Turbine Engine

Simulating 3D Crack Growth In Turbine Engine Components

ANSYS and FRANC3D/NG simulate 3D crack growth in turbine engine components. 

By Bruce J. Carter, Paul Wawrzynek and A.R. Ingraffea, Fracture Analysis Consultants, Inc., Reji John and Pat Golden, Air Force Research Laboratory, Materials and Manufacturing Directorate, AFRL/RXLM, Wright-Patterson AFB, OH Ken Barlow, NAVAIR, Propulsion & Power Engineering, Patuxent River, MD

Jet engine turbine components are designed to operate under thermal and mechanical load cycles. Fatigue crack initiation and subsequent crack growth can occur, limiting the life of the part and imposing maintenance inspections and repairs or replacement. Finite element analyses are a fundamental aspect of the initial design process as well as for post-failure analyses. Engine components are geometrically complex and the finite element analyses can be very complex, involving fluid flow, heat transfer, rotation and vibrations, and contact between parts.

A Pratt and Whitney turbofan engine is tested at Robins Air Force Base, Georgia, USA.

U.S. Air Force photo by Sue Sapp. http://www.af.mil/photos/index.asp?page=35

Pratt & Whitney has been using ANSYS for engine thermo-elastic and dynamic structural analyses for several years, and thus has a high level of ANSYS proficiency within its engineering workforce. Damage tolerance is a significant aspect of engine design and field management, often requiring full 3D crack growth simulation.

Fracture Analysis Consultants (FAC) has been working with Pratt & Whitney, the US Air Force and the US Navy to develop software that works with ANSYS to simulate arbitrary, discrete, 3D crack growth in these turbine engine components. FRANC3D/NG (Next Generation) is independent software, but relies heavily on ANSYS finite element capabilities. FRANC3D/NG is used to insert and grow cracks in the ANSYS finite element mesh. ANSYS performs the finite element analysis and feeds the displacements, temperatures, and crack surface pressures back to FRANC3D/NG, where fracture parameters are computed and cracks are propagated.

An uncracked ANSYS finite element mesh (usually just a small portion of the full ANSYS model) is the starting point for FRANC3D/NG. FRANC3D/NG inserts a crack, remeshes (or uses ANSYS to remesh) the volume using a combination of singular-wedge, brick, pyramid and tetrahedral elements, and then writes the ‘cracked’ finite element mesh to a new ANSYS file along with ANSYS macros to analyze the model. The results from the ANSYS analysis are read into FRANC3D/NG where stress intensity factors are computed and crack growth is simulated by extending the crack geometry and remeshing once again.

For example, Figure 1 shows a test article for an elevated temperature, dwell-fatigue, spin test. It is a powder metallurgy IN100, subscale forging minidisk. It was designed to produce stress states similar to those experienced by actual turbine engine disks during service. EDM notches were created to act as crack starters in a number of locations on the disk surface. One location in particular, called a ‘rim’ crack, is highlighted in Figure 2.

Figure 1. The minidisk test article.

Figure 2. EDM notched crack locations evaluated in the slot of the minidisk; the ‘rim’ crack at 150° indicated here2.

10,000 pre-crack cycles, conducted at room temperature between 12,500 and 26,000 rpm, were applied to activate cracks from the tips of the EDM notches. The temperature was approximately 621°C at the bore and 657°C at the base of the elliptical slot, where the ‘rim’ cracks were located. The heated crack growth portion of the test was conducted by cycling between 12,500 and 26,000 rpm, and included a 60-second dwell at 26,000 rpm. The test was terminated after 1200 cycles.

An uncracked ANSYS finite element model of the minidisk is analyzed to determine the initial stresses and to provide the base model for subsequent crack growth simulations. The maximum stresses occur at maximum rpm and temperature (Figure 3).

Figure 3. ANSYS model of the minidisk showing the maximum principal stress contours.

A small portion of the ANSYS model (Figure 4) is extracted from the full model and written to an ASCII .cdb file. This small portion includes enough material volume around the ‘rim’ crack in the slot to allow significant crack growth. The file is read into FRANC3D/NG; element facets on cut-surfaces are retained to ensure node and element compatibility when the remeshed cracked portion of the model is merged with the unmodified portion. FRANC3D/NG is used to insert an initial crack that matches the EDM notch at the ‘rim’ location and then ANSYS or FRANC3D/NG can be used to remesh the volume.

Figure 4. A small portion of the minidisk ANSYS mesh is extracted from ANSYS and then read into FRANC3D/NG; the facets on the cut surface are retained.

