Changes of Armature and Valve Body

Get Complete Project Material File(s) Now! »

Analysis

A thorough presentation of the simulation analysis will be conducted in Chapter 4.

ANSYS Workbench

The finite element analysis in this thesis was performed using ANSYS Mechanical 18.2. The simu-lation consisted of three components, the spring element concept, the armature and the valve body. Symmetrical planes were evaluated of each component’s geometry to simplify the simulation and de-crease the time required to solve the problem. ANSYS consists of multiple analysis systems, which is chosen depending on the problem. Static structural is an analysis system which was chosen for the problem in this thesis. Static structural determines stresses, strains and reaction forces caused by steady loading i.e., loads that with respect to time varies slowly. Static structural allows linear or nonlinear behaviors, example of nonlinearity behaviors are large deflections, plasticity, friction coeffi-cient and contacts. This thesis consisted of a nonlinear contact problem which was solved using an implicit solver. The solver consisted of an unsymmetrical Newton-Raphson method.
ANSYS allows multiple number of load steps. Each load step has a virtual time unit of 1. Each load step also consists of points at which solutions are computed, in ANSYS these points are called substeps. The amount of substeps can manually be controlled to obtain convergence. Convergence occurs when the residual, the difference between the external and internal force, is less than the convergence criterion. Error is inherent in nonlinear analysis, convergence criterion is basically the allowance of error, usually in percentage.

Changes of Armature and Valve Body

Unaffected material was removed from the armature and the valve body to simplify the simulation, see Figure 4.1 & 4.2. Dimensional changes of the armature and the valve body were also performed to allow an assembly of an additional component to prevent an increased length or height of the entire valve. Dimensional changes of the armature were an increased inner diameter of the interface and height removal. The diameter was gradually increased to ensure that there was no dislocation of the threads. A greater dimensional interface of the armature allows for additional dimensional freedom of the spring element. To prevent an increased height of the valve with an assembled spring element, the interface was also designed 0.5 mm deeper, which corresponds to the additional height caused by the material thickness of the spring element. The outer surface of the simplified armature was dimensioned equally to the lowest dimensional diameter of the threads, to not add a false material thickness.
Greatest dimensional changes of the valve body were reduction in height, removal of escape passage and simplification of the material thickness, see Figure 4.2. The material thickness was reduced to the lowest value while maintaining the original design. This was performed to achieve a sensitive result whether the inner surface of the valve body would be deformed.

Geometry Optimization

Symmetry planes of the simulation model and removal of unaffected material were utilized to minimize the required computer storage and required CPU time. It was critical to minimize these loads to achieve efficiency while providing enough accuracy of the solution. Minimizing the computer storage of the simulation files and the required CPU time are also essential if additional capacity can not be provided.
The simplified armature and valve body were uniform around Z-axis and could have enabled a 2D simulation. By the design of the spring element concept, the simulation required to be in a 3D-environment since it was not uniform around Z-axis. The final concept of the spring element was optimized with symmetry planes by 1/4 of the original model, see Figure 4.3.
Symmetry settings in ANSYS enables the behavior of a fully scaled assembly in a downscaled model. Validation of the downscaled model was performed with a simple load which was compared to a fully scaled model which also was exposed to the same load. The result displayed equal behavior and values, which ensured a correct downscaled model.

