Finite element modeling method for optical fiber cable

Abstract

The application discloses a finite element modeling method of an optical fiber cable, adopts an equivalent bar beam combined model, simulates the contact between optical fibers by using a compressible and inextensible bar element, processes the optical fibers as a composite cross-section beam element, simulates the tension of the optical fibers in the actual cable winding process according to the actual cable winding condition, models and solves layer by layer, and finally completes the modeling of the optical fiber cable. The method solves the problem that the existing optical fiber cable modeling method is prone to not converging in the solving of the contact element, and cannot analyze the stress and distribution of the multiple-turn optical fibers in the cable, greatly improves the simulation speed, can intuitively reflect the actual cable winding condition and calculate the internal stress, and further effectively improves the work efficiency in engineering.

Description

Technical Field

[0001] This invention belongs to the field of fiber optic guided missile technology, specifically relating to a finite element modeling method for fiber optic coils. Background Technology

[0002] Fiber optic coils are a crucial component of fiber optic guided missiles. A fiber optic guided missile consists of three parts: a launch guidance system, a fiber optic coil, and the missile itself. Fiber optic cables are wound onto a specially designed spool according to specific requirements, forming a fiber optic coil which is then fixed to the missile's tail section. The quality of the coil is critical to the missile's successful launch. Fiber optic winding is a key technical issue in fiber optic guidance, requiring a robust winding structure with minimal volume to facilitate successful cable deployment. Due to the limitations of missile size and volume, the winding volume should be as small as possible to maximize the winding density.

[0003] After optical fiber coils are wound, the complexity and multi-layered nature caused by the long winding distance often lead to uneven stress within the coil. Furthermore, the transmission performance of optical fibers is highly sensitive to stress; significant differences in stress between the inner and outer fiber layers result in substantial variations in signal transmission quality throughout the guided weapon's range, affecting its overall effectiveness. The low or even zero pressure exerted by the inner fiber layers on the core shaft and between layers further degrades the coil's stability. Under missile launch overload and fiber release tension, multiple layers or the entire coil may slip off the spool, causing fiber breakage, guidance signal interruption, and weapon malfunction. Current coil models are incomplete and cannot analyze the stress and distribution between multiple turns of fiber within the coil, making it difficult to predict its structural performance and potential impact on release.

[0004] In actual fiber optic packages, optical fibers exhibit mechanical behaviors such as contact, slippage, and friction between turns. However, directly using a contact model—for example, modeling the fiber using line elements and simulating the contact between line elements using CONTA176 and TARGE170—is prone to non-convergence. To improve the stability of fiber optic packages, a new modeling method for fiber optic packages is proposed. Summary of the Invention

[0005] The purpose of this invention is to provide a finite element modeling method for optical fiber coils, which solves the problems of existing optical fiber coil modeling methods where the solution of contact elements is prone to non-convergence and cannot analyze the stress and distribution between multiple turns of optical fibers inside the coil.

[0006] The technical solution adopted in this invention is as follows: a finite element modeling method for optical fiber coils, using an equivalent rod-beam combination model, using compressible but not tensile rod elements to simulate the contact between optical fibers, treating the optical fiber as a composite section beam element, simulating the tension applied to the optical fiber during the actual coil winding process according to the actual coil winding situation, modeling and solving layer by layer, and finally completing the modeling of the optical fiber coil.

[0007] The technical solution adopted in this invention is further characterized by:

[0008] The finite element modeling method for fiber optic bundles uses Ansys software to establish the fiber optic model in cylindrical coordinates. The radial direction of the bundle is r, the circumferential direction is θ, the symmetry axis direction is z, and the fiber winding follows the left-handed helix rule. The direction of the four fingers bending is the fiber winding direction, the direction of the thumb is the forward direction, the starting angle of the fiber is -40°, the helix direction is a left-handed helix, the standard section is -40° to -360°, and the cross-turn section is 0° to -40°.

[0009] The specific steps are as follows:

[0010] Step 1: Establish the core cylinder model and the first fiber layer model in cylindrical coordinates;

[0011] Step 2: Apply boundary conditions and prestress to the existing fiber layer model;

[0012] Step 3: Solve for the prestress in Step 2 to obtain the actual stress of the core cylinder and the existing fiber layer model;

[0013] Step 4: Update the model and read in the actual stress of the core and existing fiber layer models;

[0014] Step 5: Apply prestress to the current fiber layer model again and solve for and output the stress;

[0015] Step 6: Determine whether the current fiber layer model is the last fiber layer. If yes, output and process the data to complete the modeling. If no, proceed to step 7.

[0016] Step 7: Build the model for the next fiber layer, delete the initial prestress, and return to step 2;

[0017] Step 1: The core cylinder model includes the inner carbon fiber layer and the outer adjustment layer. It is divided into a central section and left and right side bosses. The specific construction method is as follows:

[0018] Modeling of the adjustment layer: The adjustment layer is modeled using solid185 solid elements;

[0019] Modeling of the middle part: The contact between the first layer of optical fiber and the bottom cylinder is established by using compressible but not tensile rod elements to create an equivalent contact model. The arrangement of nodes on the adjustment layer is consistent with the arrangement of nodes in the first layer of optical fiber.

