INDUSTRY SIMULATION

WELDING SIMULATION AT THE DEVELOPMENT OF EXHAUST SYSTEMS In the production of exhaust systems, welding is one of the most used joining processes. The distinctive hot crack inclination of the usually used nickel alloyed materials poses during this a special challenge. The article of J. Eberspächer describes a numerical method for the welding simulation, with which, amongst others, the hot crack inclination of welded components can be tested. With the aid of this method that is based on the finite element method, the relation between component geometry and hot crack initiation could be demonstrated, whereby component designs can be optimised in this aspect.

24

AUTHORS

M. ENG. (IWE) PHILIPP ZEWE

is FE-Analyst in the Basic Development Department for Exhaust Systems at J. Eberspächer GmbH & Co. KG in Esslingen (Germany).

DR.-ING. RALF RIEKERS

is responsible for Computation of Durability Methods and Project Manager in the Basic Development Department for Exhaust Systems at J. Eberspächer GmbH & Co. KG in Esslingen (Germany).

DR.-ING. MING DONG

is Team Leader in the Basic Development Department for Exhaust Systems and is responsible for Method Development in the area of Durability of Exhaust Systems at J. Eberspacher GmbH & Co. KG in Esslingen (Germany).

INITIAL SITUATION

The simulation of welding processes for the calculation of distortions and residual stresses due to welding is already used more often in the industrial practice today. Also the evaluation of other quality factors when welding, as the inclination to hot crack and cold crack initiation, is occasionally performed by the use of numerical processes, but is limited mostly to easy component geometries due to very high calculating times. Particularly with austenitic CrNi-steels, the special metallurgical hot crack sensitivity can lead to an increased failure rate when welding, which are used in the area of the exhaust technology for manifolds, catalysts and mufflers. The increasing thermic and corrosive loads of exhaust systems make the use of this heat resisting nickel alloyed steels however often indispensable. A hot crack which was initiated during production displays a “pre-damage” which represents a potential risk for the operating status. In this case there is a risk of a critical crack increase and therefore a breakdown of the complete system during use especially by the high dynamic load of an exhaust system. Therefore it has to be ensured, that in the best case hot cracks can be avoided or that they will be recognized in line with the process control and if necessary be repaired. The control and rework however is an additional expenditure of time and produces increased costs in the production area. With the aid of the newly initiated and here used numerical method, the influence of the component geometry of a muffler on the hot crack initiation was analysed and moreover a design without hot crack inclination developed. By means of the new design the initiation of cracks could be prevent-

 Cross-section polish of the girth weld with liquation crack 09I2010

Volume 71

ed, independently of material and process parameters. Using the finite element method for the hot crack evaluation, it is now possible to indicate early the potentially hot crack endangered component geometries and to improve them in this aspect that means already in the predevelopment, before the first prototypes are available. HOT CRACKS – INITIATION MECHANISM

Hot cracks initiate during welding, directly in the weld pool or in a nearby area of the weld pool. The initiation of hot cracks is generally formed by combination of different factors, whose influence and specification shows situational differences. In principal it can be differentiated between metallurgic, process-related and structuremechanical formation mechanism. Under metallurgic aspects, the austenitic CrNi-steels are e.g. considered specially sensitive for hot cracks. Reasons for that is the initiation of low melting eutectic phases during the solidification, as well as the combination of low heat conductivity with concurrent high thermal strain, which leads altogether to an increased shrinking when welding [1]. From the process, the hot crack initiation will be affected, among other things, by the interrelationship of welding speed and weld pool geometry respectively crystallization front, as e.g. a distinctive liquation concentration in the seam center favours the initiation of seam center cracks clearly. Furthermore has the structure mechanic behaviour of the welded component decisive influence on the initiation of hot cracks. For each hot crack sensitive steel, a critical high temperature interval is existent in dependency of different influencing factors; named in the following: brittle temperature inteval (BTR) [2]. The material will run through it after welding until it reaches complete solidification. Already little strains will be beared in this temperature interval by the initiation of a crack. During the BTR, the weld material is present in a multiphase area of solid and liquid phase, whereat the contingent of liquid phase is already reduced, that an initiated crack cannot be “closed” again by the molten mass. Decisive for the initiation of a hot crack is therefore the exceeding of a maximum permitted strain value within the critical temperature interval. Limit value and BTR

25

INDUSTRY SIMULATION

 Calculated temperature distribution in the range of the heat source [°C]

are therefore again dependent of the material as well as of different process parameters. Consequently, the initiation of hot cracks is based on the interaction between material, process and structure mechanic component behaviour and therefore displays a classical thermo mechanic problem. SIMULATION

The calculative evaluation of the hot crack behaviour of the tested components was performed with a structural welding simulation under the use of the FEM-software Abaqus. The finite element simulation is a transient decoupled thermo mechanic analysis, during the nonlinear component deformations as well as the contact conditions between all joining partners were considered. Specially adjusted material properties were set up for the welding filler material, which should not be active at the beginning of the simulation. For the reduction of the simulation expense, the analyzed components were meshed in a special way. In the proximate environment of the heat source, in which locally very high gradients are present, e. g. of the temperature, stress and strain, it is modelled with relatively fine volume elements. With the increasing distance from the heat source, a rougher discretisation can be chosen from shell elements. It is necessary to consider the relevant thermo physical and thermo mechanic material parameters from room until melting temperature as the base material as well as the welding material will be warmed up to liquidus temperature when welding. Material values up to 1000 °C were present for the tested material. An extrapolation of the statistical values in the area of the liquidus temperature was performed additionally. Furthermore it is to

