The Multi-Gear Shaft feature enables you to model complex gear trains in high level of fidelity for various NVH studies in Adams View and Adams Car environment. It enables you to create a shaft flexible body consisting of one or more cylindrical gear and one or more involute spline elements along with gear tooth flexibility for accurate gear contact simulations. The Multi-Gear Shaft feature removes some of the previous limitations of Full Flex Gear modeling for cylindrical gears.

This section provides a brief overview of the modeling steps in Adams environment which are specific to this modeling approach. It also describes in more detail all the preprocessing steps to get required model files ready for building Adams model with a flexible shaft and wheel body consisting of multiple cylindrical gears and involute spline elements with use of Full Flex Gear and Full Flex Spline modeling approach, respectively. In current release there is no support for bevel / hypoid, cylindrical worm, and lead-screw gears.

 

Preprocessing starts by opening Multi-Gear Shaft FE Preprocessing dialog box and browsing for shaft / wheel body FE mesh (*.BDF file) prepared by user - see Figure 79 and Figure 80

The Gear AT Mesher writes additional gear rim bulk data files per cylindrical gear and involute spline element and one Nastran input deck for SOL103. The input deck references all bulk data files by INCLUDE statement and it includes all pertinent glue contact cards to define connections of dissimilar FE meshes of the shaft / wheel body and gear rims. To make glue contact connection, you need to ensure the common surfaces of a glue contact pair is within tolerance of 0.05 mm by consistent value of a gear Rim Diameter – see Figure 83.

After the preprocessing is complete, an MNF file will be used to create a new flexible body in Adams model. You need to make it part of your model by positioning / orienting and attaching it to other bodies as appropriate or replace existing rigid body with the new flexible body.

The flexible body's local body reference frame (LBRF) corresponds to the origin of the FE structure which is transformed by Gear AT Mesher to coincide with attachment node of the first gear element and the Z axis is aligned with the shaft rotational axis.

When connecting the flexible shaft to your model be advised to parametrize I and J markers of all joints and bushings so it does not get broken during subsequent orientation of the flex body during a gear force creation.

Create cylindrical gear and involute spline elements by selecting interface markers of the shaft flexible body. It is assumed that you have preprocessed each gear for the use with so called Flexible Tooth modeling approach hence there are stiffness files (*.CGS and *.ISS) available for gear force creation.

The last step is to create all relevant cylindrical gear forces and involute spline forces between gear elements attached to adjoining shafts. Be aware that one of the flexible shaft bodies is automatically oriented relative to the other to set up proper gear meshing. In case of complex gear trains the sequence of gear force creations hence orientation has to be considered appropriately. However, the orientation of a shaft can be reset afterwards and new orientation can be set up without need to recreate a gear force – read section New Gear AT Force for more information.

The tab options of Multi-Gear Shaft dialog box are following:

 

You need to provide FE model of a shaft and wheel body which are usually connected by permanent glued contact in Nastran SOL103. Most of times contact bodies are defined by BSURF (MSC Apex) which is defined by IDs of elements. Gear rims are not modelled by user but by Gear AT Mesher.

Gear AT Mesher creates all glued contact related cards to:

It is good practice to always verify flex body after importing to Adams View. Especially check the flexible body mass and make sure that the first 6 frequencies are very close to 0.0 Hz (rigid body modes) and ensure that all these rigid body modes are disabled. In case there are 12 rigid body modes, the glue contact failed most probably due to higher distance between wheel body and toothed rim FE structures than the ERROR specified in a *_SOL103.bdf file. If the value of tolerance is not appropriate you can manually edit the input deck before running SOL103; search for ERROR keyword in BCONPRG Nastran card. Additionally there are some useful Nastran statements written in case control section of a *_SOL103.bdf file, which you might find helpful in troubleshooting some issues with glued contact such as plotting contact status or debugging glued contact grounding issues. Those statements are commented out but you can uncomment it before running Nastran SOL103 only preprocessor. Please read Nastran documentation to learn more about those Nastran statements.

 

Gear AT Mesher writes Nastran input deck for SOL103, which references all bulk data files by INCLUDE statement. Therefore the shaft input deck provided by user must not contain executive control section, case control section and following Nastran cards and delimiters:

Most of the non-required Nastran cards are automatically commented out right after browsing the Shaft Input Deck file so you do not have to edit the file manually. The original Shaft Input Deck file provided by the user is preserved with the BDF% extension. However in case the Gear AT Mesher preprocessing or Nastran SOL103 is failing you need to check if the Shaft Input Deck file is properly cleaned up.

Currently there are following prerequisites for the user FE model of the shaft / wheel body:

The Shaft Input Deck file could consist of several FE meshes glued together. Gear AT Mesher will accept those already defined and will create additional glue contact per gear rim by BCBODY1 with BCPROP card. The BCPROP internally creates BSURF with all elements of FE mesh with defined PSOLID ID. In case any user defined contact body contains the same elements, Nastran SOL103 will write following warning into *_SOL103.f06 file, which can be safely disregarded:

unless following fatal message is present:

which means that the contact body defined by Gear AT Mesher contains no FE elements since all have been assigned to user defined contact body. To resolve that conflict, you have to redefine the contact body by selecting just those elements corresponding to assumed contact face rather than complete shaft / wheel body solid, hence the BSURF of user defined contact body will not contain of all elements – see bottom part of Figure 85

The parameters of the general tab give you the possibility to control modal content of the shaft flexible body. It also helps to align shaft rotational axis so the Gear AT Mesher pre-requisite is fulfilled.