[0020] Modeling the left and right side bosses: The bosses are higher than the middle part by half the diameter of the optical fiber, and are modeled using rod elements;

[0021] The carbon fiber layer is modeled using shell 181 elements. Its node arrangement is consistent with the bottom layer element arrangement of the adjustment layer. The element creation method for the carbon fiber layer is the same as that for the adjustment layer.

[0022] Contact modeling between carbon fiber layer and adjustment layer: There is a buckle between carbon fiber layer and adjustment layer. The contact at the buckle is modeled with beam elements, and the other contact positions are modeled with rod elements.

[0023] The specific method for establishing the fiber layer model in step 1 is as follows:

[0024] The optical fiber is divided into standard segment and cross-turn segment. The standard segment optical fiber is modeled using link180 element, and the cross-turn segment optical fiber is modeled using beam188 element.

[0025] The first standard segment node is generated, which is the center point of the fiber cross section. Then, the cross-turn curve is determined according to the interpolation function, and the curve is discretized into cross-turn nodes. The entire layer of fiber nodes is established in this way, and the fiber node layer is completely established.

[0026] Finally, the contacts between optical fibers and between optical fibers and the core tube are modeled to complete the establishment of the optical fiber layer model.

[0027] The specific steps for modeling the contact between optical fibers and between optical fibers and the core are as follows: The contact between optical fibers is divided into three types: contact between optical fibers in the same layer; contact between optical fibers in the upper layer and the lower layer; and contact between the first layer optical fiber and the conditioning layer. Linear elements are used to simulate the contact for all of these.

[0028] The contact unit modeling between the first-layer optical fiber and the conditioning layer is specifically divided into three types:

[0029] (1) The contact between the standard fiber segment and the middle part of the adjustment layer is achieved by using a rod element. The first standard fiber segment node of the established fiber is extracted, and the fiber radius is reduced along the r direction to obtain the bottom boundary node corresponding to the first standard fiber segment node on the core tube surface. Based on these nodes, the contact element model between the first standard fiber segment and the middle part of the core tube can be established.

[0030] (2) The contact between the cross-turn fiber and the middle part of the adjustment layer is made using beam elements; extract the first layer cross-turn fiber node of the established fiber, and reduce the fiber radius along the r direction to obtain the bottom boundary node corresponding to the first layer cross-turn fiber node on the core cylinder surface. Based on these nodes, the contact element model between the first layer cross-turn fiber and the middle part of the core cylinder can be established.

[0031] (3) The contact between the first layer of optical fiber and the left and right side protrusions of the adjustment layer are all rod units. Extract the node information of the standard arc segment of the first turn and the last turn of the first layer of the established optical fiber respectively, and translate these nodes to the left and right by half the optical fiber diameter respectively to form the left and right boundary nodes of the left side protrusion of the optical fiber bundle and the core tube. Based on these nodes, the contact rod units of the left and right side protrusions of the optical fiber bundle and the core tube can be established.

[0032] Contact modeling between optical fibers in the same layer involves connecting the optical fiber nodes at relative positions of two adjacent turns to form contact units of optical fibers in the same layer.

[0033] The modeling of contact units between optical fibers in the upper and lower layers is specifically divided into two types:

[0034] (1) The standard fiber segment adopts pole unit contact modeling, and connects the fiber nodes of each layer that have contact with the fiber of the next layer to form fiber contact units in the same layer.

[0035] (2) The cross-turn fiber is modeled using beam element contact. Based on the number of unwound turns of the coil, the cross-turn unwound curve between layers is connected to the nodes (excluding the starting point) that are related to the fiber before it to form a cross-turn beam element model. The number of unwound turns is determined according to the actual situation.

[0036] In step 2, the boundary conditions are applied by either applying full constraints on the left end, or applying symmetry plane constraints, including fixed constraints on the degrees of freedom of rotx, rotz, and uy, and also applying full constraints on the left end of the core cylinder.

[0037] The prestress is determined based on the tension of the optical fiber during the actual winding process, specifically calculated according to formula (1):

[0038]

[0039] Finally, the prestress was solved using Ansys software to obtain the actual stress of the core cylinder and the existing fiber layer model.

[0040] In step 4, the specific operation of updating the model is to modify the coordinates of the fiber layer nodes based on the displacement results in the current database file, which is implemented by the built-in function of the Ansys software.

[0041] The beneficial effects of this invention are:

[0042] The finite element modeling method for fiber optic coils in this invention utilizes an equivalent rod-beam combination modeling technique. This method employs compressible but not tensile rod elements to simulate the contact between optical fibers, treating the optical fibers as composite cross-section beam elements. Based on the actual coil winding situation, it simulates the tension applied to the optical fibers during the actual coil winding process. Modeling and solving are performed layer by layer to ultimately complete the modeling of the fiber optic coil. This method solves the problems of existing fiber optic coil modeling methods, such as the tendency for the solution of contact elements to fail to converge and the inability to analyze the stress and distribution between multiple turns of optical fibers within the coil. It significantly improves simulation speed, intuitively reflects the actual coil winding situation, and calculates its internal stress, thereby effectively improving work efficiency in engineering. Attached Figure Description

[0043] Figure 1 This is a flowchart illustrating the finite element modeling method for the optical fiber coil of the present invention.

