Bolt analysis in Abaqus CAE 1

[Megabeast]

Hi,
I am quite new to Abaqus CAE and I am doing bolt analysis for the first time. I want to calculate bolt preload. I have a solid model with two flanges, bolt, washers and nut as seen in Figure 1.

I used contact surface to surface between the washer and flange, bolt and washer, between the two flanges, washer and nut and between the bolt shank and the bolt hole in the flanges.
The analysis failed to converge due to too many iterations tried.
It gives these warnings: Displacement increment for contact is too big and Numerical instability while processing nodes.
I reduced the time step and also specified tolerance for adjustment zone for contacts. It does not to converge. Could anyone please help me with this? I have applied bolt load at the middle of the bolt.

Also, I tried another method after referring to a report. Bolt was represented as beam elements and used kinematic coupling that extended from bolt centreline to a distance on the flange (equal to washer radius) was used to represent washers. I had to trim the flange surface to the radius of the washers to be able to select that surface for applying kinematic coupling. To trim the surface, I first created a datum plane and then drew a circle and projected that cuve on the flange and used partition face option to create a partition.
Now, I cannot deleted the features I have used to create partition and when I mesh my model, even the curve used to create a partition which is lying on the datum plane is also meshed. Is there a better way to trim surface of a part in CAE?

Contact surface to surface was used between the two flanges and with this method (Figure 2), it complained of distorted elements.
Any hint will be of great help.
Thank you!

 

[OrlandoTaddeo87]

Hi!

first of all, it's not necessary to define manually the pairs of surfaces that can be in contact.
Moreover, you can use the first 3D model of the bolt, it should work.
Follow these steps and let me know if the analysis will end correctly.

1) During the "geometric definition" of the model, be sure that the various parts of the bolt (shank, head and nut) are tied together (or better, the head and the nut must be tied to the shank), or that they are in the same "part".

2)be sure that the whole model is correctly constrained.

3)In the "interaction" module, define a new "interaction property"; for example, I usually use "penalty" contact for the tangential behaviour and "hard contact" for normal behaviour.

4) in the "interaction" module, define a new "interaction", and choose "general contact"; Abaqus will automatically find the contact pairs that can be in contact during the analysis. choose the "interaction property" that you have previously created.

3) apply the bolt pretension, and be sure that the force "pushes" the bolt, and not "stretches" it (the sign of the load is important).

Good luck!
Orlando

 

[OrlandoTaddeo87]

PS

In the "job" module, open the "job manager" and click "submit". After this, click "monitor", to monitor the process and see in which step the program has "troubles" to solve the problem

 

[corus]

Numerical instability sounds like its not restrained properly. Distorted elements sounds like you've used tetrahedral elements too as they tend to cause that kind of problem. Switch to hex elements even if that means simplifying the geometry, such as the bolt head. Looking at the geometry it appears that the flanges are in contact just at one edge. Try and make sure your contact surfaces extend beyond that edge just in case nodes fall off the contact surface. Don't use general contact as that'll be expensive to run. In the 1st step just have the bolt preload and in the 2nd step fix the length of the bolt and remove the bolt preload. There is an example of bolt preload in the manual. Have a look at that to see how they've done it.

 

[Mustaine3]

It is hard to recommend something, when the exact reason for the problem is not clear. Maybe you can attach the cae-file.

The two most common mistakes with bolt loads are:
1. There are rigid body motions in the model. Check all contacts, tie some parts togehther (flange vs. nut, e.g.) and check BC.
2. The bolt load acts in the wrong directions. To check that, switch bolt load from "force" to "displacement". When this is running, look at the results and check if the bolt gets longer or smaller. This tells you, if you have to apply the force/displacement positive or negative. Sometimes the displayed icons in the Load-module are not correct and mislead user regarding this decision.

 

[Megabeast]

Hi All,

Thanks a lot for finding time and replying back
My apologies to be replying late as I am parallely working on another project and still exploring CAE features.
OrlandoTaddeo87: I have now modeled bolt,nut and also the washers in the same part. Then used general contact as you suggested. It still fails to converge and gives the same warning displacement increment for contact is too big.And the bolt should be in tension right, why do you say the force should push the bolt, and not stretch it.
Corus: I am going to try with hex elements and surface contact now. Yes, the flanges are in contact in just one edge. I am interested in knowing how much preload is required to close the gap.
Mustaine3: I am fixing 3 dof at the bottom flange. Contacts have friction in Abaqus so it should stop the bolt from rotating about its axis. I will run an analysis with displacement instead of force.

Thanks again!

Have a nice day.

Regards,
Divya

 

[OrlandoTaddeo87]

Hi Megabeast!

I intended that the preload should determine a curtailment of the bolt, and not an elongation of it.
I said it because, the very first time I used the bolt preload, I used an uncorrect sign of the load, and it can be a common error for new users.

If I can give an advice, try to remove the bolt and to apply a pressure on both the flanges on an area that is equal to the surfaces of the bolt in contact with them; you can subdivide the parts and obtain circular surfaces on which apply the pressure. This can be helpful just to understand if the problem is the bolt or the flanges. The flanges should "touch" each other for a certain value of the load.

Orlando