Pin / Socket analysis

[garymostyn]

Hi All,

I have modelled a circular pin in a part with a clearance hole using solid elements in Nastran for windows. The pin is subject to a offset shear load which results in a shear and moment being applied to the hole. I am trying to model the resultant connection between the two parts using gap elements and sol 106 but I cannot seem to get the gap elements to behave correctly. I have tried reversing the direction of the element and have also give the gap elements a transverse stiffness. There is an 'adaptive' option in the gap element property but I am unsure what this is. Should the friction coefficients be set to 1?.

I have also tried using an enforced displacement on the end of the pin rather than the load but to no avail. The only time I get any success is if I give the gap elements tension stiffness which is the inverse of what I require.

Any help would be much appreciated. Do you know where I could obtain a similar tutorial?

Regards,

Gary Mostyn Beng (Hons)

 

[Qshake]

I'm not sure what the objective of your FEA analysis is.

If you're looking at the load on the pin due to the plate or even perhaps a clevis movement which places the pin in either single shear or double shear this should be relatively easy problem to solve with the aid of FEA.

If on the other hand you are interested in the stress on the plate which contains the hole through which the pin protudes, then I recommend that you apply a sinusoidal load distrubution on the edge of the plate within the hole. This is a very common application for evaluating plate stress due to bolted connections. As such the distributionis widely documented.

Of course, the above application only shows a moment in time during the cyclic motion of what you're trying to capture in your analysis descibed above. If your using parametric software, then perhaps you can change the general direction of the loading through a parametric angle, theta. Hence if your have some other interesting plate features that surrond the hole and wish to know the effect of this pin loading on the plate and ultimately those other features, then you can do this in a single run with the parametric function.

Please provide more information and perhaps we can provide a more specific solution.

 

[garymostyn]

Maybe I did not explain myself correctly. Imagine a blind hole is a solid part (tet elements). A solid tet element pin/bar is inserted into the hole and a shear force is applied to the end onf the pin/bar. This will result in a moment and shear load being reacted within the hole. The resultant stress distribution will be dependant upon the contact between the two parts. This is what I am trying to model using non-linear gap elements (and Nastran for Windows) but I cannot seem to get a reasonable answer. Any help or examples would be much appreciated.

Cheers,

Gary.

 

[corus]

I've found that quadrialteral tet elements aren't much good in contact analysis, or for that matter any quad element, as the mid-side nodes cause problems. It's better to use 8 noded linear brick elements as you've a better chance of getting convergence. Also use prescribed displacements first to initialise the contact, remove them in the 2nd step and apply your load.

 

[corus]

You'll also find that in a clearance hole you'll just get point contact between the pin and hole, presuming that they are both relatively stiff. In that case it might be better just to apply the point loads which you can work out by hand. Contact is usually best used when you have two flat surfaces acting against each other. In your case if the pin and hole were the same size the contact pressure distribution would be useful.

 

[garymostyn]

Thanks,

I will try using hexa elements rather than tets and changing my model such that there is no physical gap. I do not understand why you need to use 'prescibed' displacements (which are presume is the same as enforced displacemens), and then subsequently remove them. Is the purpose of this just to ensure that the model is behaving correctly, prior to removing and applying actual loads?

Regards,

Gary.

 

[corus]

No. Initially you have separate parts in contact so that even if you apply loads to make contact the program believes that there is rigid body motion in one of the bodies. By imposing displacements then you are restraining both bodies but at the same time making contact. Once the bodies are in contact then they behave as a single body and you can impose your loads whilst restraining only one. Occassionally you can get a contact problem to work by simply imposing the loads but by adopting a two step procedure then you'll have better success, I've found anyway.

 

[garymostyn]

Hi Corus,

I think I have now solved my problem. You are correct the problem was due to rigid body motion which I have overcome using dof springs (celas) elements with very low stiffness values. I also removed the physical gap in the model therefore the gap elements now connect co-incident nodes (with a orientation csys specified). I reduced the initial gap size on the pgap card to a low value (0.001 inch). I am limited in Nastran for Windows to using node to node gap elements and therefore the orientation of the element is not updated with nodal displacement. But at least I now have the capability to analyse contact type problems.

Thank you very much for your assistance.

Regards,

Gary Mostyn, Beng (Hons)

 

[RPstress]

Keeping it simple with NASTRAN and gaps is generally very good advice. If possible don't use preloads, don't use friction (at least to start with). The NASTRAN adaptive gaps aren't quite as good as (say) Abacus', but you may get convergence with adaptive gaps when you won't without. The adaptive gap behavior is more up to date than the non-adaptive, and may actually be preferred, but personally I usually try a run with non-adaptive first.

-RJP.

PS: if you have to use TET elements, try very hard to use TET10s; TET4s have to have a very close eye kept on them, as they can give stresses which are dangerously low unless there're a lot of them.

 

[garymostyn]

Hi,

I am already aware of the problems/limitations of tet 4s and always use tet10s, but thanks anyway. I am in full agreement with keeping it simple, because if you do not understand the answer you get then you have no chance with a more complex solution. People forget that FE does not replace engineering judgement.

The problem that I am trying to solve actually involves an interference fit (due to tapered tubes) which is capable of resisting all of the torque for some of the load cases to be analysed. The tubes are also subjected to bending and shear loads. Therefore friction coefficients are to be used, but I plan to use non-adaptive gap elements in Nastran for Windows (at least at first) as you suggest.

What I do not understand is how to apply a two step approach in a non-linear analysis. You suggest applying an enforced displacement to close the gap in the first instance, and then apply the loads. Is this non-linearly analysed as two seperate load cases or as one. I understand the concept on doing this to restrain rigid body motion until the point at which contact occurs, but I do not understand how to apply this in practice. Any help would be much appreciated.

Regards,

Gary Mostyn.

 

[corus]

They are two separate load cases. the first load case will give you the conditions for the second case. In the second load case remove the displacements and apply the load. You can consider the first step as being the inital conditions, in effect, where contact forces have been set up. The second load case will redistribute these contact forces for your particular loads. It'll run better if your applied displacements give a similar overall displaced shape to the applied loads, ie if you're applying a force to the top of the pin then apply a displacement in the first load case in the same direction as you will apply the load in the second case. There'll be less redistribution that way.