Bolt load problems

[Max1991]

Hi!

I'm quite new to Abaqus.

I'm trying to model a bolted assembly made of two rectangular flanges and the bolt itself (I merged the screw and the nut in a single part). I joined a pic of the assembly.

I defined surface to surface contact between the head of the screw/the nut and the flanges; between the flanges; between the screw and the hole.

I also use an encastre boundary condition on one of the flange (2 sides out of four are encastred).

I'm concerned by the results.

In my case, I'm using a M14 bolt with a preload of 50 000 N. The pretension alone makes the stress in my flanges higher than the yield limit (235 MPa). Usually there are peaks around 500 MPa (quite localized but still peaks). Any idea of what could be the origin of that? It seems excessive to me.

I wanted to try to apply the preload by adjusting the length of the bolt but I don't know how to convert the force into a length adjustment. Is there any way to know the force Abaqus applied to the bolt in order to modify it's length?

I would be so glad if someone could help me! Thank you!

 

[StefCon]

Hello,
Abaqus applies the displacement (contracts the bolt) until it reaches its goal. The force becomes whatever it needs to be. The force is dependent on the geometry and material stiffness.

You could measure the length of the bolt when you applied the force. The contraction can then be added as adjust length. You should end up with the same force again. I do not recommend doing this.

I found that calculating the bolted joint total stiffness with equations is highly inaccurate.

Calculate the force (50 kN) on the contact area and see what pressure you get. Peaks in contact pressure is to be expected. Finer mesh in the area might give you are more realistic picture of the contact. Surface smoothing option could also help.

Cheers!

 

[Max1991]

Hi Stefcon!

Thanks for the answer!

I tried with a finer mesh but still gets very high stress. Surface smoothing is already on as well.

In order to determine the force applied to the bolt when adjusting the length, I thought about verifying the reaction forces (RF) at the pre-tension node. What do you think of this?

 

[StefCon]

Hello again,
Are you modelling the bolt with solid elements?
Is the material data elastic only?

In order to determine the force applied to the bolt when adjusting the length, I thought about verifying the reaction forces (RF) at the pre-tension node. What do you think of this?

If that is what you want to do then I think it is a good approach. I myself don't know how to probe the pre-tension node. I am a big fan NFORC (nodal forces) for checking cross section forces (solid elements).

Cheers!

 

[Max1991]

Thanks again for the answer!

Yes I'm using solid elements and the elastic material properties only.

 

[Max1991]

Hi!

I still have some interrogations regarding this problem.

I tried to apply a bolt preload in a case where the hole diameter is bigger than the diameter of the screw.

The program doesn't converge and exits with an error.

I have read that I should apply some temporary boundary conditions while applying the preload.

I have no idea what kind of conditions I should apply though. Could someone help me?

Thanks!

 

[StefCon]

Hi,
Is this the same kind of geometry (bolt+nut) as before? In that case the hole should be bigger than the screw (not a threaded hole).

I used to apply one displacement BC to each bolt (screw head or nut). I usually fixed the translation degrees of freedom (pinned). The reason for not using the "pinned" BC is just overall flexibility in case I would need it later.

Since your model has 3 parts, I recommend using 3 BC's. Apply a bolt contraction until you have established contact between all components (CSTATUS), then you switch to applying bolt force. After that you release the boundary conditions you don't want in the final analysis (bolt BC being one of them + one plate maybe). Make an additional step where you fix bolt at current length and you are ready to apply the "real" loads.

Note that if you switch to an elastic-plastic material model you have to be careful so that you do not deform your components in some unrealistic way.

Good luck!