The FEA Editor always keeps separate vertices (duplicate vertices) at the boundaries between different parts. That is, two or more vertices exist at the same coordinate: one for each part. The type of contact determines whether the separate vertices create one node shared by the parts (bonded contact), or whether two separate nodes are created but not connected together (free contact), or whether two separate nodes are created and connected together with an automatically-generated element (surface contact). The merging of the vertices occurs when the Check Model is performed. Depending on the analysis type, element type, and contact type, the mesh may need to be matched between the contacting parts.
The following table indicates whether adjacent parts within an assembly need to be modeled with a zero-gap fit, or if an initial gap or interference is allowed between parts for the various analysis and contact types:
Analysis Category | Is Initial Gap or Interference Allowed Between Surfaces? |
---|---|
Linear | No. Must be zero gap, zero interference (except for Free contact). |
Nonlinear |
Yes, for Surface and Free contact. No, for other types of contact. |
Thermal | No. Must be zero gap, zero interference (except for Free contact). |
Electrostatic | No. Must be zero gap, zero interference (except for Free contact). |
The following table indicates whether or not the meshes need to be matched between adjacent parts for different analysis and contact types:
Type of Contact | ||||||
---|---|---|---|---|---|---|
Analysis Type | Bonded | Welded | Free/No Contact | Surface Contact (see Note 4) | Edge Contact | Shrink Fit Contact |
Linear, Static Stress | matched or unmatched (see Note 1) | matched or unmatched (see Note 1) | matched or unmatched | matched | matched | matched (see Note 5) |
Linear, Natural Frequency (Modal) and Natural Frequency (Modal) with Load Stiffening | matched or unmatched (see Note 1) | matched or unmatched (see Note 1) | matched or unmatched | Sliding/No Separation only (matched) | not applicable | not applicable |
Linear, Critical Buckling Load and Transient Stress (Direct Integration) | matched or unmatched (see Note 1) | matched or unmatched (see Note 1) | matched or unmatched | Sliding/No Separation only (matched) | not applicable | not applicable |
Linear, Other (see Note 2) | not applicable | not applicable | ||||
Nonlinear | matched or unmatched (see Note 3) | matched | matched or unmatched | matched or unmatched | not applicable | not applicable |
Thermal | matched or unmatched (see Note 1) | matched or unmatched (see Note 1) | matched or unmatched | matched | not applicable | not applicable |
Electrostatic | matched or unmatched (see Note 1) | matched or unmatched (see Note 1) | matched or unmatched | not applicable | not applicable | not applicable |
Note 1: If using smart bonding, the mesh can be matched or unmatched. If not using smart bonding, then the mesh must be matched to be bonded. Smart bonding is set under the following dialog boxes. See the referenced pages for details on smart bonding, including the limitations on the element types.
Note 2: The following analysis types use the results from the modal analysis. Therefore, these analysis types can take advantage of the smart bonding without any additional contact setup required:
Note 3: The mesh can be unmatched if using tied surface contact to perform the bonding, in which case the contact type would be Surface. If not using tied surface contact, then the mesh must be matched, and the contact type is Bonded. Tied surface contact is set under the Settings for the contact pair. See the page Setting Up and Performing the Analysis: Nonlinear: Loads and Constraints: Surface-to-Surface Contact: Surface-to-Surface Contact Options for details on tied contact.
Note 4: The Surface Contact column refers to three available contact types—Surface, Slide/No Separation, and Separation/No Sliding.
Note 5: The Shrink Fit Contact column refers to two available contact types—Shrink Fit/Sliding and Shrink Fit/No Sliding. The amount of interference between parts can be represented in the CAD geometry (by overlapping the parts). Upon importation of the model into Simulation Mechanical, the surfaces are matched (zero interference, zero gap). That is, the interference is removed from the geometry and the mesh is matched between the parts. However, the amount of interference is retained in numerical form. For further discussion of this, see the Shrink Fit / Sliding and Shrink Fit / No Sliding sections below.
