## General Mechanical

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

#### lap joint rivet Analysis

• Jack Cool
Subscriber

Kindly can you help me with solving rivet problems? how to define contacts? Etc

• Nanda Veralla
Ansys Employee

Hello Jack,

For a riveted lap joint, you can define contacts as below:

1. Frictional between two plates
2. Frictional between head and plate
3. Frictional between tail and plate
4. Frictional/frictionless between plate holes and shank

For more details on how Ansys contact definitions work, kindly refer to this link below:

Definition Settings (ansys.com)

Regards,

Nanda.

Guidelines for Posting on Ansys Learning Forum

How to access ANSYS help links

• Jack Cool
Subscriber

The thing is i want to analyze a simle lap joint with one rivet of 2mm shank that joins two metal plates of 215mm, 15mm, 2mm length, width , thickness repectively but i cannot validate it the stresses gets too high.

Secondly what if we define head to plate and tail to plate as bonded.

• Nanda Veralla
Ansys Employee

Hello Jack,

What are the loading conditions you're using? Does those stresses occur around any corner/sharp edges? Have a look at this video on dealing artificial high stress values.

Understanding and Dealing with Artificially High Stress Using Ansys Mechanical — Lesson 3 - YouTube

Regards,

Nanda

• Jack Cool
Subscriber

Thanks once again.

From one side i have frixed my model and the other side i Have inserted a load of 2058 N.

Should i use any other boundary condition in addition to this. Further more when i solve it with frictional contact it gives me error that deflections are too large.

Further more the max stress is in plate not the rivet.

In addition the shear stress results are not coinciding that of analytical one. Shear stress ansys in XZ plane is 205.5 Mpa and anlytical is 163Mpa using formula

• Nanda Veralla
Ansys Employee

I don't think, the head to plate and tail to plate should be bonded. It simply over-constraints the model. In reality, rivet head is hammered into plates, with certain amount of interference. Once the head is in position, tail is then formed in a die compressor. Frictional sliding is allowed but the shank stops the plates from moving.

Thanks,

Nanda

• Nanda Veralla
Ansys Employee

Hello Jack,

This message will be displayed any time the software detects nodal deformations exceeding 10% of the model diagonal. Exceeding 10% of this length suggests model mechanics that depart from linearity in response to the applied boundary conditions. Load magnitudes, surface body thicknesses, and contact options, if applicable, should be verified. If these are intended, a nonlinear analysis is advised. To request a nonlinear analysis, set Large Deflection to On in the Details view of the Analysis Settings folder.

Solver Controls (ansys.com)

Regards,

Nanda

• Nanda Veralla
Ansys Employee

The high amount of stress might be occuring around a sharp edge, you can refer to the video link above on how to deal with it. Let us know if that doesn't help

• Jack Cool
Subscriber

Should i make the edges smooth of rivet and plate contact even though in reality they are not in contact in that manner.

• Nanda Veralla
Ansys Employee

Hello Jack,

Instead of modifying the geometry, you can scope the results to areas of interest. Since, rivets are designed to fail in shear and excluding plate failures, most rivet failures occur on shank. You can scope the results to the face of the shank and use that data for comparsion with analytical data.

Regards