Compression only material

gemadagemada
Hi. I'm trying to model a reinforced concrete beam under flexion (non linear chart with load x displacements).
In Mecway I can use bilinear isotropic for steel reinforcement, but I don't have a compression only option for concrete.
From mecway operation manual it seems that I could do this by editing calculix input file but I don't know how.
From calculix manual I should input something like this:

*MATERIAL,NAME=COMPRESSION_ONLY 
*USER MATERIAL,CONSTANTS=2
 1.4e10, 1.e5 
*DENSITY 
2350. 
*MATERIAL,NAME=STEEL 
*ELASTIC 
210000.e6,.3 
*DENSITY

Can somebody help me?

Another question, are there any plans to implement compression only materials like concrete or the ability to input a stress strain curve for brittle materials?

Thanks a lot.

Comments

  • VictorVictor
    This example is in the test files called concretebeam.inp. I solved it and it looks like the tensile stress on the concrete part is much lower than the compressive stress.

    There's currently no compression only material in Mecway. I think you can just paste that material definition from CCX into Mecway's custom model definition as shown in section 14.1 of the Mecway manual.



  • gemadagemada
    Thanks for your reply Victor.
    I've done as you said but it seems that the nonlinear analisys is independent from the "compression_only" material properties that I input in custom model definition.
    I guess I'm missing something.
    Can comebody check the attached file?

  • VictorVictor
    This one works. Changes I made were:
    • Added a *SOLID SECTION block to link the *MATERIAL to an element set.
    • Added a layer of ordinary linear material on the top so it doesn't fall apart when it goes into tension. This represents reinforcement.
    • Reduced the force.


  • VictorVictor
    Here's the .liml file I didn't attach.
    cb.liml 476.8K
  • gemadagemada
    Victor, thanks a lot for your reply. That worked.
    I'm trying to model an experimental 4 point bending test in a reinforced concrete beam.
    The modeled steel was meshed with an equivalent area layered inside the concrete.
    I started by applying load in 5 kN increments (from each analisys I plotted the load-displacement values at the center of the beam), but  I started to having some convergence problems for applied loads higher than 15kN. Beyond this load large deformations appear in the support area.
    So I've edited custom step contents and applyed loads with 1 kN increment above 15 kN. This way it converges but there are still large displacements in the support area (see the liml file). Is this supposed to happen? I've attached the liml file and the plotted chart.

    Also, I'would like to try apllying vertical displacements instead of loads. How can I model this: apply a displacement increment of 1 mm until the maximum stresses exceed the ultimate tensile strenght of concrete (3.5 MPa)?

    Thanks.
  • VictorVictor
    It's probably because the material near the supports has broken. The graph shows it's tensile stress suddenly exceeding the limit so it probably loses strength in all directions when that happens.

    I tried moving the supports up to the steel part and it then works OK.


  • gemadagemada
    edited October 2016
    Thanks Victor. Should this happen even if the tensile stress (0,35 MPa) is lower than the strenght (3.5 MPa)?

    Also, I'would like to apply vertical displacements instead of loads. I've tried that but it doesn't output any results (choose the 3 upper center nodes and apply y displacement of -1).
    How could I model this: apply a y displacement with increment of 1 mm (total of 6 mm displacement, for example) and plot the maximum stress strain curves in concrete and steel?

    Thanks a lot
  • VictorVictor
    The tensile strength is only 0.35 MPa according to the material definition so it seems to be failing just right. Maybe that's a typo?

    *USER MATERIAL,CONSTANTS=2
    35e10,3.5e5

    For a fixed displacement, please see the PipeClip.liml sample described in the manual which does that. You might need to ramp up the displacement as in that sample to help it converge.

  • gemadagemada
    Thanks Victor. Sorry, that was a typo error. And PipeClip.liml sample helped me a lot.

    So I've modeled 2 rc beams in a four bending test: One is under reinforced (10 mm rebars). I've attached the ploted values (experimental and mecway non linear with concrete as a compression_only material).
    Steel was modeled as bilinear isotropic hardening. I've tried with 4 different tensile strenghts for concrete: 3.5 MPa (10% of compression strenght) and lower values.
    The FEM results don't seem good unless I choose a tensile strenght for concrete of 0.5 MPa (the ususal value is about 10% of compressive strenght).

    For better results with 4 point bending testing I believe I would need to use a user_material subroutine for concrete based on abaqus plasticity damaged model including the stress strain curves (compression and tension softening). I've read calculix manual and it's possible but it seems complicated for a beginner like me to do that. Can someone help me on this?
    Thanks once again.

