In the 60’s ASEA was a big user of NC machines and had their own NC control systems developed. They began working on their own industrial robot, after seeing a great potential in the Unimate robot but not getting the license to manufacture it. After testing concepts they decided to go with an electrical robot (Wallén, 2008, 10-11).
In 1974 the IRB 6 stood ready as “the world’s first microcomputer controlled electric industrial robot” (ABBa, 2015). In 1975 they started exporting the IRB 6 and the development of robots continued as they acquired a lot of industrial robot related companies. Later the IRB60 hit the market and it stayed there with the IRB6 for 17 years (Wallén, 2008, 11). ASEA merged with Brown Boveri et Cie in 1987 to form ABB (ABBb, 2015) and has since then developed and released a wide range of industrial robots designed for many applications.
Today ABB is one of the leading industrial robot manufacturer and they have research and development in several countries around the globe (ABBc, 2015).
The finite element method is a way to solve problems by defining a phenomenon as partial differential equations and then solving them approximately. By doing this, it is possible to analyze structures and systems before they are built. When analyzing the design and mechanical properties of an arbitrary structure with FEM, it is divided into several smaller elements. The smaller (and therefore larger in numbers) the elements are, the more accurate the approximated solution will be. By doing this, it is possible for a computer to solve the equation system and give the user information on stresses and displacements in the structure (Fish, Belytschko, 2007, 1)
Nowadays the finite element method is used everywhere as a tool for engineers and scientists to make calculations and predictions of how an object, system and construction will act and behave. Usually the finite elements are created from a CAD-model, which makes it easy to mesh the structure and make the appropriate changes for the simulation (Dhatt, Touzot, Lefranҫois, 2012, 1-3).
Meshing is the process of generating the elements (Fish, Belytschko, 2007, 1) in either 1D, 2D or 3D elements. There are also 0D elements which will not be included in this report. Meshing can preferably be made with different densities depending on what regions are of interest.
Thesis – SIMPLIFIED FINITE ELEMENT BEARING MODELLING – WITH NX NASTRAN 1D and 2D elements can be used in a number of ways to either predefine the outlines and nodes of the 3D elements or to simplify the model to make the calculations less complex. All elements are built from nodes that define the coordinates of the elements.
Some of the earlier work on this subject are two papers, a master thesis by Emil Claesson (2014) about finite element modeling in the solver ABAQUS and a research article about simplified modelling for needle roller bearings by Molnár et al (2010).
In Emil Claesson’s master thesis (2014) he built one very simplified model consisting of coupling nodes and spring elements (Claesson, 2014, 8). The other two of his models are more complex and built with the inner and outer rings modeled in finite elements. In those models a big focus is on the rolling elements, correct stiffness and the force distribution on the raceways. For this, he used rows of spring elements in both models (Claesson, 2014, 10-14). In the same paper (2014, 18) the computing time for the most complex model is about 8 500 times the simplest.
Molnár et al developed two models (2010). One is similar to the ones in Claesson’s paper (2014) with rows of spring elements and the other is a bushing replacing the rolling elements altogether. The springs in the first model are acting differently depending on the load, with no stiffness when they are “outside of the loaded zone” (Molnar et al, 2010, 30-31).
Claesson’s models are verified with a reference model, a “fully” modeled finite element needle roller bearing, “with satisfactory result” (Claesson, 2014, I). Molnár et al finds their models to be applicable for practical use (Molnár et al, 2010, 32).
NASTRAN is a structural analysis software developed by NASA in the 60’s for the aerospace engineers to analyze the structures of space- and aircraft (NASA, 2008). Siemens software NX has the Nastran FEA built in to the structural analysis part of the program. It is capable of several different kinds of analyzing, including linear, nonlinear, durability and fatigue analysis (Siemens, 2015).
Development of the methods
The development of the methods was conducted using two kinds of structures with very basic geometries, see figure 2-1. By using these structures instead of the Lower Line wrist, the many test-simulations could be done in short time.
