcements: independent from mesh of the continuum elements in which the reinforcement lines are located. In the preprocessing DIANA calculates the intersection of the reinforcement line and the individual continuum elements. Every reinforcement line is subdivided into particles which exactly match with one continuum element. Contrary to embedded reinforcements, slip reinforcements particles have their own displacement degrees of freedom and therefore can move relative to the element in which the particle is located. Internally in the DIANA program the slip reinforcement particles are converted to beam or truss elements which are connected by special interface elements to the continuum element in which the particle is located. Slip reinforcements are identified by the keyword in the element data of the reinforcement in MeshEdit. The keyword comes with the specification for the conditions where the particle shall be defined as a truss element and with the specification for the conditions where the particle shall be defined as a beam element. When the truss option is chosen a uniaxial stress condition is assumed in the line and no shear and bending is considered, similar to the embedded reinforcement concept. For steel bars with larger diameter, or bars passing heavily cracked concrete zones and shear loaded, or piles in soil, the beam element option, which includes shear and bending, is available. For slip reinforcements there is the option to define nonlinear point interfaces are the end points of the slip reinforcement. These nonlinear point interfaces define the interaction between the reinforcement end and the continuum element in which the end point is located. These point interfaces are indicated as tip interface elements and are defined by the keyword TIPLOC in the material properties for the reinforcement in table MATERI. The TIPLOC keyword comes with the options BEGIN for a tip interface only at the beginning of the reinforcement line, with the keyword END for a tip interface only at the end of the reinforcement line, or with the keyword BOTH for tip interfaces at the begin and end of the reinforcement line. When DIANA pre-processes the slip reinforcement particles, the program logs in the output file that the reinforcement is replaced by elements as follows: REINFORCEMENT 3 REPLACED BY NEW ELEMENTS to

2 Embedded Reinforcements Page 2 Slip reinforcement are defined by the following information: Location in the model keyword in the element data specification Material properties for both line and interface Optionally, the definition of tip interfaces at the end points of the slip reinforcement. In that case also the material properties for the tip interfaces must be defined. Geometrical data of beam or truss (crosssection and perimeter) Results of slip reinforcements are presented as reinforcement results. That means that both results of the beam or truss element and the line interface element are presented as results of the same reinforcement particle. Therefore, results in slip reinforcement particles can only be presented in the nodes of a particle and not in integration points.. Slip reinforcement use the default integration schemes for the beam and truss elements; no integration schemes can be defined by the user for slip reinforcements. Line-solid Interface Elements A line-solid interface element connects the beam or truss element to the continuum element in which the line element is located. The line-solid element is only used internally and is automatically generated. There are line-solid interface elements available for all solid elements with linear or quadratic interpolation schemes. Also the line side can have a linear (2 nodes) or quadratic (3 nodes) interpolation scheme. Linear solid elements can be combined only with linear lines, whereas quadratic solid elements can be combined only with quadratic lines. Line-solid interface elements can only be used in DIANA internally and cannot be explicitly defined by the user in DIANA input. line-solid element combinations in DIANA: Solid element TE12L L13BE L6TRU TP18L L13BE L6TRU HX24L L13BE L6TRU CTE30 CL18B CL9TR CTP45 CL18B CL9TR CHX60 CL18B CL9TR In the next figure the interface element that connects a 3-node beam of type CL18B to a solid element of type CHX60 is shown as example. Combination line-solid interface element that connects 3-node beam element to 20-node hexahedron element This interface element has three integration points, which are defined with a Newton-Cotes integration scheme on the line between the relative nodes 1, 2 and 3. For each of these integration points the displacement from the line nodes (nodes 1-3) is calculated by interpolation and the displacement from the solid nodes (nodes 4-23) is calculated. The relative displacement in the interface element is defined as the difference between these two displacements. For the interface element a material law is defined in terms of relative displacement in the direction of the line and the bond-stress-traction in the same direction. The bond-stress-traction is multiplied by the perimeter of the line element and integrated over the length of the line. From this distributed force along the line particle the equivalent forces in all nodes of the interface are calculated, which are used in the equilibrium check of the model. In the directions normal to the line high penalty stiffness is assumed. This stiffness is defined by the user as a material parameter. Similar to line-solid interface elements, line-plane interface elements are available for 2D plane stress elements and line-shell interface elements are available for 3D curved shell elements. line-plane element combinations in DIANA: Plane element T6MEM L13BE L6TRU Q8MEM L13BE L6TRU CT12M CL18B CL9TR CQ16M CL18B CL9TR line-shell element combinations in DIANA:

