Vibration characteristics and modal analysis of a grinding machine

2.1. Experimental modal analysis theory

For a damped mechanical member during resilient movement, the discrete component can be expressed as a linear differential equation as shown in Eq. (1) [7]:

where $\left[M\right]$ is the mass matrix, $\left[C\right]$ is the damping matrix, $\left[K\right]$ is the stiffness matrix, $\left\{\ddot{x}\right(t\left)\right\}$ is the acceleration vector, $\left\{\dot{x}\right(t\left)\right\}$ is the velocity vector, $\left\{x\right(t\left)\right\}$ is the displacement vector, and $\left\{F\right(t\left)\right\}$ is the force vector.

By applying a Laplace transform, the linear differential equation is transformed from the real domain to Laplace domain. The Laplace domain equation is shown in Eq. (2):

where $\left\{X\right(s\left)\right\}$ is the displacement of the Laplace transform, $\left\{F\right(s\left)\right\}$ is the force vector of the Laplace transform, $\left\{x\right(0\left)\right\}$ is the initial displacement vector, $\left\{v\right(0\left)\right\}$ is the initial velocity vector, and $s$ is the Laplace variable.

If the Laplace parameter $s$ is replaced by $j\omega$, the frequency information can be obtained as follows:

(1) Homogeneous solution:

$\left[P\right(s\left)\right]=s^2\left[M\right]+s\left[C\right]+\left[K\right]$ is the system matrix.

If $G_k$ is the solution of the system matrix that makes the determinant of $\left[P\right(G_k\left)\right]$ equal to zero, then $G_k$ is the eigenvalue. The corresponding eigenvector is called the modal shape. The eigenvalue and eigenvector are given as follows:

where ${\sigma }_k$ is the $k$th modal damping and ${\omega }_k$ is the $k$th modal frequency.

(2) Particular solution:

The force vector of the linear differential equation is nonzero, and $m$ eigenvectors describe the particular solution of the equation as follows:

where $\left[H\right(s\left)\right]$ is the transfer matrix.

The determinant of the system matrix $\left[P\right(s\left)\right]$ is the quadratic function given in Eq. (3):

where $G_k^{*}$ is the complex conjugate of $G_k$. The inverse matrix $\left[H\right(s\left)\right]$ is shown in Eq. (4):

The denominator of $\left[H\right(s\left)\right]$ is a quadratic function; by using the remainder theorem, Eq. (4) can be rewritten as follows:

where $\left[r_k\right]$ is the $k$th complex matrix and $\left[r_k^{*}\right]$ is the complex conjugate matrix of $\left[r_k\right]$.

Eq. (6) expresses $\left[H\right(s\left)\right]$ in the form of a mode vectors:

where $\left\{u_k\right\}$ is the $k$th modal vector, $\{u_k{\}}^{*}$ is the complex conjugate of $\left\{u_k\right\}$, $\{u_k{\}}^t$ is the transposed vector of $\left\{u_k\right\}$, and $\{u_k^{*}{\}}^t$ is the transposed vector of $\left\{{u_k}^{*}\right\}$.

2.2. Experimental modal analysis

Experimental modal analysis is illustrated in Fig. 1. The process can be divided into four stages:

(1) Measuring technology: Appropriate measuring instruments were used to measure the analyte in order to obtain the input and output response. A hammer, an accelerometer, and a spectrum analyzer were used as shown in Fig. 2.

(2) Signal analysis: The resulting input and output signals of the time-domain response signal were used for signal processing, for example, through Fourier transformation. This study used a time-domain input signal and a frequency-domain output signal as shown in Fig. 3.

(3) Curve fitting: Curve fitting techniques were used to obtain the modal parameters of the system as shown in Fig. 4.

(4) Data analysis: Using curve fitting calculate the modal is necessarily all true [8], which through the damping ratio between 1 % and 5 % to obtain correct modal parameters. The natural frequency and modal damping ratio of the machine tools are shown in Table 1.

Fig. 1Experimental modal analysis

Fig. 2Equipment

a) Hammer

b) Accelerometer

c) Spectrum analyzer

d) Precision grinding machine tools

Fig. 3Tap the signal curve

a) Signal curve

b) Frequency response

Fig. 4Curve fitting

a)

b)

3.1. Finite element modeling and meshing

In this study, the machine tool model was prepared from casting drawings. The model included the internal structure and components, omitting the fillets and holes. The entire machine tool model is shown in Fig. 5. This study used the SOLID187 and COMBIN14 elements to simulate contact rigidity. The free mesh function and SOLID187 were used for the machine tool model, and COMBIN14 was used for simulation of contact rigidity. The finite element model is shown in Fig. 6. The convergence curve is shown in Fig. 7. The element mesh size(body size) is 0.05 m and in the circle model element size (body size) is 0.01 m.

Fig. 5Machine tool model

Fig. 6Finite element model

Fig. 7Convergence curve

3.2. Materials and calculation of support rigidity and finite element model planning

In this study, grey cast iron was used as the material of the model and medium carbon steel was used for the three-axis linear ball screw and linear guideway. The spring constant was obtained through trial and error adjustments of the rigidity of the bottom support of the machine tool, which make setting $X$, $Y$, and $Z$ directions. The setting schematic diagram and position are shown in Fig. 8, and the copy node was bound. The subparts of the finite element model are spindle head, column with spindle head, and bottom with workplane, which do not share any nodes. The finite element model subparts and the experimental modal analysis model are shown in Fig. 9. The material properties and support rigidity are given in Table 2.