Figure 2-1 The two kinds of structures the development of the models were performed on Both structures were used to figure out how the different elements could be used to simulate the load of the bearing. In the one without a shaft the loads were applied to a single point in the center of the hole of the structure. This was useful when testing the models that don’t require the CBUSH element.
The structure with a shaft is more similar to the setup of the wrist which made it suitable for testing both CBUSH-based methods and the finalization of all the methods. The loads are put on the shaft by connecting a RBE2 to the end and applying one or more forces to the dependent node.
One dimensional elements and mpc’s
These are special elements that are used in the creation of the bearing models. They are used as connections with the intention to mimic some of the features of the actual deep grove ball bearing and lighten the load instead of using the computing power demanding tetrahedral elements.
RBE2 and RBE3
The RBE2 is a multi-point constraint that is useful in many ways in finite element modeling. Although the name is a little misleading, it resembles a one dimensional element in its graphical representation (Predictive Engineering Inc, 2013, 6). Simply put, it works by enforcing the connected nodes to keep the internal coordinate positions in between themselves. The RBE2 is made up of a dependent and an arbitrary amount of independent nodes, and the behavior of it is determined by the DOF of the nodes. The standard is that the independent node have six DOF and the dependent are more restricted. (Predictive Engineering Inc, 2013, 10).
The RBE3 isn’t rigid in the same manner as the RBE2. According to the authors of Small Connection Elements one should “think of them as small little free bodies floating in space. They need to have sufficient DOF defined to be stable but not more” (Predictive Engineering Inc, 2013, 12). Siemens Quick reference guide describes the RBE3 as an interpolation constraint element:
“Defines the motion at a reference point as the weighted average of the motions at a set of other grid points” (Siemens Product Lifecycle Management Software Inc, 2011, 1987).
In a technical note Mark Robinson (2008) similarly explains how the RBE3 works. It uses motion of a set of nodes to calculate how one or more nodes should move. This makes the RBE3 a good element to carry loads without over constraining the connection. (Robinson, 2008).
To illustrate how they differ this simple model is built. In figure 3-1 two circles are defined on a surface. A point-to-surface-connection is made for a RBE2 and a RBE3, and then a force is applied on each of the independent nodes.
According to the authors of the Predictive Engineering paper one of the major functions of the RBE3 is to evenly distribute a force “from the independent node to the dependent nodes” (Predictive Engineering Inc, 2013, 11). In figure 3-2 this feature is made visible.
Figure 3-2 The resulting deformations of the RBE3 and RBE2. Isometric view (left) and a sectional view (right).
The RBE3 balances the force distribution and it looks like a bag of liquid is the load, with stresses throughout the area of the dependent nodes. The RBE2 on the other hand have all the stresses in the perimeter of the circle with dependent nodes.
In the wrist model the dependent nodes of the RBE3s will be connected to the surface and point of a hole. Figure 3-3 show what the deformation looks like when radial forces are applied.
CBUSH is a spring element with the added features of viscosity and damping, figure 3-4. It is used instead of the spring element CELAS because the CELAS has been problematic (Predictive Engineering Inc, 2013, 22).
Figure 3-4 The red jagged line is the CBUSH, connecting two RBEs, it’s modeled less than 1mm long
The CBUSH has many variables to adjust. Stiffness and DOF control are the major features used in this report. It can easily be set with different stiffness’s in different directions which makes it excellent when it comes to simplify things in the FE model.
The CGAPs are used as linear contact elements when using the SOL101 solver. It is defined with an element vector and four physical property parameters in the PGAP. That includes:
• Initial opening of the gap
• Stiffness when the gap is closed
• Translational stiffness when the gap is closed
• Friction of the gap
Generally when constructing the bearings in this report, as the CGAP is not desired to be the element to define the stiffness, the parameter for stiffness when the gap is closed is set to 1015 N/m. The friction is set to 1 and the other parameters are set to 0. Setting the translational stiffness to anything else than 0 has not had any impact on the solutions, except returning errors when defined too stiff. The CGAP elements are quite hard to get to work properly and the parameters have to be set right to avoid strange results.