  • gemadagemada
    Just to correct my latest reply: the under reinforced beam has 6.3 mm rebars and not 10 mm.
  • VictorVictor
    I don't know enough to comment on these results. For anyone else looking at this, there is some further information about the same issue in this CalculiX forum thread:

    https://groups.yahoo.com/neo/groups/CALCULIX/conversations/topics/13225


  • gemadagemada
    Victor, thank you for you reply and link. I've contacted Guido (from calculix) and he also pointed me to that discussion group. I've already started a discussion about modelling concrete non linear.

    The answers I already got in calculix group:

    a) it's complicated to implement a damaged plasticity model but maybe someone there will have the ability to rewrite a subroutine for that.

    b) Compression only material is not good for plotting force x displacements but it's good for predict critical loads in concrete.

    Question 1) So if I understand correctly, this means I must apply a load (or a displacement) in a reinforced concrete beam, then output the normal stresses in the critical elements and compare those values with the materials design strenght (for compression must check the top center of the beam where concrete will crush and for tension the center of the rebars where steel will yeld). Is this approach correct?

    Question 2) I was thinking of updating in this forum all the information I'll get from calculix discussion group for anyone who is interested in modelling reinforced concrete. I could start a new topic just for that. What do you think?

    Sorry for the extended reply, but I want to say once again that Mecway is a great software. It's amazing how easy and powerful it can be. All, from meshing to solving, is great. And the support here is great.
    Now if one could implement some nonlinear model for concrete in Mecway it would be amazing. I'm just a begginner  in modelling (all my "expertise" is in experimental analisys) but I could help with the basic theory if someone is interested.

  • SergioSergio
    edited October 2016
    Hi, have you try to model your beam and rebars as a 3D extruded solid? In Salome you could mesh the two components (concrete and several rebars) with coincident nodes at the interface, so you don't have to worry about using TIE or whatever to conect both, after export as .unv and convert to .inp to follow the workflow in Mecway FEA.

    On the other side in CCX there is a card called REBAR that maybe could help you. I didn't try yet but guess that I could use for rubber hoses reinforced with textil net.

    I agree with you, Mecway is very easy to learn and with CCX gets very powerfull. You can check some nice examples at my Youtube Channel:


    Do you work on experimental analysis? I'm involved also on that (automotive parts), and even start to build my own dynamometer to play a little on my desk and obviously compare and improve my simulations.

    Regards
  • gemadagemada
    Thanks Sergio. Your simulation are great! I see you are an expert in FEM modeling.
    I've modeled the rebars with an equivalent area embedded in concrete. All in 3D solid elements (you can check the liml file in the previous replies). I've never used Salome so I must learn first how to do what you've suggested.

    My idea is to use a simple model for unconfined concrete under uniaxial compression and tension. This means for concrete in compression: elastic initial stress-strain until 0,3fc plus a multilinear isotropic plastic stress-strain hardening curve above 0,3fc until maximum strain of 0.002 (fc=ultimate strenght in compression). For concrete in tension: elastic initial until 0.1fc plus a bilinear stress-strain softening curve until the yield strain of steel. We could ignore the tension_stiffening effect for a first approach.
    The links below give a better idea of what I would like to have available in calculix + mecway.

    I work in experimental testing of mortars and concretes (materials and structures) in ambient temperature and under fire. Sometime ago I discovered mecway and I love it, but I'm still learning it. It's a slow process because my daily job is in the experimental area (it's very time consuming).
    When you build your dynamometer post it here. It's a great project.
    Best regards
  • SergioSergio
    Yeah, but will be a small machine compared with the ones you work. About 40 kN only, but will mine :-)
  • gemadagemada
    I work with a 2000 kN machine hehe but with 40 kN one can do a lot.

    Sergio I was thinking about the compression_only material for calculix. It is defined by two constants: elasticity modulus (compression) and tensile strenght (tension). It's assumed that in compression material is elastic and it is possible to input diferent E values for different temperatures.
    What if one define this compression_only material with different elasticity modulus for different load levels represented by different temperatures in a time function? (the temperature would be a fictional value just to assign different values of E for a correspondent time that is correlated with the load level). The idea would be to simulate plasticity (time represents load level and for each time the changing E value would be defined by temperature).

    Below there's the link explaining compression_only material for calculix.
  • SergioSergio
    Gemada, I don't have experience with concret or compression/traction only materials, but if you arrange the input file or best Mecway file (using custom CCX content) I will give a look and try to make it work.

    I would preffer to have the part modeled as solid, I don't like too much the treatment of 2D element in CCX. Can you add a picture or scketch of your real model?

    Regards
  • gemadagemada
    Hi Sergio,
    Sorry for the delay in the reply. Here is the mecway file.
    I've seen a reply from user jvrajadell  in version 7 beta post. He used 2 nl models for concrete (compression only and another nl model not specified). I've send him a message asking for some help about this.
    I hope I can get some help.
    Thanks once again.

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