Using ABAQUS to model the process of pipe expansion 1

[flycloud]

I wan to use ABAQUS to model the following process of expanding a steel pipe. I am not sure if this is a right problem to ask here. Since I am new to ABAQUS and need some results for this problem soon, I really appreciate if someone could help me to get started. Thank you very much in advance. I am also a new member of this Eng-Tips.

A steel cone with a 7.79" diameter (a rigid body) is pushed through a 10 ft long round pipe which has an inner diameter of 6.875", outer diameter of 7.625", and wall thickness of 0.375". Due to the plastic deformation, the inner diameter of the pipe will be enlarged to 7.79" after the process. I am particularly interested in calculating the residual stresses.

My questions are the following:

1. Since this is a highly nonlinear and dynamic problem, is this problem better handled by using ABAQUS?

2. Which geometric model should I use? Axisymmetric 2D model or a full 3D model?

3. Which element type should I use? Under axisymmetric 2D solid element category or under 3D solid element category? Specifically, which element in particular best fits here?

4. How to generate mesh? automatically or manually? What is the best mesh density?

5. How to add this dynamic load at the bottom of the cone so that at a certain value, the cone will be pushed hard enough to start to move along the pipe?

6. Finally, are there any other things that I need to pay attention to?

Thank you very much for your time and appreciate your help.

 

[Amir4deh]

Dear flycloud
Further to your questions:

1.Since you have nonlinearity and contact, this problem is very much suited for an ABAQUS analysis, especially ABAQUS/Explicit.

2.The geometric model depends on yourself, but I'll go for the axisymmetric: you can save a lot of modelling effort and CPU resources. Usually with the same effort, you could get much more accurate results from an axisymmetric modelling.

3.The common belief is that for contact problems, linear elements are preferred to the quadratic ones. So I would go for a 4-noded axisymmetrical element for your pipe and rigid elements for the cone. But you need more than one element through the thickness of the pipe. (say at least 4 elements).

4.Mesh generation method is a matter of taste: I alaways generate them manually. I would say start with 4 elements in the thickness direction for the pipe and compare the results with the case using 8 elements (so you need 2 analyses, at least)

5. In your question you haven't mention anything about the dynamic load. But if you apply a certain displacement in a certain time duration to your cone, you don't need to worry about the rest. The cone will move by the defined distance. You should define your contact surfaces by *SURFACE and the possible contacts between these surfaces by *CONTACT PAIR.

I wish this might help a little bit.
Don't hesitate to ask if you see any unclarities.
Good luck amir4deh

 

[harry123456]

Amir is right in his steps. One thing you can do. Go through the getting started with abaqus/explicit and abaqus example problems manual. you will be able to see many problems like these done there. That should help.
harry

 

[flycloud]

Dear amir4deh,

Thank you very much for your great help!

For the part on applying dynamic load, I have further question.

According to your explanation, if I just specify the speed of the cone (for example, 2ft/minute), ABAQUS will automatically apply enough load at the bottom of the cone to move it at that speed?

Or, I should start the pressure at the bottom of the cone from zero and then increase the force by steps. At the time when the cone starts to move, we will keep a force value so the cone can move in that speed?

Thanks.

 

[Amir4deh]

Dear flycloud

When you apply velocity, the cone will move with the specified velocity for the specified duration. It can apply whatever force is required to move, so you don't need to worry about the force at all.
Also the value of the velocity is not important in an elastic-platic response, since you have no characteristic time scale in your material behaviour. But if you are including creep as well, you have to choose your velocity realistically.

So you need an *amplitude, *boundary and *step.
As Harry said, you need to read the manual for these instructions.

Amir.

 

[corus]

It's easier just to apply a fixed displacement. For your given time step the constant velocity applied will be the displacement/time.

corus

 

[flycloud]

harry, Amir and corus, thank you all very much.

I think I need to be patient and keep reading.

Actually, we have ANSYS right now. Can this problem be solved by using ANSYS as good as by using ABAQUS? If not, we may have to buy ABAQUS too.

flycloud

 

[Amir4deh]

I am sorry but I haven't used ANSYS for contact problems so I can't tell.
Regards

 

[harry123456]

I would say that Abaqus Explicit would be better than standard Ansys. Maybe if you use Ls-Dyna which I think is with ansys then it would be similar to explicit.

 

[brad]

A few comments:
1) If an explicit code is used for this, time becomes VERY meaningful. This process as described sounds to me as quasi-static. Any explicit calculation requires the user to be sensitive to dynamic effects.

2) As suggested by Amir--definitely use an axisymmetric analysis if the geometry allows it. You will save tremendous computer resources, and can more rapidly troubleshoot the analysis.

Brad