Karayel İnsansız Hava Aracının Statik Ve Dinamik Analizleri

Abstract

Tezde öncelikle insansız hava araçlarının 2. Dünya Savaşı’dan günümüze kadar olan dönemdeki gelişimi, kulanıldığı alanlar ve insansız hava araçları örnekleri gibi bilgileri içeren kısa tarihçesi anlatılmıştır. Sonraki bölümlerde ise Vestel Savunma Sanayii’nin(VSS) geliştirmekte olduğu Karayel adlı insansız hava aracının; tanıtımı, sonlu elemanlar modelinin oluşturulması, yükleme ve sınır koşullarının uygulanması, statik ve dinamik analizlerinin yapılışı ve elde edilen sonuçları açıklanmıştır. Karayel’in sonlu elemanlar modeli oluşturulurken kullanılan programlar MSC Nastran/Patran 2010’dur. Aracın sonlu elemanlar modeli oluşturulurken bazı hususlara dikkat edilmiştir. SEM’ni oluşturan elemanların çoğunluğu 2 boyutlu dörtgen elemanlardır. Oluşturulan dörtgen elemanlar, 4 adet kıstasa göre oluşturulmuştur. Bunlar; açıklık oranı(aspect ratio), eleman çarpılması(element warping), yamukluk(skew), sivrilme(taper)’dir. Analiz sürelerini kısaltmak için ise rib’lerin ve frame’lerin flanş’ları bir boyutlu beam eleman olarak modellenmiştir. Ayrıca aracın yapısal olarak dayanımı olmayan parçaları ise sıfır boyutlu kütle elemanlar olarak modellenmiştir. Araçta metalik ve kompozit malzemeler kullanılmıştır. Ancak sınai mülkiyet haklarından ötürü malzeme özellikleri ve katman bilgileri paylaşılmayacaktır. Bu tezde, Karayel aracının yükleme koşullarından 2 tane farklı kritik koşul ele alınmıştır. Her koşul için uygulanacak olan basınç yükleri, Vestel Savunma Sanayii tarafından hesaplanmış, hesaplanan basınç yükleri sonlu eleman modelindeki ilgili elmanlar ile ilişkilendirilmiştir. SEM oluşturulduktan sonra modelin düzgün çalıştığını kontrol edebilmek için birtakım test analizleri yapılmıştır. Yapılan test analizlerinden model başarıyla geçmiştir. Test analizlerinden sonra ilk olarak aracın modal analizi yapılmıştır. Yapılan modal analiz sonucunda aracın normal modlarının olduğu frekanslar ile araçtaki titreşim kaynağı olan yapıların frekanslarının farklı olduğu görülmüştür. Bu sayede araçta rezonans olmayacağı anlaşılmıştır. Daha sonra aracın statik analizleri yapılmıştır. Yapılan statik analiz sonucunda elde edilen gerilme değerleri, ilgili izotropik malzemelerin dayanım değerleri ile karşılaştırılmıştır. Karşılaştırma sonucunda izotropik malzemeden yapılan yapılarda herhangi bir göçmenin (failure) olmayacağı anlaşılmıştır. Ancak aracın büyük bir bölümü kompozit yapıdır ve kompozit malzemenin dayanımlarının doğrudan gerilmeler ile karşılaştırılması yanlış değerlendirmelere yol açabilmektedir. Bu nedenle kompozit için yapılar beş ayrı göçme kriterine göre analiz edilerek tasarlanmıştır. Hesaplar Python 4.3.4’da yazılan kod vasıtasıyla yapılmıştır. Bu kod her bir kompozit eleman için beş ayrı göçme kriterini uygulayarak rezerv faktörünü (RF) hesaplamakta ve sonuçları “csv” dosyası olarak listelemektedir. Yapılan RF hesapları sonucunda aracın herhangi bir kompozit yapısında göçme olmadığı görülmüştür. Aracın kanadı VSS tarafından üretilmiş ve deplasman testi yapılmıştır. Yapılan testin yüklemesi Karayel sonlu elemanlar modelinde de uygulanmış ve elde edilen sonuçlar test ölçümleriyle karşılaştırılmıştır. Yapılan karşılaştırmalara göre test ve analiz değerlerinin oldukça yakın korelasyon gösterdiği görülmüştür. Yapılan tüm bu analiz ve testler sonucunda Karayel taktik insansız hava aracı karşılacağı yüklemeler karşısında herhangi bir göçmeye uğramayacağı görülmüştür. Ayrıca testler ile analiz sonuçlarının birbirlerine yakınlığı da aracın sonlu elemanlar modelinin düzgün çalıştığının ve sonlu elemanlar modeli oluşturulurken uyulan kriterlerin doğru olduğunun göstergesidir.