The crack front mesh includes singular-wedge elements, surrounded by rows of brick elements; pyramid elements attached to the brick elements allow for a transition to tetrahedral elements in the rest of the model (Figure 5). Once the initial crack is inserted, automated crack growth can be scripted using the FRANC3D/NG user interface to simulate increments of crack extension or cycles of loading. FRANC3D/NG writes an ANSYS .cdb file along with ANSYS macros that combine the cracked portion of the model with the rest of the model, run the analysis, and write displacements and temperatures. FRANC3D/NG automatically reads the results, computes stress intensity factors, grows the crack and remeshes, and then starts the next ANSYS analysis. For this model, the crack growth simulation relies on the ANSYS capabilities for modeling thermal gradients and rotations. The crack is propagated for 50 steps and the crack growth resembles that seen in the test article (Figures 6 and 7).

Figure 5. Deformed shape of initial 0.01mm radius crack showing element types used to mesh around the crack front and crack surface; displacement magnification factor is 5.

Figure 6. ANSYS maximum stress contours and deformed shape for crack step 40.

Figure 7. The crack surface: a) in FRANC3D/NG with crack fronts overlaid onto the surface and b) from the test article2.

Only low-cycle fatigue is modeled in this study. An ANSYS modal analysis would provide vibratory stresses that could also be incorporated into the FRANC3D/NG crack growth simulation. In a typical blade/disk assembly, blades are inserted into the slots. In service, there is contact between the blades and the disk, and ANSYS can be used to model this contact. Crack nucleation and growth often occurs near or within the edge-of-contact region along the slots (Figure 8). FRANC3D/NG has been designed to work with these types of ANSYS analysis capabilities to capture realistic crack growth in such components.

Figure 8. FRANC3D/NG and ANSYS simulated crack growth in a blade; a crack initiates near the edge-of-contact between the blade and disk. The deformed crack is shown at 10x magnification. Blade/disk model courtesy of NAVAIR.

Acknowledgments

This work was partially supported by:

Air Force Contract No. FA8650-07-C-5216, “Three-Dimensional Nonlinear Structural Analysis Methods for Gas Turbine Engine Metallic Components and Component Assemblies,” with Dr. Patrick J. Golden, AFRL/RXLMN, Project Monitor.

Navy Contract No. N68335-08-C-0011, “Fretting Fatigue Modeling and Life Prediction” , with Mr. Ken Barlow, NAVAIR, Project Monitor.

Distribution Statement A – Approved for public release; distribution is unlimited, as submitted under NAVAIR Public release Authority 09-1310

Simulating 3D Crack Growth In Turbine Engine Components

ANSYS and FRANC3D/NG simulate 3D crack growth in turbine engine components. 

By Bruce J. Carter, Paul Wawrzynek and A.R. Ingraffea, Fracture Analysis Consultants, Inc., Reji John and Pat Golden, Air Force Research Laboratory, Materials and Manufacturing Directorate, AFRL/RXLM, Wright-Patterson AFB, OH Ken Barlow, NAVAIR, Propulsion & Power Engineering, Patuxent River, MD

Jet engine turbine components are designed to operate under thermal and mechanical load cycles. Fatigue crack initiation and subsequent crack growth can occur, limiting the life of the part and imposing maintenance inspections and repairs or replacement. Finite element analyses are a fundamental aspect of the initial design process as well as for post-failure analyses. Engine components are geometrically complex and the finite element analyses can be very complex, involving fluid flow, heat transfer, rotation and vibrations, and contact between parts.

A Pratt and Whitney turbofan engine is tested at Robins Air Force Base, Georgia, USA.

U.S. Air Force photo by Sue Sapp. http://www.af.mil/photos/index.asp?page=35

Pratt & Whitney has been using ANSYS for engine thermo-elastic and dynamic structural analyses for several years, and thus has a high level of ANSYS proficiency within its engineering workforce. Damage tolerance is a significant aspect of engine design and field management, often requiring full 3D crack growth simulation.   Fracture Analysis Consultants (FAC) has been working with Pratt & Whitney, the US Air Force and the US Navy to develop software that works with ANSYS to simulate arbitrary, discrete, 3D crack growth in these turbine engine components. FRANC3D/NG (Next Generation) is independent software, but relies heavily on ANSYS finite element capabilities. FRANC3D/NG is used to insert and grow cracks in the ANSYS finite element mesh. ANSYS performs the finite element analysis and feeds the displacements, temperatures, and crack surface pressures back to FRANC3D/NG, where fracture parameters are computed and cracks are propagated.   An uncracked ANSYS finite element mesh (usually just a small portion of the full ANSYS model) is the starting point for FRANC3D/NG. FRANC3D/NG inserts a crack, remeshes (or uses ANSYS to remesh) the volume using a combination of singular-wedge, brick, pyramid and tetrahedral elements, and then writes the ‘cracked’ finite element mesh to a new ANSYS file along with ANSYS macros to analyze the model. The results from the ANSYS analysis are read into FRANC3D/NG where stress intensity factors are computed and crack growth is simulated by extending the crack geometry and remeshing once again.   For example, Figure 1 shows a test article for an elevated temperature, dwell-fatigue, spin test. It is a powder metallurgy IN100, subscale forging minidisk. It was designed to produce stress states similar to those experienced by actual turbine engine disks during service. EDM notches were created to act as crack starters in a number of locations on the disk surface. One location in particular, called a ‘rim’ crack, is highlighted in Figure 2.

