Strange stress in the bolts and bolt region

  • Last Post 10 March 2020
jbarc posted this 04 March 2020

Hey, I am simulating the connection of a structure that is being pulled by a chain, according to the drawing


This connection is attached to the rest of the structure (square body) by the bolts. However, I am having some problems with the results. Some of the stresses are very high and do not seem proper. I simulate this case with a fine mesh (element sizes in the bolted contact region were 4x smaller than the pitch distance) and here are some of the results that I got.

Since the stresses are so concentrated in a very specific reason, I am doubting these results. Is someone already experience something similar?  

P.S.: Since the simulation with the bolted case takes so long due to the mesh refinement requirement, I also attached the project with a more coarse mesh and with bonded contacts. The results look similar


Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 05 March 2020

The U-shaped link on top looks like it should have a degree of freedom to rotate about the pins. Does it stand up straight when it is pulled sideways?

Also, does the collar, which has the pins that support the U-shaped link, have a degree of freedom to rotate about the bolt?

jbarc posted this 05 March 2020


No it does not stand up straight. You are correct. The U-shaped link should have a degree of freedom so it could rotate, but the other body that you mentioned stays still mainly due to the pressure of the bolt.

I even though about putting a joint in the U-shaped link, but I am not sure if is the best approach. What would you suggest?

peteroznewman posted this 05 March 2020

In CAD, rotate the U-shaped link to align with the direction of the applied force. If there is clearance between the hole and the pin, then move the U-shaped link along the line of force until the hole and pin are tangent on the opposite side of the hole from the direction of the force.

In Mechanical, change the Bonded Contact between the holes in the U-shaped link and the pins in the holes to Frictional Contact. Under the Connections folder, insert a Contact Tool and Generate Initial Contact Status.  The Frictional Contact must be closed before you start the simulation.

jbarc posted this 05 March 2020

All the contacts are closed in the simulation. I checked that, but I will also put a picture of the contact tool as soon as I can.

I will adjust the U-shaped link as well, but looking at the problem I could see that the source of the big stress in the middle bolt (biggest) is coming from the contact with the U-shaped link I think. The edge is pressing in the bolt and creating the big stress region, which would be higher than the yield stress. This stress in my opinion is too high and it might be a problem in the connection of these two bodies during the simulation 

jbarc posted this 06 March 2020

Peter, here are the results. 

As is possible to see, all the contacts are closed. However, if I define the connection between the hook and the other geometry to frictional, then the hook and the round body that it is attached they end up separating. So the connection between the hook and the round part was defined as bonded, which I think is fine because I am more interested in the stresses in the other parts of the simulations, such as the round base and the bolts. Then, with the bonded contact, these are the results. Then, as is possible to see, the connection of the small bolts and the round base are near open, which makes sense since there is a difference between these diameters. I simulated like this, just to see what would happen, and ansys was not seeing the small bolts as a constrain. The round base was moving in the X-Y direction, passing the bolts, which I though it was very strange.

This is a little strange. I change the penetration value to prevent this to happen, but now I am curious to know why this was happening. This problem only stops when I change the contact to adjust to touch, but then the bolts are very distorted because these two bodies are not suppose to keep touching always. Maybe it would be better to not define any contact in that region, but maybe you have a better input on that.




Any how, the stress is still a little higher then I would expect in the bolts. I would like to have more certain on this before simulating with a fine mesh (fine enough for the pitch distance).

I am uploading a case with a simplified mesh in case you want to take a look

Attached Files

jbarc posted this 06 March 2020

In addition, I did a simulation with no force, just the pretension of the bolts, and it resulted in some high stress points in some locations of the bolts. I am wondering if this is not a problem with the contact interface and the contact mesh. 

jbarc posted this 10 March 2020

I realized that the problem that were happens in the bolts were purely geometric. When the drawing was done in CAD and the constrains were introduced, everything seamed fine, but when the geometry is imported to ANSYS, then there is small interference between the bolts and the wholes, causing that large stress. Then, it was better to remove the small bolts and continue only with the large/main one. I will redo that geometry inside ANSYS to see if that problem still persists, but for now, with the simulation only with the main bolt in the geometry, the big stresses do not occur anymore. However, I am now facing a problem, which I am suspecting is a mesh singularity problem.