First usage of unmanned aerial vehicles(UAV) is in 19th century. However first UAVs were single use only and they could not be controlled. They were used for only carry a bomb in military but their efficiency were poor. In II.World War Germans built V-1 which were effective bomber as unmanned aerial vehicle and this vehicles caused death of lots of people. By time people started to use UAVs for different missions. For example ABD developed an UAV named SAU-1 to shoot down V-1 unmanned bombers. UAVs used not only for attack but also used for spying. Q-2C(Firebee) was one of them which used for spying. That UAV has a jet engine and Q-2C was half-stealth UAV and these specialities make Q-2C successful aircraft. Like Firebee some of UAVs used for fake target. In 1960 Russia shoot down U-2 which is a manned spy plane, and get pilot of the plane alive. Since Russia have the pilot alive they could learn valuable information and they have a advantageous position because they had a hostage. This event has shown that UAVs are better vehicles especially for spying missions. Because of success of UAVs in battles and spying missions, countries give importance to develop UAVs. As result of developments, in these days UAVs can be used in reconnaissance & surveillance, targetting for fighters and rockets, finding person and destroying if it is needed, being fake targets for anti-aircraft systems, training air defence systems. Although Turkish first manned plane was builded in 1925 by Vecihi Hürkuş, Turkey falled behind in developing planes. In 1994 Turkey bought first UAVs named GNAT-750 from Israel. However these vehicles can not be used effectively. Turkey was aware of importance of unmanned aerial vehicles, so some domestic UAV projects were being supported by Turkish goverment. Most advanced one of these projects is ANKA is being developed TAI(Turkish Aerospace Industries). ANKA is a MALE(Medium altitude long endurance) UAV. The second one is KARAYEL which is being devoloped by VDI(Vestel Defance Industry). KARAYEL is a tactical unmanned aerial vehicle. In this study preparing of Finite Element Model(FEM) and structural analyses of KARAYEL unmanned aerial vehicle is presented. Finite Element Method(FEM) is a method that divides the structure into smaller parts and minimize the problem in these parts which is called elements. And by using numerical calculations, solution of whole structure is found. In finite element model the smaller parts are called elements, element boundaries are determined by using points called nodes. Nodes and elements creates a system named mesh. There are different kind of elements. 0D elements are named point elements, 1D elements are called bar elements, 2D elements are called shell elements, 3D elements are called solid elements. In Karayel FEM; skins, ribs, bulkheads of vehicle is modelled by shell elements. Two types of shell elements which are tria and quad, are used in the model. Since most of KARAYEL finite element model is consist mainly of quad elements, some criterias of quad elements were also explained. The criterias are taper, aspect ratio, warp and skew. Quad elements of KARAYEL finite element model have been prepared according to these criterias. Except quad elements, different kind of elements were used as well. For example, instead of unstructural parts point elements were used modeling mases of the parts, to decrease model preparation and analysis run time, flanges of ribs and bulkheads were modelled by bar elements. As connectors; MPCs(Multi Point Constraints) and fasteners were used. Most of the vehicle is consist of composite materials. Since material properties and layup is commercially confidential information they are not presented in this thesis. After finite element model had been prepared, some check runs were done to see that the model was running correct and ready for analyses. One of the check runs is static check run. The other one is dynamic check run. Static check run consists of two step. First one is unit displacement check run. For unit displacement check run, only one node of the model is displaced at one direction and analysis is run, then this proces is repeated for other directions. As a result of analyses it is aspected that whole model moves together and all stress values are zero. As a result of the unit displacement check run whole model moved together and all stress values were zero as aspected. Second step of static check runs is gravity check run. For this step, one “g” gravity load is identified and model is fixed from five nodes. These nodes are chosen from landing gear fastening areas. Model is fixed because for static analyses there must be boundary conditions that prevent singularty