Experimental and Numerical Analysis of Initial Plasticity in P91 Steel Small Punch Creep Samples

The testing programme consisted of pre-strained uniaxial creep tests and SPCTs carried out on a P91 steel at 600 ^∘. Table 1 reports the chemical composition, in wt%, of the P91 steel used in the present work, while Fig. 1 shows an SEM image of the virgin material microstructure. Cylindrical uniaxial specimens were machined on a CNC lathe from a power plant steam pipe section. The data obtained from the pre-strained uniaxial creep tests was used to characterise the plastic behaviour of the material through the determination of two parameters, ϕ and ψ, as described in Section 2.1.3.

Before manufacturing the specimen (see Fig. 2 for the specimen geometry) material blanks were tempered at 760 ^∘C for 3 hours and then cooled to room temperature at a rate of 0.8 ^∘C/min , in order to obtain a fully martensitic steel microstructure.

A Mayes EN250 machine was used for all of the pre-strained uniaxial creep tests. The deformation of the specimen was monitored by use of an extensometer with a gauge length of 50 mm, while the temperature was kept constant to within ± 1 ^∘C by the furnace controller of the machine. For each test, the specimen was plastically pre-strained under displacement control conditions. Subsequently, the configuration of the machine was changed to load control and constant load creep tests were carried out. The load levels used during the creep tests were corrected in order to account for the reduction of the cross sectional area due to plastic pre-straining. When plastic deformation takes place the volume of the specimen is constant, therefore equation (1) holds, where Ω _{p r e} and L _{p r e} are the cross section area and the gauge length of the specimen at the end of pre-straining, while Ω _{y i e l d} and L _{y i e l d} are the cross section area and the specimen gauge length at yielding.

The load, P, applied to the specimen is then obtained by equation (2), where σ is the stress applied, d ₀ is the initial diameter of the specimen’s effective section, 𝜖 _{e l,y i e l d} is the elastic engineering strain at yielding, 𝜖 _p is the plastic pre-strain and ν is the Poisson’s ratio. Deviation of equation (2) is presented in the Appendix.

The stress levels used for the creep tests are 150, 160 and 170 M P a. For the 150 M P a tests, engineering pre-strain levels of 5, 10 and 20% were used. For the other two stress levels, the pre-strain levels of 0.5, 5, 10 and 20% were used. Uniaxial creep data at 600 ^∘C was also available for the P91 steel and was used to provide 0% pre-strain creep results [36].

Figure 3 shows the variation of the creep strain, 𝜖 ^c , versus time obtained from the pre-strained creep tests performed at 150, 160 and 170 M P a at 600 ^∘C, where 𝜖 _{p r e} is the total engineering pre-strain. All of the plots exhibit the typical three regions of creep curves, i.e. primary, secondary and tertiary regions, and the experimental output was found to be significantly influenced by the plastic pre-straining carried out before creep testing. Plastic deformation mainly takes place in the pre-straining stage of the test, as the creep step is carried at stress levels well below the material’s yield stress (in it’s virgin state). The effects of plastic strain accumulation in the latter stages of the test (i.e. just before rupture) are not considered hereafter.

The results of the tests performed at 150 M P a (Fig. 3(a)), show that the material exhibited a creep resistance effect, i.e. the minimum creep strain rate decreased and the time to failure increased, for pre-strain levels of 5 and 10%, while, with a pre-strain level of 20%, a creep enhancement effect was found (i.e. the minimum creep rate increased and the time to rupture decreased). When the stress level was 160M P a, see Fig. 3(b), creep resistance effects were found for pre-strains of 0.5 and 5%, and creep enhancement was observed for 10 and 20% pre-straining. For the tests at 170M P a, the material showed creep resistance effects for 0.5% pre-strain only, while, for all of the other cases, creep enhancement occurred, as reported in Fig. 3 (c).

In view of the results shown in Fig. 3, the effects of high temperature plastic pre-strain on creep response of P91 steel may be quantified by two parameters, namely, ϕ and ψ. These parameters account for the variation in the minimum creep strain rate and the time to failure, respectively, due to the application of a total engineering pre-strain level, 𝜖 _t . Equations 3 and 4 defines the ϕ and ψ parameters, respectively, where \({\dot {\epsilon }}^{c}_{MIN,0}\) and t _f,0 are the minimum creep strain rate and the failure time of material under a 0% pre-strain condition (as received), while \({\dot {\epsilon }}^{c}_{MIN,p}\) and t _f,p refer to the material after pre-straining.