[0044] Figure 2 This is a schematic diagram of a complete model of an optical fiber package constructed using the finite element modeling method in an embodiment of the present invention.

[0045] Figure 3 This is a schematic diagram of fiber optic modeling rules in an embodiment of the present invention;

[0046] Figure 4 This is a schematic diagram of the optical fiber unwinding method in an embodiment of the present invention;

[0047] Figure 5 This is a schematic diagram of the contact method of the optical fiber in an embodiment of the present invention;

[0048] Figure 6 This is a schematic diagram of the unwinding of the 2.5 turns at the right end of the coil in an embodiment of the present invention;

[0049] Figure 7 This is a schematic diagram of the unwinding of the 1.5 turns at the left end of the coil in an embodiment of the present invention;

[0050] Figure 8 This is a schematic diagram of the interlayer optical fiber contact method in an embodiment of the present invention;

[0051] Figure 9 This is a schematic diagram of the contact unit between the optical fiber and the left and right protrusions of the adjustment layer in an embodiment of the present invention;

[0052] Figure 10 This is a schematic diagram of the modeling method for the middle part in an embodiment of the present invention;

[0053] Figure 11 This is a schematic diagram of the carbon fiber layer modeling method in an embodiment of the present invention;

[0054] Figure 12 This is a schematic diagram of the modeling method for the connection unit between the carbon fiber layer and the polytetrafluoroethylene adjustment layer in an embodiment of the present invention;

[0055] Figure 13 This is a schematic diagram of the optical fiber structure in an embodiment of the present invention;

[0056] Figure 14 This is a schematic diagram of a key node on the 0° cross-section of the optical fiber coil in an embodiment of the present invention;

[0057] Figure 15 This is a schematic diagram of the cross-sectional lines of the beam-pole model obtained from the optical fiber sheath in an embodiment of the present invention;

[0058] Figure 16 This is a schematic diagram of the rotating model of the cross-sectional lines of the beam obtained by the optical fiber sheath in an embodiment of the present invention;

[0059] Figure 17 This is a schematic diagram of the connection relationship between the first layer fiber node and the second layer fiber node of the optical fiber sheath in an embodiment of the present invention; Detailed Implementation

[0060] The present invention will now be described in detail with reference to the accompanying drawings and embodiments.

[0061] like Figure 1 As shown, the finite element modeling method for optical fiber coils provided by this invention adopts an equivalent rod-beam combination model, uses compressible but not tensile rod elements to simulate the contact between optical fibers, treats the optical fiber as a composite section beam element, simulates the tension applied to the optical fiber during the actual coil winding process according to the actual coil winding situation, models and solves layer by layer, and finally completes the modeling of the optical fiber coil.

[0062] The finite element modeling method for fiber optic bundles uses Ansys software to establish the fiber optic model in cylindrical coordinates. The radial direction of the bundle is r, the circumferential direction is θ, the symmetry axis direction is z, and the fiber winding follows the left-handed helix rule. The direction of the four fingers bending is the fiber winding direction, the direction of the thumb is the forward direction, the starting angle of the fiber is -40°, the helix direction is a left-handed helix, the standard section is -40° to -360°, and the cross-turn section is 0° to -40°.

[0063] The specific steps are as follows:

[0064] Step 1: Establish the core cylinder model and the first fiber layer model in cylindrical coordinates;

[0065] The core cylinder model includes the inner carbon fiber layer and the outer adjustment layer. It is divided into a central part and left and right side bosses. The specific construction method is as follows:

[0066] Modeling of the adjustment layer: The adjustment layer is modeled using solid185 solid elements;

[0067] Modeling of the middle part: The contact between the first layer of optical fiber and the bottom cylinder is established by using compressible but not tensile rod elements to create an equivalent contact model. The arrangement of nodes on the adjustment layer is consistent with the arrangement of nodes in the first layer of optical fiber.

[0068] Modeling the left and right side bosses: The bosses are higher than the middle part by half the diameter of the optical fiber, and are modeled using rod elements;

[0069] The carbon fiber layer is modeled using shell 181 elements. Its node arrangement is consistent with the bottom layer element arrangement of the adjustment layer. The element creation method for the carbon fiber layer is the same as that for the adjustment layer.

[0070] Contact modeling between carbon fiber layer and adjustment layer: There is a buckle between carbon fiber layer and adjustment layer. The contact at the buckle is modeled with beam elements, and the other contact positions are modeled with rod elements.

[0071] The specific method for establishing the fiber optic layer model is as follows:

[0072] The optical fiber is divided into standard segment and cross-turn segment. The standard segment optical fiber is modeled using link180 element, and the cross-turn segment optical fiber is modeled using beam188 element.