Figure 1. The minidisk test article.

Figure 2. EDM notched crack locations evaluated in the slot of the minidisk; the ‘rim’ crack at 150° indicated here2.

10,000 pre-crack cycles, conducted at room temperature between 12,500 and 26,000 rpm, were applied to activate cracks from the tips of the EDM notches. The temperature was approximately 621°C at the bore and 657°C at the base of the elliptical slot, where the ‘rim’ cracks were located. The heated crack growth portion of the test was conducted by cycling between 12,500 and 26,000 rpm, and included a 60-second dwell at 26,000 rpm. The test was terminated after 1200 cycles.   An uncracked ANSYS finite element model of the minidisk is analyzed to determine the initial stresses and to provide the base model for subsequent crack growth simulations. The maximum stresses occur at maximum rpm and temperature (Figure 3).

Figure 3. ANSYS model of the minidisk showing the maximum principal stress contours.

A small portion of the ANSYS model (Figure 4) is extracted from the full model and written to an ASCII .cdb file. This small portion includes enough material volume around the ‘rim’ crack in the slot to allow significant crack growth. The file is read into FRANC3D/NG; element facets on cut-surfaces are retained to ensure node and element compatibility when the remeshed cracked portion of the model is merged with the unmodified portion. FRANC3D/NG is used to insert an initial crack that matches the EDM notch at the ‘rim’ location and then ANSYS or FRANC3D/NG can be used to remesh the volume.

Figure 4. A small portion of the minidisk ANSYS mesh is extracted from ANSYS and then read into FRANC3D/NG; the facets on the cut surface are retained.

The crack front mesh includes singular-wedge elements, surrounded by rows of brick elements; pyramid elements attached to the brick elements allow for a transition to tetrahedral elements in the rest of the model (Figure 5). Once the initial crack is inserted, automated crack growth can be scripted using the FRANC3D/NG user interface to simulate increments of crack extension or cycles of loading. FRANC3D/NG writes an ANSYS .cdb file along with ANSYS macros that combine the cracked portion of the model with the rest of the model, run the analysis, and write displacements and temperatures. FRANC3D/NG automatically reads the results, computes stress intensity factors, grows the crack and remeshes, and then starts the next ANSYS analysis. For this model, the crack growth simulation relies on the ANSYS capabilities for modeling thermal gradients and rotations. The crack is propagated for 50 steps and the crack growth resembles that seen in the test article (Figures 6 and 7).

Figure 5. Deformed shape of initial 0.01mm radius crack showing element types used to mesh around the crack front and crack surface; displacement magnification factor is 5.

Figure 6. ANSYS maximum stress contours and deformed shape for crack step 40.

Figure 7. The crack surface: a) in FRANC3D/NG with crack fronts overlaid onto the surface and b) from the test article2.

Only low-cycle fatigue is modeled in this study. An ANSYS modal analysis would provide vibratory stresses that could also be incorporated into the FRANC3D/NG crack growth simulation. In a typical blade/disk assembly, blades are inserted into the slots. In service, there is contact between the blades and the disk, and ANSYS can be used to model this contact. Crack nucleation and growth often occurs near or within the edge-of-contact region along the slots (Figure 8). FRANC3D/NG has been designed to work with these types of ANSYS analysis capabilities to capture realistic crack growth in such components.

Figure 8. FRANC3D/NG and ANSYS simulated crack growth in a blade; a crack initiates near the edge-of-contact between the blade and disk. The deformed crack is shown at 10x magnification. Blade/disk model courtesy of NAVAIR.

Acknowledgments   This work was partially supported by:   Air Force Contract No. FA8650-07-C-5216, “Three-Dimensional Nonlinear Structural Analysis Methods for Gas Turbine Engine Metallic Components and Component Assemblies,” with Dr. Patrick J. Golden, AFRL/RXLMN, Project Monitor.   Navy Contract No. N68335-08-C-0011, “Fretting Fatigue Modeling and Life Prediction” , with Mr. Ken Barlow, NAVAIR, Project Monitor.

Distribution Statement A – Approved for public release; distribution is unlimited, as submitted under NAVAIR Public release Authority 09-1310

文章分类 应用案例