Table of contents
The Simplified Bolts is a load feature where so-called “Simplified bolts” are created and placed in a group folder in the current structural (or thermal) analysis. The Simplified Bolt is constructed of two BEAM188 solid circular for the bolt shaft and a CERIG or RBE3 remote points for the head and nut/thread. In thermal analysis LINK33 is used. This is similar as the standard Beam connections in Mechanical.
The additional features with the Simplified Bolts compared to “Beam connection” are that:
- All Simplified bolts are saved in one place, the “Simplified Bolts Group” folder.
- Multiple bolts can be defined in one load object, i.e. all M12 bolts of the model.
- A point mass (MASS21 element) can be added to the bolt head to account for missing mass.
- Pretension can be automatically calculated based on selected bolt code, material and shaft diameter.
- Custom Behavior for the “head” and “thread” interaction can be defined in an APDL macro.
- Thermal loads on the bodies will be mapped to the bolts to account for correct thermal elongation.
- Post processing of the Simplified bolts is done using the Bolts Strength or Bolts Fatigue object.
Click on “Simplified Bolts” in the toolbar to insert the Simplified Bolts Group folder in the current static analysis as well as creating the first Simplified Bolts load object.
To add additional bolts, right click on the Simplified Bolts Group folder and select “Add Simplified Bolts” or click on “Simplified Bolts” in the toolbar again. You can also use “Duplicate” on an existing Simplified Bolts and modify the properties.
There is also an option Simplified Bolts to Ground used to connect a body to ground, e.g. when using compression only support.
Inputs to define the Simplified Bolts and Simplified Bolt to Ground are:
|Geometry Selection/Named Selection
|Planar circular or conical faces OR edges connected to non-cylindrical faces. (i)
|Geometry Selection/Named Selection
|Planar circular or conical faces OR edges connected to non-cylindrical faces (Nut) OR cylindrical faces (Thread). (i)
|Select material from “Engineering Data” or app default materials.
|No (Default)/Yes. Use plasticity models defined in the selected material (ii)
|Bolt shaft diameter that defines the circular solid section for the beam element.
|Sets the maximum size of the bolt head and nut in case of edge selection. If using a surface selection, make sure that the diameter is equal or larger than the face diameter.
|Length of bolt shaft. Only visible for Bolts to Ground.
|Add the missing mass (optional).
|Head Node Position
|Head node offset factor relative to hole plane. Offset = Factor*Shaft Diameter
|Thread Node Position
|Thread node relative position 0: Beginning, 0.5: Middle (default) 1: End
|Thread engaging length symmetric around the thread node. (If 0 use full thread)
|Pretension from Code
|Select a code to get the recommended pretension force based on Shaft Diameter and Material. Default “None”.
|Initial bolt force. If zero, the pretension section is locked.
|Pretension adjustment increment. If Increment > 0 force increase. (iii)
|Load Step Apply
|Load step to apply the pretension force. Used only if Pretension Force > 0. (iv)
|Load Step Lock
|Load step to lock the bolt adjustment. (v)
|Load Step Increment
|Load step to add the Increment (Embedding). Used only if Increment ≠ 0.
|PRETS179/MPC184. Use MPC184 if there is large deformations or rotations.
|Contact Slip Radius
|Radius used for normal and slip contact force summation. (vi)
Both shell and solid bodies are supported. The bolts can have different orientation and the pretension normal will be set for each individual bolt. The head and nut/thread must have equal number of selected entities and also one unique match between head and nut. It is not allowed to have two bolt heads connecting to the same thread. This will be shown as invalid thread selection. Virtual Topology or External Models (faceted geometry) is not supported.
The following material properties (and corresponding MAPDL MP Lab) are supported: Young’s Modulus (EX), Poisson’s Ratio (NUXY), Density (DENS), Coefficient of Thermal Expansion (ALPX), Thermal Conductivity, (KXX), Specific Heat (C), Isotropic Hardening (BISO & MISO), Kinematic Hardening (BKIN, KINH). If orthotropic properties are defined the X component is automatically used (EX, NUXY, ALPX & KXX). The Bolts Pretension can be used in a thermal analysis to apply the bolt material. The pretension settings are ignored in this case.
