General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

Deviation between Ansys Bolt FEA Results and Analytical Solutions

• giorgino0907
Subscriber

Hi all, I'm currently assisting my colleague to solve a simple problem where I-beam and a plate are joined by 16 bolts (bolts at the 1st row from the bottom have a different diameter). The load and boundary condition can be seen below. The standard used for this case is EN 1993-1-8.

Problem Definition

Bolt Configuration

I modeled the bolts using beam elements and fixed joints applied to the beam vertex and plate bolt head-imprinted faces (MPC, Deformable Behavior).

The goal is to evaluate the Total Force Reaction for each bolt and compare it to the analytical solution using methods from Shigley's Mechanical Engineering Design book. However, the results look like this

Results

As we can see, most of the bolts' reaction forces calculated by Ansys have deviation, with a maximum deviation of 19% compared to the analytical calculation.

What causes these deviations? My colleague is confident with his analytical calculation (I already checked it) and he doesn't have experimental data. Does analytical calculation assume the objects to have rigid behaviors? How can I convince my colleague that the FEA model is already modeled correctly? Thanks!

• peteroznewman
Subscriber

The deviation between the ANSYS forces and the Shigley forces may be reduced if you make a few changes to the ANSYS model.

Change the diameter of the 14 mm bolts to 12 mm to match the other bolts.

Use an End Release on one end of each bolt so it does not carry any moments (forces only).

Make sure the bolt material is different from the I-beam and plate materials.

Edit the I-beam and plate material properties to increase the Young’s Modulus by a factor of 1000.

Please reply with results from these changes and show the new values of Deviation (%).

• Raihan Lutfianto
Subscriber

-

• giorgino0907
Subscriber

Thanks, Peter! I already did what you suggested and the results look like this (maximum deviation is 0.15%)

New Results

However, could you elaborate more on why do we need to apply those changes? Is it because Shigley assumes rigid structures? Or is it due to the analytical formula won’t work on the 12-14 mm bolts configuration (bolt diameters need to be the same values)?

Also, maybe you could give me some suggestions on how can we utilize FEA to evaluate bolt connections according to this EN 1993:1-8 standard. Thanks once again Peter.

• peteroznewman
Subscriber

Shigley's method uses only geometry, therefore the bolt hole location is constant so rigid materials better represent the method. Since Shigley uses only geometry, there is no weighting factor to account for different bolt diameters so making the bolts all equal better represents the method.

Shigley's method and the EN 1993:1-8 standard are useful for making design decisions, but an FEA model with the true material Young's modulus and the true bolt diameters creates forces that better represent reality.

• giorgino0907
Subscriber

I see, thanks a lot for your explanation Peter. In that case, the results from Ansys FEA model (with the true material properties and the true bolt diamaters) will never be the same/exact as the analytical solutions, right?

Again, since we don't have any experimental data for now, how can we become confident with the current FEA model?

• peteroznewman
Subscriber

For this example, the FEA model with true properties and diameters will not give the same forces as Shigley.

Shigley is still useful because there are many ways to make mistakes while building an Ansys model, so knowing what the correct answer is within 15% by a hand calculation allows you to find mistakes that result in a 100% or 1000% error in the Ansys model.

FEA models are validated against experimental data. Once you have a physical sample of a bolted joint, it is easy to apply a known load (most easily done by hanging known weights) and carefully measuring deflection. A discrepancy of 20% is a good result unless extraordinary care is taken to characterize the stiffness of the I-beam. One method is to extend the model past that cut plane and add the full length of the I-beam and the details of how that is bolted to a concrete foundation. With the Fixed Support on a close cut boundary, the deformation from the Ansys model will underpredict the actual tip deflection by a lot.