The type of contact specified by the top-level Contact (Default: __) setting in the tree view is applied to any two surfaces and are either not listed individually, or are listed individually but set as Default contact type. For example, if it can be assumed that all parts of an assembly are in perfect connection with each other – able to transmit all types of loads at their interface – then you can leave the default contact set to Bonded.
Each of the available types of contact are covered in the following sections.
If the Default command is selected for a contact entry, the type of contact will follow the global Contact (Default: __) setting. Default can only be selected in the tree view for an existing contact pair; it cannot be selected when creating the contact pair.
Bonded contact is applicable to all element types. The two surfaces will be in perfect contact throughout the analysis when bonded, and the loads are transmitted from one part to the adjacent part. In a stress analysis, when a node on one surface deflects, the node on the adjoining surface will deflect the same amount in the same direction. In a heat transfer analysis, the same temperature occurs in each part at the connection, and so forth.
Smart bonding is a method to connect the nodes on adjacent parts even though the meshes do not match. (See the Notes for Table 1 to activate the smart bonding and limitations on element types and analysis types.) Since the nodes may not line-up, a tolerance is required to match the mesh from part A surface B with the mesh from part C surface D. When using smart bonding, right-click a contact pair in the tree view and choose Settings to access the tolerances. The two options for the Tolerance type are as follows:
When the contact type is defined as part A with part C or part A with part C surface D, any nodes on part A within the tolerance of part C surface D will be bonded with the smart bonding. This may affect what size tolerance you want to use. (Technically, the software determines which surface is bonded to the adjacent surface. It does not depend on the order of the entry shown in the tree view.)
Smart bonding transmits loads from the nodes on one part to the adjacent nodes on the other part by using equations to link the degrees of freedom (displacements for stress analysis, temperature for heat transfer) of the parts together. This is done with the same method as multi-point constraints. (For details on user-defined multi-point constraints, see the page Setting Up and Performing the Analysis: Linear: Loads and Constraints: Multi-Point Constraints.) In stress analysis, the translations are linked for brick and 2D elements. For plate to plate elements, the translations and rotations are linked. See Figure 1 for examples.
Since the nodes on surface D may be connected to nodes on surface B outside the area of surface D, the smart bonding can distribute the load from part C to part A over a larger area than the physical contact area. Naturally, the degree that the load is spread out depends on the size of the mesh. See Figure 1(a).
TX 26 = TX 22 + (a/b)(TX 23 -TX 22 ) TY 26 = TY 22 + (a/b)(TY 23 -TY 22 ) TZ 26 = TZ 22 + (a/b)(TZ 23 -TZ 22 ) T is translation in X, Y, or Z at indicated node. |
|
(a) Solid (P1) to solid (P2) connection with smart bonding, stress analysis. Since part 2 is connected to part 1 at nodes 22 and 23, the load is transferred over a larger area than the interface between parts 1 and 2. This approximation is more accurate as the mesh size on part 1 is reduced. |
|
TY 26 = TY 22 + (a/b)(TY 23 -TY 22 ) TZ 26 = TZ 22 + (a/b)(TZ 23 -TZ 22 ) RX 26 = 0 R is rotation about X, Y, or Z at indicated node. |
|
(b) Plate (P2) to solid (P1) connection with smart bonding, stress analysis. (2D view considered for simplicity) |
|
T 26 = T 22 + (a/b)(T 23 -T 22 ) T is the temperature at the indicated node. |
|
(c) Solid to solid connection with smart bonding, heat transfer analysis. | |
Figure 1: Smart Bonding Examples |
Use smart bonding to connect the midside nodes on part A (a part where more accurate results are desired) with the corner nodes on part B (a part without midside nodes, not requiring as high of accuracy).
Without smart bonding, the midside nodes in the part on the right can pull away from the face of the left part. (Only nodes on contact face shown for clarity.) | With smart bonding, the midside nodes are bonded to the face of the left part. Thus, the midside nodes cannot pull away. (Parts shown with slight gap for clarity.) |
Figure 2: Bonding Midside Nodes |
Models created prior to the introduction of smart bonding may have relied on an un-matched mesh to create free surfaces even though the contact type was set to bonded. If such models are re-analyzed, the smart bonding should not be enabled; otherwise, such surfaces will now behave as bonded. See Figure 3. (By default, smart bonding is disabled for legacy models.)