Assembly and Disassembly Simulation

An assembly and disassembly simulation were performed to locate maximum stresses, strains and re-action forces. Maximum stresses, strains and reactions forces were critical values that would determine if the spring element would meet several requirements. Maximum stresses determined if the design and material of the concept were good enough. An analysis of strains would provide data if the crucial surfaces were critically deformed during the assembly. Resulting reaction forces during the simulation provided which assembly and disassembly forces were required. The simulation model was assembled and disassembled using displacements. In ANSYS, displacements are boundary conditions in static structural which displaces a chosen part within the model. Reaction forces are obtained as a displaced component is in contact with another component. The components were displaced in a specific order that allowed for a similar assembly in production. The boundary conditions were also set to enable both assembly and disassembly in one simulation.
The starting position is displayed in Figure 4.4a. In the first load step, the concept was displaced 1.99 mm which presses the concept onto the valve body but leaves a gap of one hundredths mm, which is performed to prevent interpenetration of the inner upper surface of the concept and the outer upper surface of the valve body. The concept was fixed at this position until the last load step. The valve body was fixed during all load steps except the last. In the second load step, the armature was displaced 3.99 mm which was equal to the distance required to press the armature onto the concept and valve body. All parts were in position after the second load step i.e. the assembly was complete, see Figure 4.4c. The disassembly of the model was performed at the fourth load step. The disassembly was performed by displacing the valve body 2 mm. The concept was no longer fixed at the fourth load step, which resulted in a release of the weakest press fit as the valve body was displaced, see Figure 4.4d. Figure 4.4 displays the assembly and disassembly when the press fit of the armature and concept was the weakest.
An additional scenario, which is defined as Worst Case 2 further in this thesis, would occur as the press fit of the valve body and the concept would be the weakest. This resulted in the concept remained it position with the armature as the valve body was displaced 2 mm, see Figure 4.5d. The cause and purpose of this will be explained thorough in Section 4.5
To achieve a valid result of the assembly and disassembly simulation, the model was required to move freely in Z-direction but locked in X- and Y-axis to prevent rotation around Z-axis. This was performed taking production into consideration as no rotational movement would occur during production assembly. A boundary condition that met such requirements was frictionless support. The frictionless support was applied on the faces in X- and Y-axis of the model, see Figure 4.6.

Dimension and Tolerance Evaluation

The dimension of the components was defined as grip, to reduce the parameters from three dimensions to two grips. Grip size allowance corresponds to press fit capacity allowance and was determined by an interval of maximum and minimum grip. Minimum grip was defined by the grip resulting in a disassembly force just above an insufficiently low value. Maximum grip was defined by the grip resulting in a maximum stress within the model just below the ultimate tensile strength (U T Strue) of any material, see Figure 4.7. To achieve dimensions resulting in grips within the interval, trial and error simulations were performed.
The trial and error simulations resulted in partial counteracting press fits. Counteracting press fits were defined as one press fit was reduced as the other was increased. To evaluate tolerance width allowance, worst cases were then created. Worst cases were modeled by components dimensional extremes, which included tolerance widths, to achieve the least favorable combinations. Least favorable combinations of counteracting press fits were achieved by using dimensions and tolerance extremes which caused one maximum grip and one minimum grip.Dimensions of the components were to be determined (TBD). The typical dimensional tolerance ± 0.05 mm of the spring element concept was obtained by Öhlins component supplier which was applied for deep drawing process, see Table 4.1. This was performed to evaluate if the concept would allow coarser tolerances of the armature and the valve body and if it would prevent dislocation of either the valve body or the armature during transportation or production assembly.
The tolerances which the spring element allowed were then extracted by the difference in dimension of each components max and min dimension. Nominal dimension of each component was given by the mean value of max and min dimensions.

Disassembly Force Evaluation

A value of the minimal allowed disassembly force wasn’t stated in the requirement. The result of the disassembly force using spring element would therefore be compared to the total mass of the valve body assembly, MV B, multiplied with the gravitational force, g. The valve body assembly’s weight in [N] is calculated in eq 4.1.