3 Embedded Reinforcements Page 3 Shell element T15SH L13BE L6TRU Q20SH L13BE L6TRU CT30S CL18B CL9TR CQ40S CL18B CL9TR T18SH L13BE L6TRU Q24SH L13BE L6TRU CT36S CL18B CL9TR CQ48S CL18B CL9TR CT30L CL18B CL9TR CQ40L CL18B CL9TR CT36L CL18B CL9TR CQ48L CL18B CL9TR Point-solid Interface Elements A point-solid interface element connects a point to a continuum element in which the point is located. The point-solid element is only used internally and is automatically generated. There are point-solid interface elements available for all solid elements with linear or quadratic interpolation schemes. Point-solid interface elements can only be used in DIANA internally and cannot be explicitly defined by the user in DIANA input. For the following solid elements point-solid Solid element type TE12L TP18L HX24L CTE30 CTP45 CHX60 In the next figure the connectivity of the interface element that connects a TE12L element to a point is shown as example of the point-solid interface element. Combination solid-point interface element that connects 1 point to 4-node tetrahedron element This element has one integration point which is located in the point in the body of the solid, in this figure indicated with 1. For this point, the relative displacement from this point to the displacement interpolated from the solid nodes (nodes 2-5) is calculated. For the interface element a material law is defined in terms of relative displacement in a user-defined direction and the force in the same direction. From this force the equivalent forces in all nodes of the interface are calculated, which are used in the equilibrium check of the model. In the directions normal to this direction high penalty stiffness is assumed. This stiffness is defined by the user as a material parameter. Similar to point-solid interface elements, pointinterface elements are available for 2D plane stress elements and for 3D curved shell elements. For the following plane membrane elements, pointplane Plane element type T6MEM Q8MEM CT12M CQ16M For the following curved shell elements, point-shell Shell element type T15SH Q20SH CT30S CQ40S T18SH Q24SH CT36S

4 Embedded Reinforcements Page 4 CQ48S CT30L CQ40L CT36L CQ48L Bar reinforcement in solid element Pre-processing Bar in plane stress elements Slip reinforcements can be defined in the earlier mentioned plane stress elements. Plane stress elements are automatically checked for intersection with a bar reinforcement specified with sections. A plane stress element embeds a particle of a bar section if it intersects one or two element edges, but none of them more than once. Bar reinforcement in plane stress element Bar reinforcement in curved shell elements Slip reinforcements can intersect all earlier mentioned curved shell elements. Curved shell elements are automatically checked for intersection with a bar reinforcement specified with sections. There are two conditions for a bar section to be identified in a curved shell element: (1) It must intersect one or two element edges, but none of them more than once; (2) The computed location points must be inside the thickness domain of the element. Bar reinforcement in curved shell element Bar reinforcement in solid elements Slip reinforcements can intersect all earlier mentioned solid elements. To include bar reinforcement in solid elements, DIANA needs for each solid element the location points of the particle that is embedded in that element. Load Nodal forces and prescribed displacements can be defined in the end nodes of slip reinforcements in the standard way. Connection to Other Elements When the end points of slip reinforcements are defined with nodes, the slip reinforcement can be connected to other elements by sharing these nodes. When end-points of slip reinforcement are defined with coordinates, their node-id can be defined with the element-data items BEGINN and ENDNOD in MeshEdit. When sharing nodes with elements is not possible, it can be considered to define for part of the slip reinforcement a very stiff bond, as if it is embedded in the respective elements. This is a very popular way for connecting slip reinforcements, representing foundation piles to a raft foundation which is modelled with shell or solid elements. Material Models for Bond-slip Reinforcements The material parameters of the bond-slip reinforcements define both the material for the beam or truss elements as for the interface elements. All available material models for the regular beam and truss elements can be applied. Linear elastic Von Mises elasto-plastic model with and without hardening For the interface elements the following models may be applied. Friction stress slip diagram Cubic bond-slip function by Dörr Power-law bond-slip by Noakowski Bond-slip function of Shima et al. For anchor or tip elements the following material models may be used.

5 Embedded Reinforcements Page 5 Force-relative displacement diagram Ultimate anchor force For more theoretical background about these models see the DIANA User s manual. The geometry properties of the truss or beam elements must be defined. For the interface elements the outer diameter d or the perimeter of the reinforcement should be specified. For rectangular (RECTAN), box (BOX), circular (CIRCLE), or pipe (PIPE) beam crosssections, DIANA calculates the diameter and perimeter internally. Therefore, specification of the diameter or perimeter is not required for these predefined cross-sections. DIANA uses the diameter or perimeter to convert the shaft stresses to cross-section forces per unit length. For reinforcements in shell or solid elements, there is no unique interface plane and DIANA needs a direction vector to set up the element axes. With respect to the geometric properties of the pile elements the same constraints can be made as for bond-slip reinforcements. Material Models for Pile Foundations The material parameters of the pile foundations define both the material for the beam elements as for the interface elements. All available material models for the beam elements can be applied. Below some typical material models for pile foundations are listed. Piles are usually modelled as linear elastic. For the pile shaft to soil interface elements the following models may be applied. can be defined as constant stiffness model or as stiffness varying linearly with depth. Friction stress slip diagram Ultimate shear shear-force per length can be defined as a constant ultimate shear force along the pile or as a maximum shear force that increases linearly with depth of the pile. Coulomb friction model with normal stress being the averaged horizontal stress in the soil at the location of the respective depth of pile. For pile tip interfaces the following material models may be used. Force-relative displacement diagram Ultimate pile tip force For more theoretical background about these models see the DIANA User s manual.