Fig. 8Setting schematic and support position

a) Setting schematic

b) Support position

Fig. 9Finite element model subparts and experimental modal analysis models

a) Spindle head

b) Column with spindle head

c) Bottom with workplane

3.3. Contact rigidity calculation

The contact rigidity between the linear guideway and linear slide was obtained from the design catalog. The contact rigidity has only two directions: vertical rigidity and lateral rigidity. The direction of the linear slide withstanding force is shown in Fig. 10. The contact rigidity is given in Table 3.

The linear ball screw nut and support bearing rigidity can be calculated using Eq. (7) [9]:

where $K_B$ is the axial rigidity of the support bearing, $F_{a0}$ is the withstanding pressure, and ${\delta }_{a0}$ is the axial displacement. The equation for axial displacement is given below:

where $Q$ is the axial load, $D_a$ is the diameter of steel ball bearings, and $\alpha$ is the bearing contact angle. The equation for axial load calculation is given in Eq. (9):

where $Z$ is the number of balls. The calculation parameters for the axial rigidity of support bearings can be obtained from the design catalog. In this study, the rigidity of the linear ball screw nut was calculated. Moreover, the linear ball screw prepressed value can be calculated as shown in Eq. (10) [10-12]:

where $T_p$ is the reference torque (kgf·cm), $l$ is the lead, $\beta$ is the lead angle, and $F_{a0}$ is the prepressed value (kgf). The unit length of the calculated prepressed was measured in centimeters. The axial rigidity can be calculated as shown in Eq. (11) [9, 12, 13]:

where $K_n$ is the axial rigidity of the ball screw nut (N/μm), $C_a$ is the basic dynamic load rating (N), $K$ is the original rigidity of the ball screw (N/μm), $\epsilon$ is the basic dynamic load rating coefficient, which was assumed to be 10 % of the dynamic load rating for obtaining the nut axial rigidity.

The linear ball screw was subjected to axial rigidity, and the three-axis nut axial rigidity is shown in Table 4. The axial rigidity of the three-axis support bearing was 980 N/μm.

3.4. Construction of a cylindrical coordinate system and node coupling

In precision grinding, the finite element model of the three-axis linear ball screw was used to establish the respective cylindrical coordinate system to transfer the DOF nodes of COMBIN14. The cylindrical coordinates for each linear ball screw are shown in Fig. 11. The COMBIN14 elements were used to simulate the linear ball screw nut and bearing axial rigidity. Moreover, the COMBIN14 elements were used to choose the $r$ direction of the linear ball screw coupling two nodes DOF. To avoid self-rotation, they are bound by the rotation of the motor so that the elements nodes are coupled in the $\theta$ direction at the end of the COMBIN14 elements. The cylindrical coordinates coupling of two nodes DOF; the settings of all linear ball screws are shown in Fig. 12.

The ANSYS modal analysis model was used to solve the ideal model without damping; therefore, the results of ANSYS modal analysis and experimental modal analysis will have some error. In this study, the results of ANSYS modal analysis and ME'SCOPE modal analysis were obtained for only five frequency and mode shapes. The complete settings of the finite element model are shown in Fig. 13.

Fig. 10Direction of linear slide withstanding force

a)

b)

Fig. 11Cylindrical coordinates of each linear ball screw

Fig. 12Coupling of cylindrical coordinates and the settings of linear ball screws

a) Cylindrical coordinates of two DOF nodes

b) Linear ball screws of the model

Fig. 13Complete finite element model

4.1. Natural frequency value comparison

The experimental process was assumed to be free from human error. The dynamic characteristics obtained through the experimental modal analysis were similar to the actual results. The experimental modal analysis results obtained in this study were the contact rigidity set reference. A comparison of the natural frequency of the five groups obtained through experimental modal analysis and finite element analysis is shown in Table 5 and Fig. 14. The error of 1.3 % for the second group was the optimal result obtained.

Fig. 14Natural frequency comparison

The ANSYS finite element model ignores the fillets and the gap between the structures; the ANSYS modal analysis process has no damping, thereby resulting in the error. In the experimental modal analysis, the first group exhibited a low-frequency signal interference because of the size of the hammer.

Fig. 15Five groups of corresponding mode shape

a) Comparison of first group

b) Comparison of second group

c) Comparison of third group

d) Comparison of fourth group

e) Comparison of fifth group

4.2. Comparison of modal shapes

In the experimental modal analysis and finite element analysis, the natural frequency was divided into five groups; because of the size of the hammer, natural frequency error resulted in a signal interference of mode shape in the first group. The five groups corresponding to the natural frequency of mode shape are shown in Fig. 15.

4.3. Analysis of results for a precision grinding machine

In this study, the operating speed of the precision grinding machine was 15.000-26.000 rpm; therefore, model shapes from 250-500 Hz were discussed. For the given operating speed, the spindle head causes larger vibration than do any other structures. The relative movement of the structure is shown in Table 6.