(a) Prior to smart bonding, parts are not bonded because the nodes do not match. (Actually, no type of contact would have worked since the nodes do not match.) A tangential force F causes the parts can separate. |
(b) If the same model is opened in software with smart bonding capability, and if the contact type is bonded, and if smart bonding is enabled, the parts will bond even though the nodes do not match. Thus, the parts will not separate. To avoid this, either deactivate the Enable smart bonded/welded contact option, or set the contact type for the appropriate surfaces to Free/No Contact. |
Figure 3: Free Contact with Unmatched Mesh (Older Models) |
Spot welding is an example of congruent surfaces where some nodes do not match and you do not want these nodes to be bonded.
The above discussion (Figure 1) implied that the nodes on part 2 are connected to the nodes on part 1. You do not have this level of control. Instead, you specify whether the nodes on the surface with the coarser mesh are connected to the other side, or vice versa. This selection is made from the Setup Model Setup Parameters dialog box. Beyond the user-selection, the software decides which surface is the finer mesh and which is coarser. Note that all elements on the contacting surface are considered; the mesh size at a portion of the contact surface is not the deciding factor between fine and coarse. Only nodes that are within the tolerance (see above) of the opposite surface are used; nodes outside the contact area are not used to determine fine or coarse. For example, if you define a contact pair between parts 1 and 4, then all nodes that contact between parts 1 and 4 are counted regardless of whether the contact is at one face or many faces; the part with the fewer contact nodes becomes the coarser mesh. (The same is true for the default contact setting; all contact nodes between two parts are used to determine whether the mesh is fine or coarse.) For contact pairs that define contact between part/surface and part/surface, the nodes that contact on the specified surfaces are used to determine which mesh is fine or coarse.
When choosing what type of smart bonding to use (Coarse bonded to fine mesh or Fine bonded to coarse mesh), it is helpful to consider what is supposed to occur at the interface between the two parts. This is demonstrated in figures 4 through 7.
For stress analysis where the interface experiences pure compression, all of the nodes on the interface should deflect the same amount. Thus, choosing Fine bonded to coarse mesh will give more accurate results. See Figure 4.
(a) The Model. A simple compression model. |
(b) Incorrect. When using Coarse bonded to fine mesh smart bonding, only the nodes on the coarse mesh are forced to follow the displacement of the fine mesh. Thus, the inner nodes on the fine mesh are free to move independently. As seen here in this exaggerated displacement plot, the fine mesh displaces incorrectly. |
(c) Correct. When using Fine bonded to coarse mesh smart bonding, the nodes on the fine mesh are forced to follow the displacement of the coarse mesh. Both meshes deflect as desired (although the fine mesh is forced to displace linearly at the nodes between the coarse element nodes. This might introduce some inaccuracy). The same exaggerated displacement scale used in (b) is shown here. |
Figure 4: Stress Analysis Under Pure Compression |
For stress analysis where the interface experiences bending, the nodes on finer mesh surface must be allowed to move independently of the nodes on the coarser mesh; that is, both sets of nodes should displace so as to create the same radius of curvature. Thus, choosing Coarse bonded to fine mesh will give more accurate results. See Figure 5.
(a) The Model. A simple bending model. |
(b) Incorrect. When using Fine bonded to coarse mesh smart bonding, the nodes on the fine mesh are forced to follow the displacement of the coarse mesh. By forcing the fine mesh to bend to the same curvature produced by the coarser mesh, the displacement results are less accurate. Because of the kink or sudden change in slope in each set of 4 elements in the bottom part, the stress results in particular would show high stresses. The same exaggerated displacement scale used in (c) is shown here, so this deflection is noticeably smaller. |
(c) Correct. When using Coarse bonded to fine mesh smart bonding, only the nodes on the coarse mesh are forced to follow the displacement of the fine mesh. Thus, the inner nodes on the fine mesh are free to move independently. Although the displacement of the bottom part may appear to be incorrect because of the separation from the top part (greatly exaggerated here to show the shape better), the fact that both parts follow the proper curvature indicates that these results are more accurate. |
Figure 5: Stress Analysis Under Pure Bending |
In heat transfer analysis, the flow of heat should be continuous from the finer mesh into the coarser mesh. Thus, choosing Fine bonded to coarse mesh will give more accurate results. See Figure 6. Similar philosophy applies to electrostatic analysis.
