Sheet Metal Bending Simulation- Non Linear CCX , Steel Strip using Contacts

barrtibarrti
Greetings

I have been trying to model the bending of a 10mm wide x 1mm thick strip. The bending is done by a steel block approximately 40x20x10mm with a rounded contact for the bend operation. It is trying to simulate a Wiping Die Bend (as opposed to a Vee Bend). The block is forced upwards and contacts the strip. This model works until Time= 0.1722 seconds at which time the model "explodes as seen in the second image.

I am using 20 node elements with reasonable mesh density. It is a surface to surface contact.
I have tried using lots of different settings in "Analysis Settings".
I have tried switching the contact faces.

I am trying to get it to the point where the 10mm strip is bent at 90 degrees.

I am using plastic bilinear material.
I have not used friction in the contact

It looks like the solution fails just as the contact between the block and strip starts to move onto the radiussed corner??

Does anyone have any suggestions for why the model explodes at this time (0.1722 sec)?
Just before the solution stops, the number of iterations goes up to say 50.

Am I better off using 10 Node Tets for contact?
Should I increase the number of elements thru the thickness?

Regards Barrti

Comments

  • barrtibarrti
    Update: The "exploding" does not wreck the model where it is constrained (see Capture7 and 8below)
    Barrti
  • VictorVictor
    All those settings look pretty good. Two suggestions:

    1) Use a prescribed displacement instead of a force. It looks like the strip has reached yield across the whole cross-section so maybe it's collapsing and can no longer support any more force from the block.

    2) Turn off plasticity. If that works, then turn it back on with gentler parameters (larger tangent modulus) and it might fail later in the process where you can see more clearly what's going wrong.

    I tried 1) along but it seemed to get suck at 0.002 s. 1) and 2) together works easily, as shown in the picture. So I'd look at the tangent modulus next.
  • barrtibarrti
    Victor,

    Thanks for this. I am trying to get about 10mm movement of the big block -i.e 90 degrees bend. I followed your instructions and eventually got about 5mm by increasing the Contact stiffness to about 100xE.

    I still cant get the 90 degree bend by using plasticity. One trial used Bilinear with 250MPa/50 MPa tangent stiffness but no luck. I tried Ramberg-Osgood model for 1020 Steel - no good either.

    The model just explodes and I cant see any hints as to the problem.

    Are there any other tricks I could try?
  • SergioSergio
    1) First I would try with lineal elements
    2) You could try to reduce the size of elements in the contact zone, and to keep the model small and quick to solve reduce the number of elements in Y direction to 1 and use simmetry to consider the full geometry.
    3) Another try could be the use of reduced integration elements, they have special formulation to avoid hourglassing.
  • SergioSergio
    I just make some trials, you can do for improve:

    Use lineal elements
    Include both parts of the die (male/female)
    More important, you cannot block (clamp) the end of the strip, the material must have some possibility of sliding, otherwise will be excesive and artificially streched

    Reduced or incompatible elements doesn´t help.
  • SergioSergio
    I create a new model based on the one that is available on Youtube, but made it with Code_Aster, a very similar case. A punch, die and a blank sheet to press, and want to model the donward and upward of the punch to see if is possible also to check the springback.

    https://youtube.com/watch?v=9VrowX5BO6M

    The nominal distance between punch/die is 30 mm, so in the first configuration I did the same as the videos, without considering the binder....can´t reach the full displacement, only up to 29.9925, but elments explodes and can´t do the upward of the punch



    Then I setup a displacement restriction to quicky simulate the binder, but again the same displacement and element explosion







    Then I though, ok, I cannot reach 30 mm, but -29.9925 is ok, so I setup a third configuration up to a little less displacement to see if I can complete the run... but now elements doesn´t explode but a new weird deformation at a lower displacement!!! What can be happening??? I try several times decreasing a little the displacement, 29.9, 29,8, 29.5 and always explode, but in the first case it can compute up to 29.9925




    I´m attaching also the liml model and the cad source if somebody wants to keep playing.



  • barrtibarrti
    Sergio
    Thanks so much for all of the work you have put into this. I'm not finished yet but I followed your suggestions and got an improvement when I used 8 node elements and also simplified the restraint. I got greater movement and the strip was almost at 90 degrees but I'm using an elastic material to get it there. Not finished yet.....! Still trying to get a realistic plastic model working.

    Thanks for sharing your work on the press tool. Very interesting and helpful. The friction values for friction were helpful too.

    Regards
    Barrti
  • barrtibarrti
    Sergio
    I ran your exact file in v7.0 with automatic steps unticked and it ran to completion which it would not do before. Before with automatick ticked, V7.0 would stop at T=0.33sec.
    I stopped its motion at 29.9 sec to avaoid explosion.
    Barrti
  • SergioSergio
    edited October 2017
    Barrti, you meant you have been able to go downward and then upward with the die? Was a matter of v8 automatic settings? If that the case can you copy/paste the step definiton of the .inp that solves succesfull?