Material Data

The armature is made out of carbon steel alloy which is a processed high carbon chromium bar. A high carbon chromium steel prevents oxidation and it allows cutting processes to achieve the required fine tolerances. The valve body is made of a brass-copper-zinc alloy. The material is easily machined which is essential to achieve the fine tolerances and milling of the escape passage.
The material of the concept had to be chosen before performing simulation the model. The system required material data of all component to compute the stresses and deformations. The material of the concept had to meet several requirements, which were enabling a deep drawing process and allowing great elastic and/or plastic deformation without fracturing. An additional important property was which friction coefficient the material would yield when in contact with the material of the armature and the valve body. A too high friction coefficient would yield high stresses within the materials but the required force to disassembly would potentially be high, which was desired. A too low friction coefficient would result in a potentially low disassembly force. A material that met the requirements was a steel manufactured by SSAB. The elongation of the steel was 34% which defines a highly ductile steel with potentials of meeting the material requirements of a spring element. Further material properties can be seen in Table 4.3. Friction coefficients of material combinations will be presented in Section 4.8.
Isotropic elasticity was chosen in ANSYS material model of the armature’s and the valve body’s material. Isotropic elasticity model only takes materials elastic deformation into account. The material of the spring element concept would experience both elastic and plastic deformation to operate. Two different material models had to be used to enable both, which were isotropic elasticity and bilinear isotropic hardening. Bilinear isotropic hardening sets a linear plastic deformation hardening of the material. Bilinear isotropic hardening required the material’s tangent modulus, which was calculated using the derivation presented in Chapter 2 Strain Hardening.
The material data from SSAB consisted of a range of engineering ultimate tensile strength, 270 – 370 MPa. The true ultimate tensile strength of SSAB Form 03 was calculated using the lowest value of the range (270 MPa), see Figure 4.8. Evaluation using the lowest value of UTS was used to increase the safety margin during a potential production. Linear plastic deformation was chosen because no true stress-strain curve was available and the plastic behaviour was unknown.

Contacts

A contact occurs as two different bodies shares the same boundary. Physical contacts do not interpen-etrate the surfaces. In simulation environment, the system must there for enable settings to prevent the surfaces from interpenetrate. ANSYS offers several contact algorithms which enforces the contact behavior of physical contacts [1]. Contact settings in ANSYS allows the user to set several parameters in which the desired contact behavior is achieved. To achieve a simulation model with high reliability, the contact settings are critical.
Contact Type is a contact setting which defines the type of contact. Frictional contact takes frictional forces into account as sliding of the contact occurs. Contact sliding would occur during the assembly and disassembly and frictional forces would be generated. The model required static frictional coef-ficient of each contact to enable the computation of frictional contact. The frictional coefficient was determined by the materials which were in contact, but also by whether the contact surface of each material was dry or lubricated. The model consisted of a valve body, spring element concept and an armature which yielded two contacts, Brass – Steel (valve body and spring element concept) and Steel
– Steel (spring element concept and armature). All components are manufactured and assembled with a clean and dry surface. Table 4.4 is a summarized table of friction coefficient of material combinations conducted in this thesis. Several simulations revealed that the disassembly force was the most critical parameter. To achieve the absolute worst cases of the disassembly forces, the lowest value of frictional coefficient was chosen of steel – steel contact, which would yield a lower disassembly force.
Frictional Contact was applied on the outer surface of the valve body and the inner surface of the concept, see Figure 4.9. The frictional coefficient was set to 0.35 µs. Frictional Contact was also applied on the outer surface of the valve body and the inner surface of the armature, see Figure 4.10.
The frictional coefficient was set to 0.50 µs.
Frictionless Contact is a contact type which enables contact sliding without generating frictional forces. Frictionless Contact was applied on the upper outer surface of the valve body and the inner
upper surface of the concept, this to prevent the surfaces to stick to each other, see Figure 4.11.
Frictionless Contact was also applied on the outer upper surface of the concept and the inner upper
surface of the armature, see Figure 4.12.
Normal Stiffness Factor determines the stiffness of the contact springs, located at each node. Normal Stiffness Factor can be defined according to eq 4.2
where Fnormal is the finite contact force, knormal is the contact stiffness and xpenetration is the pen-etration of contact surfaces [1]. According to eq 4.2, an increase in contact stiffness would decrease the contact penetration. The solution would be accurate if the penetration was small or negligible. A stiffness factor of 10 was chosen, which was recommended for bulk deformations [7]. Contact springs which determines contact stiffness can be seen in Figure 4.13.
Additional contact settings were set to Program Controlled. Program Controlled property of each contact setting allows the program to set which property of each setting to be used based of its calculations. Program Controlled is set as the default property of each setting in ANSYS. List of all contact settings and each property can be found in [7].

