Non-uniform pressure distribution from gudgeon pin

[diverblue]

Hi all,

I'm relatively new to Abaqus and have run into difficulty modelling a non-uniform pressure distribution supplied to a conrod by the gudgeon pin while under pure tensile loading in the direction of its length.

To model the analysis I have assigned a pressure to the interior surfaces of the conrod's small end whilst rigidly clamping the big end. By default the pressure distribution is uniform and in a direction normal to the small end's cylindrical surfaces. I wish to change this to pressure in one direction parallel to the conrod's length (x-axis) and distributed so that the maximum load is experienced at the apex of the small end’s gudgeon pin hole, with the pressure decaying in magnitude 90degrees either side of the apex. This pressure is representative of a bearing load.

I have already successfully created and run the analysis in CATIA which offers a one-click method for assigning a bearing load to cylindrical surfaces. Abaqus is trickier and I know I need some form of script to transform the pressure from uniform to what I’ve (hopefully) described. This is where my knowledge breaks down! If anyone could help me out with a script or at least point me in the right direction that would be fantastic! FYI I am running Abaqus V6.11-1.

Thanks in advance for any help!

 

[corus]

Not too sure what you mean by a script, but the way to do it would be by a fortran subroutine where the pressure is a sine function.

 

[diverblue]

Ah yes subroutine, I got confused with script. Im aware I need to use a wave function but i'be failed to implement it accurately. Do I used the analytical field option to input the formula?

 

[corus]

Never seen an analytical field option. Specify user defined function in the Load module, magnitude 1, and include the .f file containing the subroutine for dload when submitting the job (if you have a fortran compiler). Simples.

 

[diverblue]

The analytical field is there but perhaps it's a recent addition to the software. It allows for user defined formula which can be assigned in the load module. I have used the analytical field to write an equation defining the load as a sine wave but I don't know exactly how Abaqus integrates this function with the my specified load magnitude to produce the necessary loading condition.

In terms of the subroutine how do I develop that? I've had a flick through the documentation but there's a lot to take in! Also that magnitude of 1, is that independant of the actual load and just acts as a scalar? i.e. do you include the magnitude of the real load in the subroutine?

Thanks for the help so far, appreciate it.

 

[corus]

Ok, found the analytical field option as a tiny f(x) button at the side.

If you have a pressure distribution over half a cylinder that varies as P.sin(theta) and you know the total load, F, that is being applied to the pin. Then the pressure distribution is 2F.sin(theta)/(Pi.R.L) where R is the radius, L the length of cylinder. In the function definition you'd have to use sin(theta) in terms of X and Y, I guess.

In the manuals there are examples of the DLOAD subroutine. This would probably do the same job as the analytical field function.

If you use the function as described then you don't have to worry about applying a value of magnitude, and just leave it as one. Alternatively, just define the sin(theta) function and apply a magnitude of 2F/(Pi.R.L)

 

[diverblue]

Thanks for the help corus. I'll have a play about with that equation and see what I can do. I have been using similar equations in the analytical field already and they haven't seemed to work but fingers crossed!