(a) The Model. A simple two-part model with the bottom surface exposed to a hot environment and the top surface exposed to a cold environment. Since the parts are practically the same width, this 2D model represents a 1-D heat transfer. |
(b) Incorrect. When using Coarse bonded to fine mesh smart bonding, only the nodes on the coarse mesh are forced to follow the temperature of the fine mesh. Thus, the inner nodes on the finer mesh (shown by the dots) are not connected to the top part. These create a blockage to the flow of heat (shown by the arrows at the center of each element.) The heat must flow sideways at the blocked nodes to get to the top part; this creates a less accurate temperature profile. |
(c) Correct. When using Fine bonded to coarse mesh smart bonding, the nodes on the fine mesh are forced to follow the temperature of the coarse mesh. Thus, only the two outer nodes (shown by the dots) are not connected to the top part. With a reduced blockage to the flow of heat, the heat flux vectors are closer to being parallel (as they should be for 1-D heat transfer). The result is a more accurate temperature profile. |
Figure 6: Heat Transfer Analysis |
Another consideration in choosing the type of smart bonding is that there needs to be nodes on the chosen surface that physically match the opposite surface. See Figure 7.
Coarse bonded to fine mesh smart bonding versus Fine bonded to coarse mesh smart bonding. If only nodes on the coarse (bottom, red) part are bonded to the fine (top, green) part by choosing Coarse bonded to fine mesh, then only one node (the one on the right) will be bonded. No other nodes will be bonded since the nodes on the coarse mesh do not touch the other part. If this were a stress analysis, the top part could be statically unstable. For this example to work, the better choice would be Fine bonded to coarse mesh smart bonding. All nodes on the top part will be bonded to the nodes on the bottom part because all of those nodes touch the bottom part. |
Figure 7: Bonding Drastically Different Mesh Sizes |
Keep in mind that smart bonding approximates the transfer of loads at the boundaries of two parts. In a stress analysis, the continuity of the displacements is conserved. Other quantities such as force, stress, derivative of the displacements are not continuous. Therefore, the results at the boundary where smart bonding occurs may be inaccurate depending on the relative mesh density. However, results remote from the boundary should be accurate, relative to the effects (if any) caused by the smart bonding. If accurate results are desired at the boundary between the parts, smart bonding should not be used; the meshes should be matched instead.
One advantage of smart bonding is to perform what-if studies and change the mesh on one part without the need to re-mesh the entire model. The smart bonding will maintain the connection at the contact faces even though the mesh may not align. See Figure 8.
Figure 8: Example Use of Smart Bonding. A mesh sensitivity study can be performed by changing the mesh on part 2 [P2] without the need to re-mesh the entire model. The geometry of part 2 can even be changed, such as comparing a chamfer versus a large radius fillet versus a small radius fillet. |
The equations created with smart bonding are solved using a penalty method. A stiffness is applied to the MPC equations, and this stiffness is added to the normal stiffness matrix. The stiffness of the penalty equations depends on the Solution method you choose (see Multi-Point Constraints). For the Penalty Method you enter the stiffness in the Penalty multiplier field. A multiplier of 0 implies that the parts are not connected, and a multiplier of infinity implies a perfect bonding between the parts. Unfortunately, infinite stiffness is not acceptable in a numerical solution, nor is it required. Generally, a penalty multiplier on the order of 1E4 to 1E6 provides a satisfactory solution. However, some analyses may give a maximum to minimum stiffness warning (max/min stiffness) or fail to find a solution if the penalty multiplier is too large.