Mesh

A mesh independence study has been performed to analyze the mesh influence of the results. Mesh independence study can be found in Appendix A.
The armature and the valve body were considered non-critical due to the high material thicknesses of the components. The armature and the valve body were assigned an element size of 1.00mm. Relevant values of stresses and strains of the non-critical components were expected to emerge just below contact surfaces. Inflation layers of the mesh model were applied on each contact surface of the non-critical components. Inflation layers provides user defined number of layers below a desired surface. Inflation layers enables a more accurate value of stresses and strains to be obtained close to surfaces using a coarse mesh of the entire model. Five inflation layers were applied on the armatures inner surface and the outer surface of the valve body, see Figure 4.14. A mesh of element size 0.33 mm was applied on the valve body’s upper surface. No critical values of stresses or strains were expected on the surface, however a finer mesh was required for the model to perceive the contact between the valve body’s upper surface and the spring element’s inner-upper surface. The result of the final mesh of the model can be seen in Figure 4.14. The model consisted of 60238 nodes and 48351 elements total.
Element order of the mesh was set to program controlled. Program controlled element order enables different element orders within the mesh. ANSYS defines element orders by element descriptions. The model was given element descriptions SOLID186 and SOLID187.
SOLID186 is a quadratic element order. A SOLID186 element is defined by 20 nodes, each with three degrees of freedom. SOLID186 can be defined in several options displayed in Figure 4.15. A high order hexahedral element provides a highly accurate result due to increased number of nodes. Hexahedral element however causes an increased computation time and complicates the implementation within complex shapes. Hexahedral elements were implemented by using inflation layers setting of the contact surfaces. The mesh model also consists of a high order prism. This is to enable the transformation of element shapes hexahedral and tetrahedral. [8]
SOLID187 defines a tetrahedral element with quadratic order, see Figure 4.16. The element consists of 10 nodes, each with three degrees of freedom. Compared to hexahedral elements, tetrahedral elements are more easily fitted into complex shapes and decreases the computation time due to lower number of nodes. Tetrahedral elements have been implemented of the body sized mesh of every component within the model. [9]

Escape Passage Evaluation

Two methods were used to evaluate the escape passage capacity, since two different methods with a similar result increases the reliability of the result. The first method was performed by using the derivation expressed in Chapter 2 Fluid Dynamics. Two points were required i.e, two areas within a streamline as which the fluid behavior was studied. The derivation in Fluid Dynamic theory neglected the potential energy if the height of two points in relation to a reference plane is equal. Since the height of a valve, let alone the relative height of the pilot stage, is only a few centimeters, the potential energy could be neglected. The second point within the derivation was determined by the minimum cross-sectional area of the spring element’s escape passage. The first point was obtained by the definition of the initial requirement in combination of the derivation expressed in the Fluid Dynamic section. The initial requirement stated:
The escape passage of the spring element must not result in pressure drop of the pilot stage.
The derivation expressed by Bernoulli’s equation and the continuity equation of fluids stated that the final pressure was determined by the relation of two points within a streamline. The requirement also specified for the pilot stage. This resulted in the first point of the derivation was obtained by the lowest cross-sectional area of the pilot stage during an uncompressed the flow. This point can be seen as “pd-restriction” in Figure 1.3. Pd-restriction consists of three holes on a component called Pilot Seat. To prevent a pressure drop within the pilot stage, the summarized area of the spring element concept’s escape passages was required to be equal or greater than the summarized passage area of the pilot seat.
Instead of using the derivation expressed in previous chapter of fluid dynamics, the second method was performed by analyzing the current escape passage capacity. Current escape passage capacity has not created a pressure drop within the pilot stage, which is a result of an escape passage with sufficient capacity. The spring element’s escape passage would meet the requirement if its capacity was equal or greater than the capacity of the current escape passage, which is the milled surface of the valve body. Calculation of the minimum cross-sectional area of the current escape passage was calculated to yield a safety factor of 4 compared to the pd-restriction.

Results

This chapter presents the result of concept development and the result of the final concept evaluation using finite element analysis.