[0073] The first standard segment node is generated, which is the center point of the fiber cross section. Then, the cross-turn curve is determined according to the interpolation function, and the curve is discretized into cross-turn nodes. The entire layer of fiber nodes is established in this way, and the fiber node layer is completely established.

[0074] Finally, the contact between optical fibers and between optical fibers and the core tube is modeled to complete the establishment of the optical fiber layer model;

[0075] The specific steps for modeling the contact between optical fibers and between optical fibers and the core are as follows: The contact between optical fibers is divided into three types: contact between optical fibers in the same layer; contact between optical fibers in the upper layer and the lower layer; and contact between the first layer optical fiber and the conditioning layer. Linear elements are used to simulate the contact for all of these.

[0076] The contact unit modeling between the first-layer optical fiber and the conditioning layer is specifically divided into three types:

[0077] (1) The contact between the standard fiber segment and the middle part of the adjustment layer is achieved by using a rod element. The first standard fiber segment node of the established fiber is extracted, and the fiber radius is reduced along the r direction to obtain the bottom boundary node corresponding to the first standard fiber segment node on the core tube surface. Based on these nodes, the contact element model between the first standard fiber segment and the middle part of the core tube can be established.

[0078] (2) The contact between the cross-turn fiber and the middle part of the adjustment layer is made using beam elements; extract the first layer cross-turn fiber node of the established fiber, and reduce the fiber radius along the r direction to obtain the bottom boundary node corresponding to the first layer cross-turn fiber node on the core cylinder surface. Based on these nodes, the contact element model between the first layer cross-turn fiber and the middle part of the core cylinder can be established.

[0079] (3) The contact between the first layer of optical fiber and the left and right side protrusions of the adjustment layer are all rod units. Extract the node information of the standard arc segment of the first turn and the last turn of the first layer of the established optical fiber respectively, and translate these nodes to the left and right by half the optical fiber diameter respectively to form the left and right boundary nodes of the left side protrusion of the optical fiber bundle and the core tube. Based on these nodes, the contact rod units of the left and right side protrusions of the optical fiber bundle and the core tube can be established.

[0080] Contact modeling between optical fibers in the same layer involves connecting the optical fiber nodes at relative positions of two adjacent turns to form contact units of optical fibers in the same layer.

[0081] The modeling of contact units between optical fibers in the upper and lower layers is specifically divided into two types:

[0082] (1) The standard fiber segment adopts pole unit contact modeling, and connects the fiber nodes of each layer that have contact with the fiber of the next layer to form fiber contact units in the same layer.

[0083] (2) The cross-turn fiber is modeled using beam element contact. Based on the number of unwound turns of the coil, the cross-turn unwound curve between layers is connected to the nodes (excluding the starting point) that are related to the fiber before it to form a cross-turn beam element model. The number of unwound turns is determined according to the actual situation.

[0084] Step 2: Apply boundary conditions and prestress to the existing fiber layer model;

[0085] The boundary conditions can be applied by either applying full constraints on the left end, or by applying symmetry plane constraints, including fixed constraints on the degrees of freedom of rotx, rotz, and uy, and also by applying full constraints on the left end of the core cylinder.

[0086] The prestress is determined based on the tension of the optical fiber during the actual winding process, and is specifically calculated according to formula (1):

[0087]

[0088] Finally, the actual stress of the core cylinder and the existing fiber layer model was obtained by solving the prestress using Ansys software.

[0089] Step 3: Solve for the prestress in Step 2 to obtain the actual stress of the core cylinder and the existing fiber layer model;

[0090] Step 4: Update the model and read in the actual stress of the core and existing fiber layer models;

[0091] The specific operation of updating the model involves modifying the coordinates of the fiber layer nodes based on the displacement results in the current database file, which is implemented by the built-in functions of the Ansys software.

[0092] Step 5: Apply prestress to the current fiber layer model again and solve for and output the stress;

[0093] Step 6: Determine whether the current fiber layer model is the last fiber layer. If yes, output and process the data to complete the modeling. If no, proceed to step 7.

[0094] Step 7: Build the model for the next fiber layer, delete the initial prestress, and return to step 2;

[0095] Example

[0096] A schematic diagram of the complete model of the optical fiber bundle constructed using the finite element modeling method in this embodiment is shown below. Figure 2 As shown, the modeling is performed using the following method:

[0097] An equivalent beam-rod composite model is adopted, with optical fibers treated as composite cross-section beam (wire) elements. Their tensile and bending properties can be precisely controlled by ANSYS settings. The contact between optical fibers is represented by an equivalent virtual contact rod. Therefore, an equivalent contact model is used: compressible but not tensile rod elements are used to simulate the contact.

[0098] Fiber optic modeling rules: The fiber optic model is established in cylindrical coordinates. The radial direction of the fiber coil is r, the circumferential direction is θ, and the direction of the fiber coil's axis of symmetry is z. Fiber winding follows a left-handed helix rule; the direction of the four fingers' bend indicates the fiber winding direction, and the direction of the thumb's movement indicates the forward direction. The fiber's starting angle is -40°, and the helix direction is a left-handed helix. The standard section ranges from -40° to -360°, and the cross-turn section ranges from 0° to -40°, as shown below. Figure 3 As shown.