In the experimental study conducted by Tai and Endo [38], the ϕ parameter was used to model the variation of the minimum strain rate after pre-creep deformation in a 2.25Cr1Mo steel. In the present work the accumulation of time dependent inelastic strain during pre-straining is considered to be negligible.

For each stress level, the variation of the ϕ parameter with 𝜖 _p was fitted by an equation of the form of equation (5) (see Table 2 for coefficient values) where 𝜖 _p is the plastic engineering pre-strain, expressed as a percentage. The values of each fitting coefficient, obtained for each stress level, was averaged over the three stress levels, in order to obtain an average fitting surface.

Figure 4 shows the ϕ parameter versus the engineering plastic pre-strain and the stress (for creep) obtained from the experiments, together with the average fitting surface (see equation (5)).

Similarly, the rupture data for the pre-strained creep tests was used to determine the variation of the ψ parameter. Equation 6 is the fitting equation used to model the ψ variation versus 𝜖 _p , for each stress level, and Table 3 lists the coefficients of the average fitting.

Figure 5 shows the variation of the ψ parameter with the engineering plastic pre-strain and stress obtained from the experiments, and the average surface (equation (6)).

When ϕ > 1, the material shows an increase of the minimum creep strain rate when compared with the 0% pre-strained condition (hence it exhibits a creep enhancement effect). When ϕ < 1, a creep resistance effect is evident. Similarly, when ψ < 1 the failure life of the specimen increases (creep resistance effect) while, when ψ > 1, the failure time decreases (creep enhancement effect). Both equation (5 and 6) lead to ϕ = ψ = 1 when the plastic pre-strain equals 0, i.e. for the 0% pre-strained condition.

Small punch creep tests were carried out at 600 ^∘C on the same batch of material as that used for the pre-strained tests (see Table 1). A dead-weight machine was used for the SPCTs (see Fig. 6(a) for a cross section of the experimental set-up). The disc specimen was held in place by a clamping ring while it was loaded by the hemispherical end punch. The outer tube and the clamping ring have through-passing holes for the top thermocouple to be inserted. In Fig. 6(b), the dimensions of the testing set-up, which conform to those recommended by the CEN draft code of practice [5], are also shown.

The specimen was clamped by applying a clamping torque to a M25x1.5 thread, connecting the outer tube and the insert tube. The value of the clamping force was controlled by monitoring the applied torque and which is set to 10N m for all of the tests, in order to ensure consistent experimental conditions.

The set-up represented in Fig. 6 was located in a furnace with a single-zone temperature controller. During the tests, the temperature was controlled to 600 ± 1^∘C. Two thermocouples were inserted in the testing set-up (located at the top surface of the specimen and immediately below the specimen) in order to record any temperature fluctuations.

The central deformation of the specimen was monitored by a linear variable differential transducer (LVDT), which measures the displacement of the punch with time.

To date, the magnitude of friction forces acting on SPCT specimen has not been identified in a definitive manner. However, numerical and experimental investigations [39‐41] showed that, for the same test load and temperature, friction has the effect of increasing the time to rupture and decreasing the rate of creep deformation of the specimen. Friction forces generate a bending moment in the specimen which opposes the rotation of the annular region of the specimen in the vicinity of the edge of contact between the specimen and the punch. In turn, the viscous (creep) deformation of the specimen takes place at a lower rate and the failure time is therefore increased [40]. Although SPCT is a static test, the temperature and the test load level in the present investigation are likely to be high enough for the asperity junctions of the punch and the specimen to generate a stick/slip scenario. The generation of such contact regime is intrinsic of this testing typology, therefore, in the present work, it could not be eliminated.

SPCTs were performed with punch loads (P) of 25, 28, 30, 34 and 40k g. Figure 7 shows the experimental output of the tests, i.e. the variation of the central displacement of the specimen versus time. The experimental curves shown in Fig. 7 exhibit the 3 typical SPCT regions described in the literature [1, 20, 42‐44].

