Home / Featured / An Overview of Methods for Modelling Bolts in ANSYS

An Overview of Methods for Modelling Bolts in ANSYS

Bolted joints are commonly used to assemble mechanical structures. Modelling bolts for three-dimensional finite element applications has always been a tricky proposition because the details of bolt geometric features usually result in large model size and high computational cost. Therefore, efficient methods to model bolts are always desirable.

 

The approach to modelling bolts usually involves undertaking the following:

  • Prepare geometry: bolt and associated components
  • Mesh: Minimum DOF for best representation/ Hex or Tet
  • Contact: load transfer/stress
  • Load definition:

–        Step 1: Apply bolt pretension load

–        Step 2: Lock the defined bolt pretension load

–        Step 3: Apply in-service loads to structures

How one prepares the bolt geometry is an essential factor that will influence the subsequent modelling techniques including meshing, contact and analysis settings. This blog summarises eight methods for modelling bolts in ANSYS 15.0. A simple eight-bolt flange model is used for assessing the different methods.

Image_1

 

 

 

 

 

 

 

 

 

 

 

Bolt Model 1:

  • Full thread on bolt and nut are modelled;
  • Good geometric representation of stiffness if mesh is fine enough;
  • Tetrahedral mesh would normally be produced, the element quality on threads need to be check carefully, fine mesh needs to be used on the threads
  • Contact between bolt and flange, nut and bolt are defined as any contact type aside from bonded;

Image_2Image_3Image_4

 

 

 

 

 

 

 

 

 

 

Bolt Model 2:

  • Threads on bolt and nut are removed;
  • The removal of thread could influence the bolt stiffness subjected to loadings;
  • Tetrahedral mesh are used, similar to Bolt Model 1, but less mesh on thread region can be obtained;
  • Contact between bolt and flange, nut and bolt are defined as any contact type aside from bonded.

Image_5Image_6Image_7

 

 

 

 

 

 

 

 

 

 

Bolt Model 3:

  • Threads on bolt and nut are removed, similar to Bolt Model 2.
  • New bolt thread contact technique in ANSYS 15.0 is applied to define the contact between bolt and nut. This contact method defines all of the thread characteristics. The computational cost for getting similar stresses in thread region is reduced by a factor of 10 compared to Bolt Model 1;
  • Tetrahedral elements are used, similar to Bolt Model 1; use contact sizing to increase number of elements in thread area.
  • Contact between bolt and flange, nut and bolt are defined as bonded with asymmetric behaviour.

Image_8Image_9Image_10

 

 

 

 

 

 

 

 

 

 

Image_11

 

 

 

 

 

 

 

 

 

 

Bolt Model 4:

  • The bolt and nut are defeatured and sliced to be sweepable bodies;
  • Better mesh controls can be applied to generate hex mesh.
  • New bolt thread contact technique in ANSYS 15.0 is applied to model the contact between bolt and nut, similar to Bolt Model 3 (recommended 4 elements span 1 thread width).
  • Contact between bolt and flange, nut and bolt are defined as bonded with asymmetric behaviour.

Image_12Image_13Image_14

 

 

 

 

 

 

 

 

 

 

Bolt Model 5:

  • Geometry is same as Bolt Model 4;
  • Bolt thread contact between bolt and nut is replaced by a cylindrical joint
  • APDL command is inserted to redefine joint as a crew joint
  • Contact between bolt and flange as bonded with asymmetric behaviour.

Image_15Image_16

 

 

 

 

 

 

 

 

 

 

Image_17

 

 

 

 

Bolt Model 6:

  • Bolt joint is simplified and modelled as line body;
  • Cylindrical surfaces are imprinted on both upper and lower flange to simulate contact regions;
  • Bonded contact (MPC) used to attach cylindrical contact region with ends of line body
  • Line body meshed as beam elements, hence reducing model size significantly;
  • However, the details of the stress of the bolt joint would not be available.

Image_18Image_19Image_20

 

 

 

 

 

 

 

 

 

 

Bolt Model 7:

  • Bolt joint is simplified and modelled as line body, similar to Bolt Model 6.
  • No cylindrical faces are imported on the flanges.
  • Bonded contact (MPC) used to define contact between ends of line body and cylindrical edges of the bolt holes. Pinball radius should be big enough to include the cylindrical edges;
  • The details of the stress of the bolt joint might not be avaiable, similar to Bolt Model 6.

Image_21Image_22

 

 

 

 

 

 

 

 

 

 

Bolt Model 8:

  • Use Body-Body > beam connector to simulate the bolt joint; No bolt/nut geomerty required;
  • Single beam 188 element created between mobile/reference geometry;
  • Scope to edge or surface of bolt holes on flanges to generate beam connector;
  • This method cannot use bolt-pretension load directly. APDL command needs to be inserted to define the initial stress/strain induced by the bolt force.

Image_23Image_24Image_25

 

 

 

 

 

 

 

 

 

 

Apply Bolt Pretension Load

In the example, the bolt pretension load (500N) will be applied to bolt models except the Bolt Model 8. Select bolt shank surface (solid bolt) or edge (line bolt) to apply the load

Image_26

 

 

 

 

 

Two load steps are required: first load step is to apply the pretension load, second is to lock the load.

Image_27

 

 

 

 

 

 

 

Image_28

 

 

 

Result Comparison:

The deflection of the top flange is consistent irrespective of how bolt has been modelled.

Image_29Image_30

 

 

 

 

 

 

 

 

Total deformation is also axisymmetric irrespective of bolt modelling methods

Image_31

 

 

 

 

 

 

 

 

 

The first five bolt models (solid geometry) has predicted similar stress along the bolt shank, around 25MPa. The stress level from hand calculation is 25.6MPa (500N/19.537mm2), less than 3% difference.

Image_32

 

 

 

 

 

 

 

For the bolts modelled as line body, the stress in bolt shank is about 25.5MPa. (Post process using “Beam Tool”)

Image_33Image_34

 

 

 

 

 

 

 

For the beam connector, using APDL commands to post process the stress result. The magnitude is about 25.4MPa.

Image_35

 

 

 

 

 

 

 

In conclusion, users should think carefully before taking the decision on which method should be employed to model the bolt joints. In general, if the behaviour of the whole assembly is of interest, not details of stresses level in the bolt joints, the line bodies/beam connectors would be a better option as this can significantly reduce your model size.

If you need to understand the contact status between the bolt and flange and stresses, solid modelling is recommended, however some additional geometry preparation and mesh control are required. The bolt thread contact technique in ANSYS 15.0 would be highly recommended to minimise the model size and computational time.

There will be another following blog introducing more details of the bolt thread contact technique in ANSYS 15.0.

 

Leave a Reply

Your email address will not be published. Required fields are marked *