 

 

Maximum Frequency: The value defines upper limit for frequency range of interest for fixed boundary normal modes extraction during SOL103 solution process. It corresponds to V2 parameter of EIGRL card – for more information read Nastran documentation.

Number of modes: Enter appropriate number of fixed boundary normal modes (also known as component dynamic modes) to define sufficiently large modal basis of your shaft / wheel body. It corresponds to ND parameter of EIGRL card – for more information read the Nastran documentation. Note that the default value of 10 will be most probably insufficient to capture real deformations of the flexible wheel body structure.

Structural Damping: The value defines structural damping in the form of percentage of modal deformation for given mode. This damping is in contrast to modal damping proportional to deformation. The damping matrix is generated and stored in MNF file of the shaft / wheel body assembly.

Axis of Rotation: The shaft / wheel body FE model gets transformed by Gear AT Mesher:

Fill up the table to define topology of the shaft / wheel body and related gears as well as FE mesh division of the gear rims.

 

Node ID: It defines the ID of attachment node (Nastran GRID card ID) per gear element to which appropriate toothed rim FE mesh will be located in assembled FE model. The option menu is populated by every node of RBE2 and RBE3 element found in the Shaft Input Deck BDF file.

The FE structure is transformed by Gear AT Mesher to coincide with attachment node of the first gear element in the table and the Z axis is aligned with the shaft rotational axis.

Mesh Density: It defines the number of finite elements along the involute curve of tooth profile – see Figure 90. Valid input entries for mesh density are 0 to 5, representing 8, 16, 24, 32, 40 or 48 elements along the contact line. For the Full Flex modeling, the value of 0 provides sufficient FE mesh resolution to capture flexibility of the gear rim.

Axial Divisions: It defines division of the tooth width into a number of equidistant sections in lead direction of a tooth flank.

It is suggested to use a number which is a multiple of 3. A default value is 12 axial divisions.

To make flexible shaft body a part of your model, you need to connect it to elements in your model by use of kinematic or flexible connections and apply forces to it. To learn more about the rules, best practices, and limitations, refer Connecting Flexible Bodies to Your Model.

To capture the effects of attachments on the flexible body the modal basis also needs to include so called constraint modes (boundary DOF). This is achieved by usage of RBE2 and RBE3 elements and promoting its reference node to be so called attachment or interface node by ASET1 Nastran card. You also need to define attachment degrees of freedom in Nastran SOL103 analysis set which are defined in the new FE basic system, where X-axis and Y-axis are normal to the shaft axis of rotation and Z-axis coincides with rotational axis – see Figure 87.

The table in Shaft Body Attachment tab is automatically populated by all reference grids of RBE2, RBE3 and ASET cards found in the Shaft Input Deck you provided however it could be expanded and edited appropriately.

 

Number of Nodes: Before executing Nastran SOL103 you need to define attachment nodes of all gears of the shaft including all shaft supports (bearings) and coupling connections (also known as interface node) which will be written in the MNF file and can be used to connect the flexible body to other parts and elements of your Adams model. When you create a Full Flex Gear element in your Adams model, you select reference marker on the flexible shaft / wheel body to attach the gear element to. Gear AT creates for you an appropriate constraint to attach gear element to the part which takes all 6 DoF. To capture the effects of applied load on the flexible body, the modal basis also needs to include so called constraint modes accompanied to that reference marker. Therefore the reference marker should be connected to so called attachment (interface) node.

Node ID: Enter the node id of each flexible shaft / wheel body attachment. This node could belong either to RBE2 or RBE3 element. In order to avoid the use of “PARAM, AUTOMSET, YES” which is required for defining ASET with attachment nodes belonging to RBE3 element, there is CBUSH element created per attachment node along with coincident node which becomes so called interface node in Adams.

Therefore, you will find a different ID of the interface node in Adams than specified in this table cell.

ASET DoF: Enter the degree of freedom (DoF) per attachment node of your flexible shaft / wheel body FE model. When you build a flexible body into an Adams model, you interface with the body using a variety of attachments, either joints or forces. In Adams Flex, you can model the variable boundary conditions at attachment points, which are nodes that have been idealized for attachment, by preserving all six Cartesian degrees of freedom (DoFs) of those points as you export the flexible body from your finite element analysis (FEA) program. An attachment point is equivalent to a super-element exterior grid point. Each attachment point normally contributes six modal DOF. Corresponding to each attachment point DOF is one constraint mode, which is a static mode shape due to a unit displacement of that DOF while holding all other DOFs of all attachment points fixed. A large number of attachment points can result in unwieldy data files and can significantly impact CPU time, if the associated modes are enabled during an Adams dynamic simulation. It is advised to limit the number of constraint modes by prescribing adequate DoFs per attachment node. For instance, if you intend to model spherical joint, it is enough to preserve translational DoF for the ASET (123). However, the ASET for attachment of the gear element to a shaft should always preserve all DoFs (123456).