[0099] The fiber modeling unit is beam188; in the equivalent contact line unit, the contact between the turns of the same layer of fiber and the contact between the fiber and the left and right bosses of the adjustment layer are linked180.

[0100] In the contact between optical fiber layers, the standard section of optical fiber uses link180, the non-standard section of optical fiber uses beam188, and the contact between the optical fiber at the interlayer cross-turn and the other optical fibers uses beam188.

[0101] In the contact between the optical fiber and the conditioning layer, the contact unit at the standard section position is Link180, and the contact unit at the non-standard section position is Beam188.

[0102] The equivalent contact line element uses beam elements in some parts because the special characteristics of the cross-turn area lead to insufficient degree of freedom constraints during the solution process, making it impossible to solve. Therefore, beam elements are used instead.

[0103] Specific modeling scheme: The fiber unit is divided into standard segment and cross-turn segment.

[0104] First, the first standard segment node is generated. Then, the cross-turn segment curve is determined according to the interpolation function, and the curve is discretized into cross-turn segment nodes. The entire layer of fiber nodes is established in this way.

[0105] Finally, the contacts between optical fibers and between optical fibers and the core tube are modeled, thus establishing a complete layer of optical fiber nodes.

[0106] Next, all fiber optic nodes will be established using the method described above for constructing standard fiber optic segments and cross-turn nodes.

[0107] The fiber optic cable is unwound in the following manner: 1.5 turns per layer on the left side and 2.5 turns per layer on the right side, as follows. Figure 4 As shown.

[0108] like Figure 5 As shown, there are three types of contact that occur between optical fibers: contact between fibers in the same layer; contact between fibers in the upper layer and the lower layer; and contact between the first layer fiber and the conditioning layer. Linear elements are used to simulate these contacts.

[0109] First, model the same-layer fiber contact unit, and connect the fiber nodes at the relative positions of each two adjacent turns to form the same-layer fiber contact unit.

[0110] Next, the fiber optic contact unit at the interlayer cross-turn is modeled. There are two types of modeling for the fiber optic contact unit at the interlayer cross-turn: one is the 2.5-turn unwinding case at the right end of the coil, such as... Figure 6 As shown.

[0111] In the case of 2.5 turns unwinding: the curve of the 2.5-turn interlayer cross-turn unwinding segment is related to the three turns of fiber before it. There are 9 nodes (excluding the starting point) connected to the first turn immediately next to it; starting from the 9th node, it is related to the second turn of fiber, and then 5 more nodes are connected; finally, it is connected to the third turn by 7 nodes, for a total of 21 contact rods (the 9th node is connected to both the first and second turn of fiber, and the 13th node is connected to both the second and third turn of fiber).

[0112] Next is the modeling of the contact elements between each layer of optical fiber and the layer of optical fiber below it:

[0113] Interlayer fiber optic contact is divided into two types: standard fiber segments are connected using pole units, while cross-turn fiber segments are connected using beam units. The standard curve segment's contact with the fiber optic layer below is achieved using pole units, and it has contact with the first and second turn fiber units of the layer below. The cross-turn curve segment's contact with the fiber optic layer below is achieved using beam units, and it has contact with the second and third turn fiber units of the layer below. Figure 7 As shown.

[0114] Next is the modeling of the contact elements between each layer of optical fiber and the layer of optical fiber below it:

[0115] Interlayer fiber optic contact is divided into two types: standard fiber segments are connected using pole units, while cross-turn fiber segments are connected using beam units. The standard curve segment's contact with the fiber optic layer below is achieved using pole units, and it has contact with the first and second turn fiber units of the layer below. The cross-turn curve segment's contact with the fiber optic layer below is achieved using beam units, and it has contact with the second and third turn fiber units of the layer below. Figure 8 As shown.

[0116] The last type is the contact unit between the first layer of optical fiber and the adjustment layer. The connection between the standard section of optical fiber and the middle part of the adjustment layer uses rod units, while the connection between the inter-turn section of optical fiber and the middle part of the adjustment layer uses beam units. The connection between the first layer of optical fiber and the adjustment layer bosses is also a rod unit.

[0117] Contact units between the optical fiber and the adjustment layer: Extract the first layer nodes of the established optical fiber, and reduce the fiber radius along the r-direction to obtain the bottom boundary nodes on the core tube surface corresponding to the first layer fiber nodes. Based on these nodes, contact units between the optical fiber sheath and the middle part of the core tube can be established. These contact units are divided into two types: beam units at the fiber crossover points and rod units at standard sections.

[0118] Contact units between the optical fiber and the left and right bosses of the adjustment layer: Extract the node information of the standard arc segments of the first and last turns of the first layer of the established optical fiber, and shift these nodes to the left and right by half the optical fiber diameter, respectively, to form the left and right boundary nodes of the left boss of the optical fiber sheath and the core. Based on these nodes, the contact rod units for the left and right bosses of the optical fiber sheath and the core can be established, such as... Figure 9 As shown.

