contact stress pressure in an interference fit

DRQDRQ
Hi,
I've been modelling an assembly that includes a cylindrical interference fit using CCX 3D Nonlinear and contact loads/constraints (as per 9.9 of Mecway 14 manual).

I'm having some difficulty understanding quite what is meant by "contact stress pressure" and how that relates to the radial stress at the interface.

I expected the "contact stress pressure" to be equal to (or close to) the value for the radial stress at the interface, and this seems to be about right when the "Normal stiffness per unit area" is close to its default value. However the "contact displacement clearance" is reporting values that are big enough (or look that way) to be significant, around 1-10% of the interference and I'm interpreting that as the interference isn't quite fully applied.

Since the model is reporting stresses fairly close to the design limits I've tried reducing that "contact displacement clearance" by increasing the "Normal stiffness per unit area" and that does appear to work, as I increase the "Normal stiffness per unit area" the "contact displacement clearance" is reduced. But the relationship between radial stress and "contact stress pressure" appears to affected detrimentally. For example, I increased the "Normal stiffness per unit area" by a factor of 10^4 and the "contact displacement clearance" reduced to much lower values (0.05% of initial interference) but the value for radial stress is now about 81% of the "contact stress pressure".

I've got a couple of concerns in that it's got me doubting the reported stress values and I need to know what the actual contact pressure is. If I was doing hand calcs I'd use the radial stress at the interface but the geometry is too complicated for me to get a reasonable comparison between hand calcs and FEA. Which of course now makes me think I should do a simple FEA that I can replicate in hand calcs, but I hadn't thought of that when I started writing this!

By the way, there are added complications such as using "thermal stress" and applying temperatures, etc. but everything else seems to make sense.

If anyone has any comments on this they will be appreciated, even if it is to tell me that I'm doing something completely stupid!

Comments

  • JohnMJohnM
    Your press fit is a deflection-controlled problem, meaning it's important for the contact stiffness to be high enough that the penetration is low compared to your interference. For instance, if a 10mm pin is pressed into a 9.98mm bushing, the 0.01mm radial clearance creates all of the stress. If your contact stiffness is low, and your penetration is 0.005mm, your loads will be cut in half.

    Try running the attached model. For the 1MPa pressure, the blocks have a 1MPa stress in the Y-direction, and the contact pressure is also 1MPa. This is a load controlled problem.

    Next, note the UY deflection where the pressure is applied, and change the pressure to a UY displacement input. Re-run, and you will find that the stresses have dropped. The problem is now deflection controlled, and the contact stiffness now matters. Change the contact stiffness from 700 to 2000 GPa/m (I think, or maybe a bit higher), and the stresses will start to match the first problem.
  • DRQDRQ
    Hi JohnM,

    Thanks for taking a look at this, and your example. It was particularly useful because I'd made some kind of mistake in my simplified model and I was pulling my hair out thinking I'd completely misunderstood how it worked.

    I've run through your example as you suggested and it all works as you describe and that's what I was expecting. However in my complicated model the radial stress (since it's cylindrical) doesn't seem to match the contact pressure once I increase the contact normal stiffness. In your example I can see that "stress YY" doesn't quite match "contact stress pressure" for "s102" but it's not very different, and not as different as I was seeing.

    I managed to get my simple cylindrical model working and matching up to my hand calcs and that, like your example, doesn't show the divergence between normal stress at the interface and the contact pressure.

    I guess that means it's something peculiar with my model rather than my refreshed understanding of contact generally.
  • JohnMJohnM
    Pin/ bushing work best with hexahedral geometries when possible. Elements with mid side nodes will also help preserve the curvature characterization. Tetrahedral meshes, especially if not very fine, can give some strange results.

    Here is another example, you can download the case:

  • VictorVictor
    Also make sure the mesh is fine enough. You can check that by putting a local refinement at a point on the interface and see if it makes any difference to the stress there. As JohnM said, make sure the curved surface remains curved when you do this.
Sign In or Register to comment.

Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Register