The early stage of the test is characterised by a decreasing displacement rate, followed by a stationary region, where the displacement rate reaches its minimum value. The later stage of the tests shows rapidly increasing displacement rate until failure occurs. The fluctuations in displacement found in the early stages of the 25k g test curve were caused by electronically induced noise, caused by interference between two data acquisition system units; this was eliminated in the early stages of the other tests. Figure 8 shows the variation of the minimum displacement rate (MDR) versus the load level, P.

A power law correlation between MDR and P was found and is represented by equation (7), where MDR is expressed in m m/h r and P in kg.

Figure 9 shows the variation of the failure time, t _f , versus load level using logarithmic scales. A power law correlation of t _f with load level, given by equation (8), was obtained.

According to the CEN Code of Practice CWA 15627, the load level, P, must be calculated such that the small punch creep test specimen has the same time to failure as an uniaxial creep test specimen subjected to an equivalent uniaxial stress, \({\sigma _{UNI}^{EQ}}\) [5]. The dimensions of the testing set-up, i.e. R _s = 1.04m m, a _p = 2m m and t ₀ = 0.5m m, were used in equation (9) and the multiplication factor of 0.8 was included because the disc specimens were clamped into the experimental set-up [5], conforming with the CEN code of best practice for SPCT. The k _{s p} parameter is a correction factor describing the effects of the ductility of the tested material at different temperatures. k _{s p} has then been calculated for each load level and it has been found to increase with the load, in agreement with the results of Gülçimen and Hähner [8]. An average k _{s p} value (1.353) was found for the load range used in the investigation.

Interrupted tests were also performed using a load of 25k g in order to investigate the evolution of failure in the specimen during the test. Figure 10 is a plot of the output of the 25k g completed and interrupted tests (at 2, 200, 400 and 669 hrs). As with previous investigations, a significant amount of data scatter in the experimental results was found to exist [4]. In the present investigation, the scatter appeared to be related to the characteristics of the testing machine, and to slight misalignments in the loading punch with respect to the axial direction of the test rig. Detailed numerical investigations of this misalignment are discussed elsewhere [24, 45].

Interrupted test specimens were imaged using Nikon Eclipse LV100ND optical microscope (see Figs. 11, 12 and 13). A crack was found to nucleate at the bottom surface of the specimen at some distance from the axis of symmetry in the 400h r s sample (see Figs. 12(b) and 13(c)) which propagates along a direction at approximately 45^∘ from the loading axis (Fig. 13(b)).

Such a crack has a significant role in the evolution of the apparent creep response of the specimen, as it constitutes the main mechanism which leads to the loss of load carrying capability of the structure and to rupture (through fracture) of the specimen.

An elastic/plastic/creep constitutive model, capable of accounting for the effects of plastic deformations on subsequent creep material behaviour, was used for the FE analyses. The true stress/strain curve, reported in Fig. 14, was approximated from the engineering tensile curve obtained using a stress/strain test of a P91 steel at 600 ^∘C, and it was implemented, in a tabular form, in the FE solver ABAQUS (see Table 4), where σ is the equivalent von Mises stress and 𝜖 _p is the von Mises equivalent plastic strain.

A creep damage model that takes into account the multiaxiality of the stress state, and thus it is suitable for numerical simulations of the small punch creep test, is the Liu and Murakami creep constitutive damage model [35]. Liu and Murakami based their model on those by Hutchinson and Riedel for materials undergoing creep-constrained grain boundaries cavitation [46, 47]. The former stated that a damaged material contains a dilute concentration of microcracks and, as a consequence, the creep strain rate has a linear dependence on the microcrack damage parameter [46]. Riedel extended Hutchinson’s model to non-dilute microcracks assumption, demonstrating the existing of an exponential relationship between the microcrack damage parameter and the creep strain rate for the uniaxial stress state [47]. In the Hutchinson model the creep strain rate is expressed as the sum of the dilatational creep components and the deviatoric creep components. According to Liu and Murakami, the former components are negligible when the material constant n is higher then 3 [35]. In the conventional damage mechanics, the damage parameter, ω, is intended as the ratio between the damaged area, due to material deterioration, and the initial undamaged area, and therefore it ranges from 0, for an undamaged material, to 1, for a failed/fractured material element. By assuming this definition for ω and by considering a cylindrical material cell, whose diameter and height have the same size, containing a penny shaped microcrack, or, equivalently, a cavitated grain boundary facet, Liu and Murakami proved that the damage parameter, ω, is a function of the length and the density of the microcracks and does not depend on the material constant n [35]. Instead the microcrack parameter, ρ, is also a function of n, as shown in equation (10) [35].