26

be considered, that the thermal strains will take place in a very short time due to the high heating and cooling rates of more than 1000 °C/s during welding. Tests for this purpose have shown that the strainrate dependent behaviour is to be considered at least in the area of the weld seam and the heat affected zone. The strain-rate dependency was represented for this purpose by a viscoplastic simulation model with temperature dependent coefficients D and q, Eq. 1. EQ. 1

T = T0

. F + 1 + __ D

[

( )]

of a separately performed process simulation. For this reason, only the structure mechanic influencing factors of the hot crack initiation can be considered with the described process. The influence of material and process on the crack building can only be considered indirectly by an adaption of strain limit values and temperature intervals of brittleness. A maximum permitted strain Fcrit, as well as the top and lower limit temperature of the temperature interval of brittleness (TBTR,min, TBTR,max) have to be set for the represented welding situation in the finite element analysis prior to the hot crack evaluation. A critical time interval [tcrit,min; tcrit,max] can be defined on the base of the temperature interval of brittleness for the area of the weld seam and the heat affected zone. The temperature interval of brittleness and the critical time interval are connected with each other over the cooling conditions of the particular welding situation according to the equation, Eq. 2 and Eq. 3. EQ. 2

TBTR(tcrit,max) = TBTR,max

EQ. 3

TBTR(tcrit,min) = TBTR,min

1_ q

The base for the numerical hot crack evaluation forms a structural welding simulation of the relevant crack prone weld seams. This simulation type provides by definition therefore only results, which are based on the structure respectively thermo mechanic behaviour of the welded components. The fluid flow within the weld pool will not be considered in this case. They would be part

Within the critical time interval, the transient progress of the plastic strain Fplast will be determined and compared with the set limit value. The numerical hot crack criteria which is applied during of the structural welding simulation is now based on the correlation between the exceeding of the permitted

 Basic variant; plastic strain progression in the critical time interval

 Von Mises equivalent stress on deformed model (scale factor ten) [MPa]

strain value and the initiation of a hot crack at the same position. SIMULATION OF A FRONT MUFFLER

Hot cracks appeared in the circumferential welds between shell and outer baffles during weld tests at a prototype muffler. The cracking could not be counteracted by the variation of different base material and filler material combinations as well as by the optimization of the welding parameters. However, with the aid of the simulation it could be demonstrated, that a direct relation is present between the hot crack initiation and the transient structure mechanic behaviour during the welding process. In addition it could be shown by the simulated comparison of different design variants, that the structural hot crack inclination can be influenced by the specific modification of the component geometry.

Identical welding parameters were used for all components in the structural welding simulation: : process: MAG : voltage: 16.0 V : amperage: 180 A : welding speed: 24 mm/s : base material: 1.4828 : welding filler material: 1.4829. The finite element models were specially meshed for the hot crack evaluation in the area of the analysed circumferential welds and are composed of approximately 50,000 elements. The calculating time for the heat conduction simulation and the thermo mechanic analysis amounted to several hours. The hot cracks at the base variant have its origin in the inner side of the inserted outer baffles. The hot cracks were initiated in the heat affected zone, which spread in the longitudinal direction of the

 Optimised design; Plastic strain progression in the critical time interval

circumferential welds and partly grew into the last solidified weld material, . The detailed evaluation of the finite element simulation is limited to the hot crack prone area at the inner side of the baffle, . The plastic strains were determined for all component variants within the temperature area above TBTR,min. The maximum occurred strain value served for every variant as a qualitative evaluation criteria of the different designs. The determined strain progress for the evaluated area at the inner side of the outer baffle is represented for the base variant in . The occurred peak within the time interval is lying above the assumed limit value. Cause of this overcritical strain in the heat affected zone for the high temperature area is the strong deformation by the bending of the baffle rim during the welding process, . By the means of a modification of the muffler design, this deformation and therefore the occurred plastic strains in the critical time could be counteracted, . On the basis of the used numerical criteria, a considerable reduction of the structure mechanic hot crack inclination for the optimised component geometry is assumed. The result of the finite element simulations was confirmed by welding tests at comparable muffler variants. No hot cracks have occurred when using the adjusted geometry. SUMMARY

In the course of a structural welding simulation, the relation of component geometry and structural hot crack inclination on a complex component of an exhaust system could be demonstrated. By using this method, the hot crack inclination of a component can be shown and the optimising potential of different design variants be evaluated already at an earlier time in the initiation phase. The successful application of the method on the product was confirmed by welding tests. REFERENCES

[1] Tösch, J.; Schabereiter, H.; Pereneder, E.; Rabensteiner, G.: Bedeutung und praktische Beeinflussbarkeit des Ferritgehaltes bei der Schweißung austenitischer Stähle. In: Schweiß- & Prüftechnik 2/97 (1997), S. 18-26 [2] Prokhorov, N. N.; Jakuschin, B.F.: Theorie und Verfahren zum Bestimmen der technologischen Festigkeit von Metallen während des Kristallisationsprozesses beim Schweißen. In: Schweißtechnik 18 (1968), S. 8-11

09I2010

Volume 71

27