To judge the accuracy of the solution, the summary file includes a line with the satisfaction factor. A value of 100% indicates that the MPC equations (such as in Figure 1) are satisfied accurately. Any value less than 100% indicates some separation of the parts. It is not possible to say that X% indicates the solution is wrong. Rely on experience to judge when the satisfaction indicates an unacceptable result.
Welded contact is applicable only to brick and 3D element types. If the Welded command is selected, the nodes along the edges of the contact surfaces act the same as if the Bonded command were selected. The nodes along the interior of these surfaces act the same as if the Free/No Contact command were selected.
Free/No Contact is applicable to all element types. If the Free/No Contact command is selected, the nodes on the two surfaces in this contact pair will not be collapsed to one node even if the mesh is matched. In a CAD model, the mesher will not necessarily force the mesh to match. These nodes will not transmit a load between the parts. In a stress analysis, the nodes will be free to move relative to the nodes on the other surface. In a heat transfer analysis, no heat will be conducted between the parts, and so forth.
Surface contact is applicable only to the element types indicated below. Surface contact is available for CAD solid models, 2D created meshes, and hand-built models as follows.
If the Surface Contact command is selected, a zero-length contact element (similar to a user-created gap element) is placed between the nodes. The nodes will be free to move away from each other, but the nodes cannot pass through each other when they come into contact. Imagine a very small line created between the nodes on these surfaces. If that line becomes longer during the analysis, it will have no effect on the model. If that line becomes zero length, it will act as a spring with a stiffness value that will resist this motion.
When using Surface Contact, the analysis will involve an iterative process; hence, the analysis will take longer to run than an analysis with bonded contact. This process will be used to determine if the deflection due to the loading will cause each pair of nodes on these surfaces to be in contact or not.
When the contact elements are defined for surface contact pairs, a direction is calculated for each contact element. The method used for calculating this direction can be specified by right-clicking on the heading for the surface contact par in the tree view and selecting the Settings command to access the Contact Options dialog. The direction calculation method can be selected in the Surface contact direction drop-down box. The default option of Calculate by matching directions will calculate the direction from the normals of the elements at each node. This is the recommended method. If a mesh is coarse, some of the elements may be non-flat (i.e. the fourth node is not coplanar with the other three). In this case the default method may not result in valid directions. To achieve valid directions, you can increase the value in the Direction tolerance angle field. If one of the surfaces does contain flat elements, you can correct the direction calculation by selecting either the Normal to the first part/surface or Normal to the second part/surface option in the Surface contact direction drop-down box. You should select the option for the part/surface that contains flat elements.
Friction can be added to a contact pair or the default contact if Surface Contact or Edge Contact is selected. To turn on friction, right-click the contact pair and then select the Settings command. This will open a dialog that will allow you to activate the Include friction check box and define the Static friction coefficient. Contact in Static Stress with Linear Material Models analyses assumes that the contact force is transmitted through the same set of nodes as originally in contact and the direction of the force is the same as the original normal direction. That is, the deflection does not change the points in contact or direction (small deformation theory).
In Figure 9, a block is on a fixed surface. A normal force, N, is applied to allow the generation of a friction force, F f .A static coefficient of friction of μ exists between the block and the fixed surface. A lateral force, F is applied to the block. A spring is placed between the block and a wall to create a statically stable model. F f can range from 0 to μN as follows:
For F <= μN: F f =F F s =0 |
For F >= μN: F f =0 F s =F |
Figure 9: Static Friction
In summary, once the force exceeds the maximum value of the friction force, the friction force goes to zero and no longer resists the motion. If what happens after this is important, a Mechanical Event Simulation (MES) analysis using surface to surface contact should be performed. In MES, a dynamic coefficient of friction can be defined to calculate the friction force after the static friction force is exceeded.
The contact parameters in a Mechanical Event Simulation/nonlinear static stress analysis are entered in the surface to surface contact screens. Both static and sliding (dynamic) friction can be included in the analysis. For details, see the page Setting Up and Performing the Analysis: Nonlinear: Loads and Constraints: Surface-to-Surface Contact.