In this paper, in order to model the creep behaviour of the material by also taking into account the pre-straining effects in the SPCT, the authors propose a modified Liu-Murakami constitutive model, which was implemented through the CREEP user subroutine in ABAQUS [49]. The modified constitutive equations allow the effects of plastic pre-strain on the minimum creep rate and on the failure life to be included. The Liu-Murakami constitutive model was modified using the ϕ and ψ parameters defined in equation (3 and 4), respectively. Equations 11 and 12 shows the evolution of the creep strain rate, \(\dot {\epsilon _{ij}^{c}}\), (in multi-axial form) and of the damage rate, \(\dot {\omega }\), in the creep constitutive model adopted for the FE calculations, where σ _{E Q} is the von Mises equivalent stress, σ ₁ is the maximum principal stress, S _{i j} is the generic component of the deviatoric stress tensor and B is a material constant. σ _{R U P} is the rupture stress, defined by equation (13). The effects of temperature on the creep behaviour of the material are taken into account by the material constants. It should be noted that, in the Liu and Murakami constitutive model, the rupture stress is a composition of the maximum principal stress and of the von Mises equivalent stress, summarising the multi-axiality of the stress state in a single variable.

In order to include the variations of ϕ and ψ with the plastic strain, equation (5 and 6) were also implemented in the constitutive model. The maximum damage value was limited to ω _{M A X} = 0.9901 in order to avoid numerical problems which arise when ω approaches unity.

In order to account for the loss of load carrying capability due to material creep deterioration, the creep constitutive model is fully coupled with the elastic material properties . The decrease in the stiffness of damaged elements with the increase of ω is governed by equation (14) [35], where E ₀ is the Young’s modulus of undamaged material, and E is the instantaneous modulus corresponding to a damaged element [48].

Table 5 lists the elastic properties and material constants for the Liu-Murakami creep constitutive model obtained for the P91 steel at 600 ^∘C (as received 0% pre-strain condition).

The correlations between pre-strain and the ϕ and ψ parameters were obtained using experimental results where strain levels are taken to be the engineering total strain for the specimen. In reality however, local strains (particularly in the necked regions) can be far greater than the average engineering strain of the uniaxial specimens (discussed in “Material constitutive model”). This is especially true for the high pre-strain level tests. In order to account for this mismatch and to implement a correlation between the true strains and the pre-strain parameters (i.e. ϕ and ψ) in the SPCT model, an additional FE calculation of a uniaxial tensile test of a P91 steel at 600 ^∘C was carried out using the tensile curve described in Table 4. The mesh used is shown in Fig. 15 and it consists of 2974 axisymmetric quadrilateral elements. In view of the symmetry of the uniaxial creep test specimen (see Fig. 2), a quarter section only was modelled.

By using the geometry non-linear (GNL) approach (which updates the stiffness matrix of the structure at each time increment during the analysis) the uniaxial specimen FE model can take into account the large deformations and necking occurring for large engineering strains. Figure 16 is a contour plot of the plastic equivalent strain, expressed in absolute value, for an engineering strain level of 0.122%, while Fig. 17 shows the engineering stress/strain curves obtained from the uniaxial FE model and from a tensile test carried out on a P91 steel at 600 ^∘C.

From the results of the additional uniaxial FE analysis, the variation of the total engineering strain (𝜖 _{t,e n g} ) was related to that of the true equivalent plastic strain (𝜖 _{p,t r u e} ) in the necked section of the uniaxial specimen. Equation 15 was fitted to the FE results, where both 𝜖 _{t,e n g} , and 𝜖 _{p,t r u e} are expressed in absolute value, with a = 0.052, b = 0.118 and m = 0.508 (Fig. 18).