The linear contact element works by making the solver iterate the simulation so that it can adjust the conditions when contacts occur. This removes the true linearity of the SOL101 but it is still linear calculations between the iterations.
The CGAP is dependent on the user defining a coordinate system for it. The element itself consists of three axis and an orientation vector (Siemens Product Lifecycle Management Software Inc, 2011, 1175). The orientation vector cannot be parallel with the x-axis or NX will return error messages about it. This causes a few problems since, apparently, similar constructions need to have the CGAP coordinate system defined differently.
When using CGAP elements the parameters of the solver has to be tweaked, according to the Siemens NX Nastran support.
In the solver settings there are four important parts:
• the “element iterative solver” is enabled
• the “Treat CGAP as Linear Contact Element” is enabled
• in the system cells the “OLDGAPS(412)” is activated on 0 (default)
• “User defined text” modelling object is created
(Djeni, 2015). See figures 11-6 to 11-8 in appendix C for clarification.
The first activates the iterating process of the solver. When working with contacts the conditions change as elements collide with each other. The second does just what it is called, it makes the CGAPs acting as contacts in the linear solver. The third makes sure that it uses the NX 9.0s way to solve the gaps. The last one is necessary to create a BCSET card which defines contact in the solver (Siemens Product Lifecycle Management Software Inc, 2011, 1175).
In a query about the CGAP-elements David Whitehead, product support at Siemens Industry Software, stated:
In my experience, I would say that getting models which include CGAP elements to work properly can be somewhat fiddly, particularly if there are a number of them. I’m not sure that there are any ‘hard and fast rules’ which can be used to guarantee success in every case. (Whitehead, 2015)
The CBEAM is a one dimensional beam that can be assigned material and geometric specifications. Even though the element itself is one-dimensional the solver calculates the stresses and strains based on the physical properties given to the element.
These 3D solids, tetrahedrals, are common elements in finite element structures. They look and behave like real structures which make them preferred when building finite element models. The nodes in a 3D solid are not allowed any rotational freedoms, they are restricted to translational movement. The downside with using 3D solid elements is that they require heavy processing power since no simplifications are made. Of course it can be regulated with the number and size of elements, but the accuracy of the solution might suffer with too few nodes (Baguley, Hose, 1997, 31).
Table of contents :
1.1 Background to the report
1.2 The problem
1.3 Purpose and goal
1.5.2 The strain test
2.1 ABB Robotics
2.3 Previous work
2.5 Development of the methods
3.1 One dimensional elements and mpc’s
3.1.1 RBE2 and RBE3
3.3 Linear elasticity
3.5 Calculations for beam geometry
3.6 Calculations for CGAP defined stiffness
3.7 Von Mises stress
4.1 Wrist model preparation
4.1.1 CAD and FE-model
4.1.2 Load sub-cases
4.2 Model A – Single point RBE2-connections
4.3 Model B – Single point RBE3-connections
4.4 Model C – Multi CGAP-spokes
4.5 Model D – Single CGAP-spokes
4.6 Model E – Single CBEAM-spokes
4.7 Model F – Inner CBEAM-mix
4.8 Model G – Outer CBEAM-mix
4.9 Model H – CGAP defined stiffness
4.10 Model X – RBE3 ring
4.11 Model Z – RBE2 rigid ring
5 Measure points
6 Results – Simulation and Experimental
6.1 Graphical results from the simulations
6.2 Solving time
7.1 Error ratio
7.2 Pattern error
7.3 Stress direction
8.1 Reliability of the results
8.2 The time consuming CGAP
8.3 Evaluation of the models
8.4 The failed models
10 Suggestions for continued work
A. Parameters of the Models