Reaction force from quasi-static solution

DaveStuppleDaveStupple
Hi all, I am trying to recreate a very satisfying study I did previously and is now lost. It involves an elastomer O-ring being compressed into a groove. I have meshed a cross section and revolved through 1°. The CONTACT between the optic that is doing the pushing and the O-ring and the CONTACT between the O-ring and its groove all seem to be working and the O-ring compresses nicely as a neo-Hooke material.

Previously, I initially tried to apply a force over time to compress the email, but this failed so I used a displacement instead. I somehow summed the reaction forces on the optic face to get the total force applied at any time step. The 'add new reaction force' in the solution is greyed out. Solution>Tools>Sum doesn't give me a reaction force option, and the external Y force option doesn't give a sensible value.

Could someone advise how to replicate how I inferred the applied force before, or suggest an alternative approach?

Thanks for reading.

Comments

  • SergioSergio
    edited March 2021
    Hi @DaveStupple, what I do normally in these cases is define a node set "MOVIL", on the upper surface of the movil part, then create a custom CCX card with

    *NODE PRINT,NSET=MOVIL, TOTALS=ONLY
    U,RF

    CCX will create a separate .dat file with the data in a ugly tabular format that you must open with a spreadsheet and filter to get a usable table and create a load/displacement plot. TOTALS=ONLY makes the summatory trick.
  • DaveStuppleDaveStupple
    Thanks Sergio, does it give values for all time steps?

    I found this from Victor on another post:

    "1. Select the fixed elements and right click one then Add elements to new named selection.
    2. Solve.
    3. Solution -> Sum external forces on the element selection:
    a) Choose an external force component
    b) Select only the element selection for the domain D
    c) Evaluate

    That shows the sum of reaction forces at the current time step."

    I still think that the numbers this gives are too low (see attached). I am currently revisiting the definitions of C10 and D1, and I think I may have had it wrong before, but I am not close to being sure I am right this time. I wish I were clever.
  • SergioSergio
    Dave, the NODE PRINT cards by default gives you all the time increments and steps, there is a modifier to made every n increment.

    About your problem, guess that you miss to attach the file.
  • DaveStuppleDaveStupple
    Sergio,

    I was just going to attach the image. As originally stated, the force seems very low, even when multiplied by 360 to sum for the whole circular O-ring. On the next time step the mesh destroys itself - I presume because the deformation exceeds that allowed by the Poisson's ratio. I think I need to understand the D1 and C10 parameters better (and C1 for Mooney-Rivlin), to make sure the material properties are approaching reality but I think I'll make a separate post on that. It might be also because some of the dimensions are quite arbitrary and might not be realistic.


  • SergioSergio
    If you have the dimentions/material of the oring and groove, I could try to reproduce the simulation and see the force.
  • JohnMJohnM
    We do a lot of this. If the parts around the o-ring are much stiffer than the rubber, there is a nice trick. Attach a layer of "stiff" material to top or bottom part (make it a sector model as well). push with only one node that you have put into a named selection. In the results you can look at that single node as a reaction force vs time, and if you right-click the graph you can paste into excel.
  • SergioSergio
    I use something similar, by means of the RIGID BODY card to atach the movil nodes to one pilot node, then apply the bc and ask the reactions forces to this single node.
  • DaveStuppleDaveStupple
    Thanks John & Sergio, that could save a lot of time. I've chosen to move the groove up onto the O-ring, so that the displacement plots tell me more about the O-ring. Is there any reason I shouldn't just use a node on the underside of the block with the groove?

    I have just tried this and it looks much better. The scaled up force is now 132451 N for the whole O-ring. This configuration has also run to full displacement whereas the previous one exploded. No idea why.

    Does the shading for the external force indicate that reaction force is shared by other nodes meaning that this is an underestimate of force through deflection of the component? Maybe this is why you guys use the stiff material/rigid body trick. Neat stuff.

    Looking back, it's amazing how many of the questions I have currently in my mind have been discussed in my previous post:

    http://mecway.com/forum/discussion/comment/2017/#Comment_2017

    It's also amazing how much simpler setting this up has been compared to all the fiddling about with CCX cards back then. I think this a tribute to Victor's development of the software rather than any increase in genius by me.

    image
    F.jpg 322.3K
  • VictorVictor
    I'm a bit late to the party, but I notice your first picture shows the external force is being summed on Optic_underside. Is that the side in contact with the o-ring and without the load? If so, it won't work because contact forces aren't included in external forces so it would be ~zero.

    As for failing on the next time step. That can be more likely if Automatic time stepping is turned off which it looks like it might be.
  • DaveStuppleDaveStupple
    No worries Victor, as long as you've brought a bottle.

    Yes, where the contact is. Thanks for the explanation.

    Yes, saw a few suggestions in earlier posts to turn off Automatic time stepping. When I did, the deformation near first contact was much more reasonable.
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