The geometry of the FE model of the SPCT is identical to that used for testing as shown in Fig. 6, with a specimen thickness, t _h , and diameter, D _{S P T} , of 0.5m m and 8m m, respectively, punch radius, R _s , of 1.04m m, receiving hole radius (see Fig. 6(b)), a _p , of 2m m and lower clamp radius of 0.25m m.

Three load levels (25, 28 and 30k g) were applied to the punch in the analyses and suitable boundary conditions were imposed to the degrees of freedom of the rigid bodies which model the components of the test rig. The radial and axial translations and the rotation around the axis of symmetry of the support were constrained. The horizontal translation and the rotation of the punch and of the upper clamp were also constrained. A load of 500k g was applied to the rigid holder (representative of the clamping load resulting from a 10N m tightening torque [45]) in order to secure the specimen between the two dies. Figure 19 schematically shows the loads and the boundary conditions applied to the model.

Since the behaviour of the specimen is characterised by large incompressible deformations due to creep and by severe local loading conditions at the contact edge (between the punch and the specimen), the FE mesh adopted to model the SPCT specimen consists of 883 nodes and 790 bilinear axisymmetric 4-node elements. Figure 20 shows the mesh used for the SPCT FE analyses. 10 elements were used through the thickness of the specimen and the mesh was refined in the region where the edge of contact between the punch and the specimen is located for most of the analysis. The minimum element size, in the refined region, is 0.013 mm.

Quadratic elements (second order formulation) were avoided because, for the present work, they lead to a larger computational cost without producing any increase in the accuracy of the FE solutions as significant plastic deformations occur in the model. The reduced integration formulation was used, in order to avoid “locking” problems and convergence difficulties encountered when ”fully integrated” linear elements were adopted. These problems are due to a non-physical increase of the stiffness of the elements (“parasitic stiffness components” [49]) when bending deformation occurs, such as at the beginning of the creep step in the SPCT analyses, causing non-convergence of the solution. Hybrid formulation elements were adopted in order to avoid numerical singularities, which can occur when standard constant strain elements (such as the 4-node axis symmetric bilinear elements) are used with incompressible deformation fields. The hybrid formulation processes the pressure stress as an independently interpolated solution variable, coupled with the displacement solution [49]. Thus, unstable solutions for the displacement field after an infinitesimal increase of the pressure stress are avoided. In view of these requirements, the CAX4RH element type, available in ABAQUS, was used. The elements are refined near the edge of the unsupported region of the specimen, where significant bending deformation take place, and in the region close to the contact edge between the punch and the specimen, which was identified as the most critical location in the specimen [16, 28, 43].

Surface-to-surface contact interactions have been used for all of the contacting pairs. The contact elements were automatically generated by the solver and consist of stiff springs which, once activated, apply the contact forces to the contact nodes on master and slave surfaces [50]. The activation of contact elements occurs when the interference between the contact nodes is less than the specified tolerance (0 in the present analyses). The stiffness of the contact elements varies non-linearly with the contact penetration (i.e. the non-linear penalty contact formulation was used). This was found to be a critical feature of the FE analyses when material flow due to plasticity and/or creep is included as it directly influences the convergence rate and the accuracy of the solution. Also the slip tolerance under stick conditions (identifying the stiffness of tangential contact elements) significantly affects the convergence rate of both the elastic/plastic and creep steps of the FE analysis. Although the friction coefficient between the specimen and the clamping components, as well as between the punch and the disk, cannot be straightforwardly quantified, for steels at temperatures of 600 ^∘C or higher, a realistic value of the coefficient of friction between the punch and the specimen was found to be 0.3 by Dymáček et al. [41]. It was also demonstrated, by finite element analysis, that friction effects become important when the friction coefficient between the specimen and the punch varies from 0 to 0.5, making the failure life to increase up to 8 times [39, 40]. For this work the Coulomb classical friction formulation was used and the friction coefficients were taken to be 0.3 and 0.8 for the punch/specimen and the punch/clamps interactions, respectively [45]. The Coulomb friction formulation used for the numerical analyses does not account for stick/slip between contact surfaces. During the test the small disc specimen undergoes severe changes in its shape (it gradually deforms into a conical shape). In order to account for large deformation, the geometrical non-linearity formulation (GNL in ABAQUS) has been used for all of the analyses.