Surface contact in a thermal analysis creates a zero-thickness 2D or 3D element between the surfaces. Since the nodes on the two parts are not merged together, there will be a temperature gradient across the joint.
For a thermal analysis, a contact resistance can be defined for any surface contact pair. This can be used to simulate imperfect contact resulting in a temperature gradient between the parts. This can also be used to simulate a thin film between two parts. You can define the resistance by right-clicking on the heading for the contact pair and selecting the Settings command. You can choose Total Resistance or Distributed Resistance in the Thermal Resistance: drop-down box. If the Total Resistance option is selected, the resistance value defined in the Value: field will be evenly distributed over the surface pair. (For 2D planar models, the total resistance is for the thickness of the mating parts. For 2D axisymmetric models, the total resistance is for 1 radian.) If the Distributed Resistance option is selected, the value defined in the Value: field will be divided by the area of the contact pair and applied to the model.
Contact elements are not created at boundaries where two parts with surface contact are bonded to a different part (or multiple parts). For example, imagine parts 2 and 4 are defined as surface contact with each other and bonded to part 1. See Figure 10(a). A detail of the joint shows that parts 2 and 4 are separated from each, and the gap is filled with an 8-node thermal contact element (for 3D models) or 4-node thermal contact element (for 2D models). See Figure 10(b). However, no contact element is created at the location where parts 2 and 4 are bonded to part 1.
(a) Example three part model. Parts 2 (P2) and 4 (P4) have surface contact defined between them. Both are bonded to part 1 (P1). |
contact element (b) Detailed view of the contact between the parts. Thermal contact elements are create everywhere except for the element in contact with part 1 because of the bonding. Thus, the contact area between parts 2 and 4 is smaller than ideal. (The gap between parts 2 and 4 is exaggerated for clarity. No gap is created in the analysis.) |
Figure 10: Example Thermal Contact |
Bonds contact surfaces in the normal direction while allowing the surfaces to slide relative to each other in the tangential direction.
Contact surfaces can partially or fully separate in the normal direction, but cannot slide relative to each other in the tangential direction.
If the Edge Contact command is selected, the nodes along the edges of the contact surfaces will act the same as if the Surface Contact command were selected. The nodes along the interior of these surfaces will act as if the Free/No Contact command were selected.
Behaves like Surface Contact but with initial interference between the contacting parts. The Contact Options dialog box includes an Interference input field and an Automatic checkbox to the right of this field. If your model is CAD-based and there is geometric interference in the CAD assembly, the interference is removed from the geometry and the meshes are matched to each other in a net fit (zero-interference, zero-clearance). However, the interference from the original CAD assembly is retained numerically. You will still have to define shrink fit contact in Simulation Mechanical (assuming you want to quantify the effects of the interference). The Automatic interference option is activated by default, and the interference magnitude is assigned automatically on a node-by-node basis (that is, it can be non-uniform).
If you disable the Automatic option, or if you are using a hand-built model or a CAD model without geometric interference, you can specify a uniform radial interference between the contacting parts. For example, if a bearing with a bore of 40 mm diameter is pressed onto a 40.03 mm diameter shaft, the radial interference is 0.015 mm [half of the diametral interference, or (40.03-40) / 2]. Manually specifying the interference is a quick way to determine the effects of various intensities of fit without having to modify the CAD geometry. It also makes it easy to determine the effects of interferences when they are not represented in the CAD model or for hand-built models.
A CAD assembly can be modeled with a net fit between the contacting parts. A hand-built assembly must be modeled with matched surfaces (net fit). In either case, a uniform interference can be manually specified within the Contact Options dialog box. In addition, the geometric interference, if any, in a CAD model can be overridden with a user-specified, uniform interference value.
Behaves like Separation / No Sliding contact but with initial interference between the contacting parts. Use this option when the intensity of fit and friction are great enough to prevent relative motion (sliding) between the contacting parts. The radial interference is specified automatically (CAD-based) or manually in the same manner as it is for Shrink Fit / Sliding contact (see above).