(iii) Increment (Embedding)
You may use Increment (Embedding) as “Preadjustment” if Pretension Force = 0 and Load Step Increment = 1.
(iv) Load Step Apply
The Load Steps may be defined as a “series” to define a sequential bolt pretension.
(v) Load Step Lock All inputs are checked to be valid to avoid error during solution, i.e. the analysis must have at least two load steps to use the Pretension Force and Lock and two or three load steps if also using the Increment. You can use the Pretension Force and only one load step if you set Load Step Apply = 1 and Load Step Lock = 2.
(vi) Contact Slip Radius
The Head Diameter is used as default radius. The solution is not invalidated if changed but a solved bolt result object must be cleared and re-evaluated to see the changes in contact normal and slip force.
A property file is also written to the solver files directory that is used by the Bolt Report feature.
A graphic representation is created once valid inputs are given. The Simplified Bolts load object searches to connect the head and nut with the minimum distance. The head geometry is plotted in red and the nut/thread in blue. The head and nut diameter are plotted as a green disc (normal to the bolt shaft) and the bolt shaft as a green line. If the Thread Length is given turquoise circles are plotted to indicate the thread engagement. The Contact Slip Radius is plotted as a purple circle at the mid of the bolt shaft.
The bolt Id number is printed at the center of each bolt head. This number is used in the result tables. The printing of Id number can be turned on/off in the Bolt Settings object (or preference file “showBoltId = False”).
The head centroid (and disc) is adjusted to be on the axis from the corresponding thread/nut. If selecting non-matching head and thread geometry the app may still create valid bolts if the bolt head plane is the same.
The Simplified Bolts connection behavior is defined in the macro file “simpleBolt.mac” found in the extension installation folder. (%AppData%\Ansys\v22X\ACT\extensions\BoltToolkit_V22X)
Edit the file in the sections “*else ! ‘Custom’” to define any type of connections using the center node on the bolt shaft (_npilot) and the selected edge nodes.
The Simplified Bolts to Ground works in the same way as the “Beam Body-Ground”. Based on the Bolt Head scoping and Bolt Length bolts are created and pretension force can be applied just as for the standard Simplified Bolts. In a structural analysis the end of the bolt is locked in all degrees of freedom.
In both structural and thermal analyses, the environment (or initial) temperature is applied to the fixed end of the bolt and the temperature will be interpolated along the bolt shaft.
Using Rivets or Simplified bolts will add beam elements to the FE-model. This will influence the moment convergence. Using the default setting “Program Controlled” for Moment Convergence in Analysis Settings/Nonlinear Controls may result in long solution time or un-converged solutions for certain types of models and loads.
Review the Solution Output: “Force Convergence” and “Moment Convergence” for the first pretension step to find the convergence criteria value “Force Criteria” and “Moment Criteria”.
If the “Moment Criteria” drops to a very low value for load step two and up and the solution struggle to converge you may assign a manual value. See the red ring in the plot!
Assign Moment Convergence “On” and set the “Value” and “Tolerance” for all load steps to have manual criteria. The “criteria” is defined from “Value*Tolerance”. In this case Value = 20000 and Tolerance = 1% gave a similar convergence behavior for both Force and Moment.
Tip: Click on “Analysis Settings” and then “Worksheet” button to review settings for all load steps.
If using an upstream thermal analysis linked to the structural analysis with “Imported Body Temperatures” and/or “Thermal Condition” the temperatures will be automatically mapped to the rivet and bolts. Temperatures will be interpolated over the bolt using the head and thread/nut temperatures.
If using a mix of imported and thermal conditions, like in the figure below, each part of the bolt/rivet will have constant temperature based on its connected part. For a solid bolt the entire bolt will have constant temperature up to the pretension split based on the connected parts thermal condition at the bolt head and thread respectively.
Detail of mapped temperatures with interpolated temperatures on the advanced bolts.