    Regards
  • barrtibarrti
    Sergio
    I meant that I ran your model down and up to completion to 29.9mm deflection (T=1.0 sec) on my machine using v7.0. When I first ran your model on v7.0 , it stopped at T=0.33 sec. When I unticked automatic time steps, it ran to completion (T=1.0 sec).
    I have attached my run of your model below if u need it. (inp file as requested)

    Unticking automatic steps seems to have helped my model as well. I got it to run successfully to the end for the first time with a realistic material (T=5.0 sec and 10mm deflection). The difference was that I used 8 node elements for strip and block, simplified my restraints as u suggested and unticked Automatic steps.

    My restraints on the strip were mostly Z-axis with a few to stop movement in X and Y.

    The material is Bilinear Isotropic 250 MPa yield and 1GPa Tangent Modulus.

    I have not yet changed my model to come backwards to the beginning as you have so that I can see the springback. I will post it once I have.

    There seems to be a lot of springback with your model. I suppose that changing the plastic model and using more elements would help?

    Do you think that there is any advantage by using 20 node elements? Will this help modelling springback? They sure are a lot slower.

    Regards
    Barrti
  • barrtibarrti
    Sergio
    I finally finished a run with a refined 8 node version of the test strip. I have attached the liml and inp files as requested below as well as a few images.

    This version use fairly realistic material - Bilinear withe 250MPa yield and Tangent Modulus=1GPa.

    Contact K was 20000 GPa (100xE), no friction.

    Auto time step was turned off which for 5000 steps (0.001 sec each) meant that the run time was about 18 hours with an i7-3770k PC!

    Results are shown. The final deformation at T=5.0 sec looks a very wierd.
    At T=1.0 sec, you can see the strip is penetrating a lot despite K being 100xE.
    After this the penetration gets worse - decidely funky even.

    I guess turning off auto time step in this case forced the solution to finish without exploding. It clearly takes too long so as u suggest, using less elements is always good.

    I didn't try to show springback as it would take longer.

    Victor, I'm curious if you have any comments or suggestions.

    Regards
    Barrti
  • simonsimon
    edited October 2017
    Sergio,

    After a bit of tweaking, I got your model to work with both elastic and plastic material. What caused the "explosion" seems to be the contact not converging. It can go the full cycle up and down, but with automatic time stepping it does not always stop at exactly 30 mm. It could probably work with with very small increments, but I gave up at .01s.
  • simonsimon
    Barrti,

    Just a few tips you might find helpful. With plastic analysis like these, you should be looking more at strains instead of stress, which are likely very high at the bend. Idealy, you should also use an actual stress-strain curve instead of a BISO model. Your tangent modulus seems pretty low, at less than 1% of the elastic one. You would also need a lot more elements for an accurate springback estimate.

    These type of models are easier to do in 2D, but that's not possible in CCX.

    I'm not very encouraging, but severe plastic deformation modeling is pretty hard to do.

    Simon
  • SergioSergio
    Hi Simon and Barrti, I was able to solve also using fixed time step (0.001 second), with plastic material. In my model I just use a bilineal isotropic option with the yield and tangent modulus for a basic hot rolled steeel.

    What is making me noise now is how big is the springback, I check some videos on youtube of similar models and they use the plastic definition by means of the data points, i´m not sure if that would be enough to change the behavieur substancially.

    Other thing to try is to improve the binder modeling, now is only a restrain in horizontal direction, but should be a compression with friction, this must create some restrain of the part (not only horizontal but also lateral) and then create more strain on the bends (and then maybe less springback).

    I agree with Simon, for this kind of analisis what you must postprocess is PEEQ compared with the maximun strain on the material, that will tell you if the part will breack or not on the bends.
  • barrtibarrti
    Simon

    Thanks for all of your work and advice. That has helped a lot.

    Yes, I am convinced you are correct - it is hard. I did a little with several big name codes a few years back. Can't say I was impressed then. I was trying to model impact forces on a structure. There was less deformation and I got some pretty animations but we ended up using a fair bit of judgement. The vendor later admitted that their software was not good at modelling impact.

    We later used a quicker approach which was a bit more convincing and quicker.
  • barrtibarrti
    Sergio
    Thankyou for your advice too. Greatly appreciate your efforts.

    Cheers
  • VictorVictor
    Barrti, just a comment on the 8-node hex's. Are you using reduced integration as Sergio suggested somewhere way back? He found it didn't help with hex20 but it's particularly important with hex8. Without that, 2 layers is probably too stiff. That might be why penetration is so high - they might have a big artificial stiffness.
  • barrtibarrti
    Hi Victor
    No, i didn't get to it. Is it as easy as going to Tools/Labs/and clicking CCX Reduced Integration on Linear Elements?

  • VictorVictor
    Yes. Just beware that the setting clears itself when you close the program. In v8, it's under Loads & Constraints and is persistent.
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