[0119] After the fiber optic part is modeled, the polytetrafluoroethylene (PTFE) conditioning layer is modeled: the conditioning layer is modeled using solid185 solid elements.

[0120] Modeling the middle section: The contact between the first layer of optical fiber and the bottom cylinder is modeled using compressible but not tensile rod elements. Therefore, the node arrangement on the adjustment layer should be consistent with the node arrangement of the first layer of optical fiber. The middle section of the adjustment layer is 2mm thick, with a total of 5 nodes and 4 element layers. Modeling the left and right side bosses: The bosses are 0.5mm higher than the middle section, and the optical fiber diameter is 0.36mm. The sides of the bosses only contact one layer of optical fiber, so the bosses are built as 2 element layers. The thickness of the bottom element is half the diameter of the optical fiber, facilitating contact rod connection with the optical fiber. Figure 10 As shown.

[0121] The carbon fiber layer is modeled using shell 181 elements. Its node arrangement is consistent with the bottom layer of the adjustment layer, with the nodes of the bottom layer of the adjustment layer reduced by 0.5mm radially. The element creation order for the carbon fiber layer is the same as that for the adjustment layer: first, create the nodes and elements in the middle section; then, create the nodes and elements on the left and right sides; finally, fill in the elements at the gaps. Figure 11 As shown.

[0122] Finally, the carbon fiber layer and the PTFE adjustment layer are connected. To investigate slippage between the carbon fiber layer and the adjustment layer, connection units are modeled. The modeling is divided into: a left-side rod connection unit for the carbon fiber layer and the adjustment layer snapping together, a beam connection unit at the snapping point, and a right-side rod connection unit. Since the lengths of the protrusions on both sides are much shorter than the length of the middle part of the adjustment layer, the connection between the carbon fiber layer and the adjustment layer under the protrusions on both sides is ignored.

[0123] To simulate the effect of the carbon fiber layer clips on the adjustment layer, beam elements were used to model the connection between the carbon fiber layer and the adjustment layer at the clips. Specifically, the clips are located approximately in the middle of the carbon fiber layer, with a width equal to 8 turns of fiber diameter. Therefore, the starting position of the clips is at turns 2-4 of the first layer. The remaining connections are represented by rod elements, such as... Figure 12 As shown.

[0124] like Figure 13 As shown, an optical fiber structure generally includes at least an optical fiber core and a buffer coating; some types of optical fibers also include an outer coating, such as... Figure 11 As shown. Here we calculate based on two layers. In the equivalent contact example, the fiber diameter is 0.36 mm, the inner layer diameter is 0.12 mm, and the axial length is 2 mm. One end of the rigid plate is fixed, and the other end of the rigid plate is displaced by 0.01 mm along the fiber radius. The nodes at both ends of the fiber are constrained in the UZ direction.

[0125] The actual stiffness value is obtained from the formula. The stiffness of the equivalent line element should be consistent with it. The equivalent elastic modulus can be obtained by giving the diameter of the line element. The material properties are shown in Table 1.

[0126] Table 1 Material Properties

[0127]

[0128] Extract the support reaction force values ​​at the nodes where the cylindrical solid contacts the rigid plate.

[0129] From the formula Its actual stiffness is:

[0130] Therefore, the stiffness of the rod element used to simulate fiber optic contact should also be K. 杆 =5726.88. With the same force applied to both ends of the rod element at this stiffness, according to the formula, EA = K. 杆 If the diameter of the rod unit is 0.18 mm, then the elastic modulus is...

[0131] For line element modeling, the first step is to generate a list of key node information on the 0° cross-section of the line package. Line package modeling is performed in cylindrical coordinates, with the radial direction of the line package as r, the circumferential direction as θ, and the symmetry axis direction as z. Data processing is first performed using Mathematica software. First, the list of key node information on the 0° cross-section of the line package is generated: the z-coordinate of the centerline of the first turn in each layer is calculated. The total number of turns in each fiber layer is directly determined through calculation, thus naturally determining the right boundary of each fiber layer. The number of turns in the next layer is calculated based on the number of turns removed from the left and right sides. Simultaneously, the starting position of the current layer's fiber turn is determined based on the number of turns removed from the left end of the line package and the starting position of the previous layer's fiber turn. This process is repeated until the last layer of fiber turn nodes is generated. The key nodes of the first layer of fiber are extracted, and the key nodes of the first layer are uniformly reduced by half the fiber diameter to obtain the core tube key nodes. Several nodes are added to the left of the core tube key nodes to form the core tube boundary. More nodes are added to the left to ensure that the constraint position deviates from the fiber itself. The boundary on the right side can be directly added.

