2.2.1. Material Model
There are two simulation parts with regard to composite and processing modeling, respectively. Composite-material modeling is built by Digimat-MF. Digimat is linear and nonlinear multiscale-material modeling software (Digimat 2017.0, MSC software, Los Angeles, CA, USA) that accurately predicts the nonlinear microscopic behavior of complex multiphase composites and structures (e.g., PA, PA66, ABS, and nano-reinforced composites), and the constitutive behavior of various materials. The material properties of raw materials are input to the software user interface.
The composites’ performance prediction by Digimat-MF is including thermal–mechanical analysis and thermal analysis.
1. Mechanical analysis
(1) Linear Elastic Model
The material model of carbon powder is a linear elastic model. The stress-strain relationship of elastomers can be described by Hooke’s law shown as Equation (1):
C is Hooke’s operator, σ is stress, and ε is strain.
The distribution of carbon powder in composites has no fixed direction. The properties of the material are independent of the loading direction under consideration. At this point, the Hooke’ operator only needs to be represented by two engineering constants: Young’s modulus and Poisson’s ratio shown as Equations (2) and (3).
E is elasticity modulus, is Poisson’s ratio, G is shear modulus, and K is bulk modulus.
(2) Elastic-plastic Model
The material model of PA66 is elastic-plastic model. The elastic-plastic constitutive model provided by Digimat-MF is
J2 plastic model. And the plastic cumulative hardening stress solution model is Equation (4):
is hardening stress, is cumulative plastic strain, is hardening modulus, m is the hardening exponent, k is the linear hardening exponent.
With temperature changing, the thermal strain occurred to the material besides elastic strain and plastic strain. Thermal strain is isotropic, which is the function of actual temperature
T, reference temperature
Tref and initial temperature
Tini shown as Equation (5):
is the coefficient of thermal expansion.
2. Thermal analysis
Digimat-MF only provides a model for thermal analysis: Fourier model. The formula is shown in Equation (6).
, c, T, t, q, r represent density, specific heat, temperature, time, heat flow, and volume heating, respectively.
If only a single thermal conductivity is considered, according to the Fourier law, the heat flow is expressed as Equation (7).
is thermal conductivity matrix. When the material is isotropic, the matrix can be expressed as Equation (8).
k is thermal conductivity.
In this study, carbon powder was seen as a linear elastic model. The material properties needed to be input, including elasticity modulus, Poisson’s ratio, and coefficient of linear expansion. Then, carbon-powder size and shape were input. PA66 was viewed as elastoplastic material which is shown in
Figure 1.
The constitutive curve needed to be imported to build the material model of PA66 and carbon powder. For this purpose, the latent heat of the phase change was expressed by equivalent heat capacity, the specific heat of PA66 changing with the temperature needed to be input. The specific heat capacity and constitutive curve of the raw materials were measured by differential scanning calorimeter (DSC, HESON, Shanghai, China) and universal electronic testing machine (Yangzhou drei instrument equipment co. LTD, Yangzhou, China), respectively. The remaining physical-performance parameters were given by the manufacturer. Carbon content was changed from 0% to 20% to observe the numerical results of linear expansion coefficients and the constitutive curves that are mainly material elements to affect thermal deformation; parameters are shown in
Table 1 and
Table 2. Digimat, based on mean-field homogenization, homogenized the original material. Therefore, thermal composite deformation with proper mass fraction was obtained by simulation, which was later experimentally verified. The predicted composite model was the material model in the ANSYS thermal–mechanical coupling.
2.2.2. FDM Numerical Processing
Thermal–mechanical coupling analysis during FDM processing was carried out with ANSYS. ANSYS is a large general-purpose finite element analysis (FEA) software developed by ANSYS corporation of America (15.0, USA). It is used to solve structural, fluid, electrical, electromagnetic and collision problems. The birth and death element are a function in ANSYS. To achieve the “element death” effect, the program does not actually remove “killed” elements. Instead, it deactivates them by multiplying their stiffness (or conductivity, or other analogous quantity) by a severe reduction factor (ESTIF). This factor is set to 1.0 × 10−6 by default, but can be given other values. Element loads associated with deactivated elements are zeroed out of the load vector, however, they still appear in element-load lists. Similarly, mass, damping, specific heat, and other such effects are set to zero for deactivated elements. The mass and energy of deactivated elements are not included in the summations over the model. An element’s strain is also set to zero as soon as that element is killed. In like manner, when elements are “born”, they are not actually added to the model; they are simply reactivated. All elements are created, including those to be born in later stages of analysis, while in PREP7. It is not allowed to create new elements in SOLUTION. To “add” an element, the performer first deactivates it, then reactivates it at the proper load step. When an element is reactivated, its stiffness, mass, element loads, etc. return to their full original values. Elements are reactivated with no record of strain history (or heat storage, etc.); that is, a reactivated element is generally strain-free. Initial strain defined as a real constant, however, is not be affected by birth and death operations.
At the beginning, every element is “dead”. If the position accumulated by material is activated, the physical performance parameters are back to normal. The function was used to imitate the process of accumulating material. Every element that needed to be activated was a 0.4 × 0.4 × 0.2 mm3 cuboid. The whole model was 8 × 2 × 2 mm3, which means that the total number of elements were 1000. And there are 1386 nodes. At the beginning, every element was “dead”, which means that the element parameters were multiplied by a value close to 0. The accumulated position with the material was activated. Composite-material modeling in ANSYS was from the Digimat numerical results. The type of elements used in thermal analysis is solid70. Then, that in mechanical analysis is changed into an equivalent structural element solid45. The model surfaces except underside had natural convection with the air. Environment temperature was 15 °C. The underside surface had heat conduction with hot bed. The temperature of hot bed was 70 °C, 80 °C, and 90 °C. According to the experiment, the polymer’s thermal convection coefficient under natural convection was around 72. In this paper, PA66’s thermal convection coefficient was 72 and the thermal conductivity was predicted results from Digimat. The heat source was nozzle whose temperature was from 240 °C to 260 °C. The underside surface was stuck to the hot bed, so it had no deformation. The displacement of underside is 0 in three directions (x, y, and z). The results of thermal analysis are as the loads in mechanical analysis in order of time.
The thermal–mechanical coupling simulated the temperature change during FDM. Then, warp and thermal-deformation displacement occurred.
The parameters analyzed by ANSYS included nozzle and hot-bed temperature, the ratio of extrusion speed to filling speed, and aspect ratio. The reason for choosing these parameters is as follows. Hot-bed and nozzle temperature directly determine specimen temperatures. Aspect ratio is defined as, assuming that the nozzle moving direction is in the x direction of a specimen, the size ratio of the x direction to the y direction of a specimen is the aspect ratio. The aspect ratio affects specimen-temperature distribution. The ratio of extrusion speed to filling speed is an important element impacting processing quality. A poor ratio leads to the discontinuity of the formed material, and if there are bubbles in the specimens, the heat-conducting property and mechanical strength are affected. The numerical model was obtained shown in
Figure 2.