otherwise the run will end up with an error. However if inertia relief metod is used, there is no need for boundary condition. As a result of gravity check, all displacements must be logical and “OLOAD” results must match with reaction forces of nodes that fixed for the analysis. After gravity check analysis for the model, all displacements were logical and “OLOAD” results matched with reaction forces at fixed nodes. For dynamic check run, modal analysis of the model is run. There is no need for load in modal analysis and since in-flight normal mods are needed, any boundary condition is not defined to the model. As a result of modal analysis, there must be six rigid modes, sixth of rigid modes must has been a frequency value that smaller than 0.01, ratio of first elastic mod (seventh mod) to sixth mod must be bigger than 10000. After modal analysis check run, it is seen that all requirements are satisfied. Overall check runs are shown that model is ready for structural analyses. Flight loads were calculated for several load cases by VDI. For this thesis the most critical two load cases have been selected and results of them are presented. These load cases are max nz and minimum nz load cases, which cover majority of the minimum RFs(Reserve Factor) in the whole structure. First of all modal analysis was made to find out frequencies of the normal modes of the vehicle. These frequencies are importand because if a vibration source’s frequency and a normal mode’s frequency are the same, resonance will be happen. As a result of resonance structure of the vehicle fails. However modal analysis has shown that there are no such a situation and structure was not going to be failed. Frequency values of normal mods is not shared in this thesis since analysis results are commercially confidential information. Second analysis was static analysis. As mentioned before there are two load case for this thesis, thus static analysis is repeated for two load cases. Analysis is done for in-flight situations, that is why inertia relief method is used for static analyses and there is no fixed node. As output of static analyses; displacement, stress and element force values were taken. However since the values commercially confidential information all static analyses results is shown after all values have been gotten dimensionless. Displacement results were as aspected by taking into consideration direction of ‘g’ acceleration. For positive ‘g’ maximum displacement was accured at tip of wings, for negative ‘g’ maximum displacement was accured at elevator. For other components of vehicle there is no big deformation and all deformations were acceptable. Applied stresses obtained from static analysis are compared with ultimate strength of metallic materials. For both load cases stress values were under material strengths. Thus for structures which have isotropic materials is in safe zone and will not fail. For composite materials stress values should not compare directly with material strengths. Especially for sandvich composites there are different types of failure criterias. In this study calculations of some failure criterias for composite shells were shared. This criteria are dimpling, face wrinkling, shear crimping, core shear for sandvich shells and for carbon plies unnotched strength. A python 3.4.3 code was written. The code takes metarial properties and composite ply informations from “bdf” file which is MSC Nastran input file, then takes element forces of composite elements from “f06” file which is an output file of MSC Nastran, that is why element forces must be requested before analysis in “bdf” file. As final input, the code requests from user to enter strength values of metarials is used in composites. After getting all information, the code applies all these failure criterias to all composite elements of Karayel finite element madel and calculates RFs(Reserve Factor) for all the criterias are mentioned before. Results were listed in csv file which can be easily imported in Msc Patran 2010 by the code. RF calculations is repeated for two load load cases and results were shown that all composite elements have enough strength for applied forces. VDI has conducted full scale static test on a test wing. Test and analysis results match quite well. No structural failure has been observed until ultimate loading. Consequently, all tests and analyses are shown that Karayel tactical unmanned aerial vehicle can survive without any failure against estimated forces during life time. Similarity of test results and static analyses results are also shown that estimations and criteria have been done during create finite element model of Karayel were true and the model works fine.