[0132] Let the number of turns of the first layer of optical fiber in the coil be n. k1 The number of unwound turns on the left side of the coil is n. bl The number of unwound turns on the right side of the coil is n. br The maximum number of layers in the coil is l max Then the number of critical nodes n of the core tube can be obtained. c Number of critical nodes per fiber layer n ki and the total number of fiber optic critical nodes n k for:

[0133] n c = k1 +5

[0134] n ki = k1 -(i-1)(n bl + br), i = (1, 2, ... l max )

[0135]

[0136] like Figure 14 As shown, taking an optical fiber coil with 20 turns in the first layer, a total of 4 layers, 1.5 unwound turns on the left side, and 2.5 unwound turns on the right side as an example, the following is generated: Figure 12 The list of key node information on the 0° cross-section of the coil shown is as follows: the number of key nodes in the core is 25, and the number of key nodes in the optical fiber is 56.

[0137] Generate the connection relationships on the 0° cross-section of the coil. This requires generating the basic modeling lines for the core shell unit, as well as the modeling lines for the beam unit when the core shell contacts the optical fiber, the horizontal contact beam modeling lines for each layer of optical fiber, and the oblique contact beam lines between layers. The key nodes of the core shell are located in the first set of data in the key node information list on the 0° cross-section of the coil, and the key nodes of each layer of optical fiber are located in the subsequent sets of data in the node information list. Establishing connection relationships involves connecting the nodes in each set of data, such as... Figure 15 The image shows the cross-sectional lines of the obtained beam model.

[0138] Establish as Figure 16 The example shown is a rotating model of the cross-section lines of a beam. All nodes of the optical fiber and core are generated by rotation. The nodes are divided into multiple faces according to the circumferential curvature, and the node numbers on each face have the same increment relative to the previous face. The example model has 7 faces.

[0139] Create a core cylinder element, enclosing four key points of the core cylinder on adjacent faces into a surface element. Based on the aforementioned cross-sectional line connection relationships, establish the connection relationships between fiber nodes on the first face of the rotation model, as well as the connection relationships between fiber nodes and core cylinder nodes. It is necessary to generate fiber elements and contact rod elements layer by layer and solve them; therefore, the following is given first... Figure 17 The diagram shows the connection relationship between the first-layer fiber optic nodes and the second-layer fiber optic nodes.

[0140] The finite element analysis elements selected are Beam188 and Shell181, with the beam element used for modeling the optical fiber and contact rod, and the shell element used for modeling the core cylinder. Three material properties corresponding to the optical fiber element, contact rod element, and core cylinder element are defined, as shown in Table 2. Three cross-sectional types corresponding to the optical fiber element, contact rod element, and core cylinder element are defined, as shown in Table 3.

[0141] Table 2 Material Properties

[0142]

[0143] Table 3. Cross-sectional parameters of line and surface elements

[0144]

[0145] The wire element model applies boundary conditions to the coil according to the actual situation. The model is divided into a partial model and a full-loop model. The partial model requires the application of symmetry plane constraints, including fixed constraints on the degrees of freedom of rotx, rotz, and uy, as well as full constraints on the left end of the core tube; the full-loop model only requires full constraints on its left end. To simulate the tension application problem of optical fiber during the actual coil winding process, a layer-by-layer modeling and solving approach is adopted. This ensures that after the modeling of each layer of optical fiber is completed, the axial tension of the surface layer optical fiber unit of the coil is the specified winding tension value.

[0146] This invention achieves overall modeling of the fiber optic coil by modeling and solving layer by layer, resulting in a coil with a winding width of 177 mm and a winding pitch of 0.36 mm. Specific parameters include an optical fiber diameter of 0.36 mm, 400 turns in the first layer, 1.5 turns on the left and 2.5 turns on the right for a total of 69 layers, and a core outer diameter of 55 mm. This invention solves the modeling problem of the fiber optic coil, laying the foundation for studying the internal stress of the coil after winding, and is of great significance for improving the stability and release reliability of the fiber optic coil.