Final Spring Element Concept

The final spring element concept is a cup half bulged in the shape of an ellipse, see Figure 5.1. SSAB’s Form 03 was selected as the material of the spring element concept which is a high performance ductile steel recommended for deep drawing process. The concept has a positive draft and an even material thickness which are required when using deep drawing as a manufacturing process. The cutout of the upper surface can effectively be manufactured by one punch solely. The cutout enables the hydraulic flow passage. The concept is 6 mm deep and has an inner bend radius of 0.5 mm which yields a bend allowance of 1.04 mm. Insufficient material data has been provided to validate if the bend allowance is acceptable and at what degree dilutions would occur using deep drawing. By nominal dimensions, the greatest width of the concept is 22.35 mm. The concept is designed to minimize required material removal of the armature and the valve body.
The concept was designed to maximize the spring functionality with every other requirement taken into account. Maximum spring functionality is achieved by a maximized lever arm distance to a press fit. An ellipse shaped concept was determined to allow maximum spring functionality as its lever arm distance is solely limited by the size of the concept. An ellipse is defined by two axes, a major axis and a minor axis. The internal press fit, the interference of valve body and concept, was achieved by the minor axis of the concept was lower dimensioned than the outer diameter of the valve body. This yielded a symmetrical variable press fit but it prevented an uniform press fit, see Figure 5.2. To minimize stresses within the material and simplifying the assembly, the chamfer angle of the valve body was steeper designed and the chamfer fillet was increased. Larger fillet of the valve body and larger radius of the inside bulged radius yielded a softer assembly.
Using an ellipse shaped concept also yielded critical parameters. Displayed in Figure 5.2b, the di-mensional difference of an ellipse shaped concept and a circular shaped valve body formed the escape passage. By the spring functionality of the spring element concept, the escape passage capacity would decrease as the external interference was increased. The escape passage gap was solely determined by the interference which determined the dimension and tolerance of the armature. Both enabling a hy-draulic flow and allowing for a wider tolerance range were parameters which must not be compromised. The gap of the escape passage could be increased by increasing the major axis of the concept, but it would have required additional material removal of the armature’s interface, which could potentially have caused the threads of the other armature surface to dislocate.
By rotating the sectional side view 45° around Z-axis and lowering the sectional top view in Z-direction of the previous figures, interferences of the external press fit can be displayed, see Figure 5.3. The spring element concept also yielded a symmetrical variable press fit but prevented an uniform external press fit. The ellipse shaped concept enabled a hydraulic flow to pass through the two dimensional differences and by the punched out surface of the concept, see Figure 5.3a. This enables a symmetrical hydraulic flow and a symmetrical press fit. This would not be possible using a circular shaped spring element without compromising spring functionality or symmetry requirements. The bulged angle was a critical parameter. A too large bulge angle would have yielded an increased disassembly force, but it would increase the required assembly force and stresses within the material significantly. It has been designed taking both parameters into consideration.
By using the ellipse shaped spring element, the press fits were predicted to counteract, which was justified by previously mentioned nominal simulations. Counteracting press fits are a critical weakness which may result in a too low disassembly force. Simulations of a concept with no bulge resulted in fully counteracting press fits. The bulge was additionally added to potentially decrease the relation of the counteracting press fits. The bulge could potentially decrease the relation causing counteracting press fits by preventing a uniform shaped concept in Z-direction. The bulge also enables for an easy assembly as the press fit is gradually increased.

Contents
Abstract
Sammanfattning
Preface
1. Introduction
1.1. Background
1.2. Problem Description
1.3. Purpose and Aim
1.4. Delimitations
1.5. Outline
2. Theory
2.1. Connection Between Problem and Theories
2.2. Fluid Dynamics
2.3. Dimensional Tolerances and Interference
2.4. Contact Mechanics
2.5. Material Science and Engineering
3. Method
3.1. Concept and Evaluation Study
3.2. Validity and Reliability
4. Analysis
4.1. ANSYS Workbench
4.2. Changes of Armature and Valve Body
4.3. Geometry Optimization
4.4. Assembly and Disassembly Simulation
4.5. Dimension and Tolerance Evaluation
4.6. Disassembly Force Evaluation
4.7. Material Data
4.8. Contacts
4.9. Mesh
4.10. Escape Passage Evaluation
5. Results
5.1. Final Spring Element Concept
5.2. Tolerance Widths
5.3. Worst Case 1
5.4. Worst Case 2
5.5. Escape Passage
6. Discussion
6.1. Implications
6.2. Lessons Learned
7. Conclusions 52
7.1. Requirements Summary
7.2. Answered Issues
8. Future Work
GET THE COMPLETE PROJECT