Claims

1. A method of finite element modeling of a fiber optic cable, characterized by, An equivalent beam-rod combined model is adopted, in which the compressible and inextensible rod elements are used to simulate the contact between optical fibers, and the optical fibers are treated as composite cross-section beam elements. According to the actual winding condition of the wire package, the tension of the optical fiber during the actual winding process is simulated, and the modeling is built and solved layer by layer, and finally the modeling of the optical fiber wire package is completed. Ansys software is used to establish the optical fiber model in the cylindrical coordinate system. The radial direction of the wire package is r, the circumferential direction of the wire package is θ, the direction of the wire package symmetry axis is z, the optical fiber winding complies with the left-hand spiral rule, the four-finger bending direction is the winding direction of the optical fiber, the thumb direction is the forward direction, the initial angle of the optical fiber is-40°, the spiral direction is left-hand spiral, the standard section is-40° to-360°, and the cross-section section is 0° to-40°. The following steps are implemented: Step 1: Establishing a core barrel model and a first layer of optical fiber model in the cylindrical coordinate system; The step 1 core barrel model includes a carbon fiber layer inside and an adjusting layer outside, and is divided into a middle part and left and right side bosses as a whole, and the specific establishment method is as follows: Modeling of the adjusting layer: the adjusting layer is modeled by solid185 solid element; Middle part modeling: the contact between the first layer of optical fiber and the bottom barrel is modeled by using compressible and inextensible rod elements to establish an equivalent contact model, and the arrangement of nodes on the adjusting layer is consistent with the arrangement rule of the first layer of optical fiber nodes; Left and right side boss modeling: the boss is higher than the middle part by half the diameter of the optical fiber, and is modeled by using rod elements; Modeling of the carbon fiber layer: the carbon fiber layer is modeled by shell 181 shell element: the node arrangement is consistent with the node arrangement of the bottom layer of the adjusting layer, and the element establishment method of the carbon fiber layer is consistent with the element establishment method of the adjusting layer, Modeling of the contact between the carbon fiber layer and the adjusting layer: buckles are provided between the carbon fiber layer and the adjusting layer, the contact at the buckles is modeled by beam elements, and the rest of the contact positions are modeled by rod elements; The establishment method of the step 1 optical fiber layer model is as follows: Divide the optical fiber into standard sections and cross-section sections, model the standard section optical fiber by link180 element, and model the cross-section section optical fiber by beam188 element; Generate a first turn standard section node, which is the center point of the optical fiber cross section, then determine the cross-section section curve according to the interpolation function, and then discretize the curve into cross-section section nodes, and establish the nodes of the whole layer of optical fiber in this way, thus the nodes of one layer of optical fiber are completely established; Finally, the contact between the optical fibers and the contact between the optical fibers and the core barrel are modeled, and the establishment of the optical fiber layer model is completed; The specific operation of modeling the contact between the optical fibers and the contact between the optical fibers and the core barrel is as follows: the contact between the optical fibers is divided into three types: the contact between the optical fibers in the same layer; the contact between the optical fibers in the upper and lower layers; and the contact between the first layer of optical fiber and the adjusting layer. Linear elements are used to simulate the contact for these contacts; The contact element modeling between the first layer of optical fiber and the adjusting layer is specifically divided into three types: (1) The contact between the standard section optical fiber and the middle part of the adjusting layer is modeled by rod elements. The first layer of standard section optical fiber nodes of the established optical fiber are extracted, the bottom boundary nodes corresponding to the first layer of standard section optical fiber nodes on the surface of the core barrel are obtained by reducing the optical fiber radius along the r direction, and the contact element model of the first layer of standard section optical fiber and the middle part of the core barrel is established according to these nodes. (2) The contact between the cross-turn section fiber and the middle part of the adjusting layer adopts a beam element; the first layer of cross-turn section fiber nodes of the established fiber are extracted, and the bottom boundary nodes corresponding to the first layer of cross-turn section fiber nodes on the surface of the core barrel are obtained by reducing the fiber radius in the r direction, and the contact element model between the first layer of cross-turn section fiber and the middle part of the core barrel is established according to the nodes; (3) The contact between the first layer of fiber and the left and right side bosses of the adjusting layer is a rod element, the node information of the standard circular arc section of the first turn and the last turn of the first layer of the established fiber is extracted, and the left and right boundary nodes of the fiber package and the left and right side bosses of the core barrel are formed by translating the nodes to the left and right by half of the fiber diameter, and the contact rod element between the fiber package and the left and right side bosses of the core barrel is established according to the nodes; The contact between the fibers in the same layer is modeled by connecting the fiber nodes at the relative positions of each adjacent two turns to form the contact element of the fiber in the same layer; The contact element modeling between the upper layer and the lower layer of fiber is divided into two kinds: (1) The standard section fiber adopts a rod element contact modeling, and the fiber nodes of each layer and the next layer of fiber are connected to form the contact element of the fiber in the same layer; (2) The cross-turn section fiber adopts a beam element contact modeling, and the nodes related to the cross-turn section curve and the fiber before it are connected according to the number of turns of the wire package, except for the starting point, to form the cross-turn section beam element modeling, and the number of turns is determined according to the actual situation; Step 2, apply boundary conditions and prestress to the existing fiber layer model; Step 3, solve the actual stress of the core barrel and the existing fiber layer model under the prestress of step 2; Step 4, update the model and read in the actual stress of the core barrel and the existing fiber layer model; Step 5, apply prestress to the current fiber layer model again and solve and output the stress; Step 6, determine whether the current fiber layer model is the last fiber layer, if yes, output and perform data processing, complete modeling, if not, go to step 7; Step 7, establish the next fiber layer model, delete the initial prestress, and return to step 2.

2. The finite element modeling method of an optical fiber line package according to claim 1, characterized by, In step 2, the boundary conditions are applied by fully constraining the left end, or by applying symmetric face constraints, including fixed constraints of rotx, rotz and uy degrees of freedom, and also applying full constraints to the left end of the core barrel; The prestress is determined according to the tension of the fiber during the actual wire winding process, and is calculated according to formula (1): （1） Finally, the actual stress of the core barrel and the existing fiber layer model is obtained by solving the prestress by Ansys software.

3. The finite element modeling method of an optical fiber line package according to claim 1, characterized in that, In step 4, the model updating operation is to modify the fiber layer node coordinates according to the displacement results in the current database file, which is realized by the self-function of Ansys software.

Images