CCX "custom" for user defined material prop's?

scottr99scottr99
Hi everyone! Currently I see two opportunities to input CCX-specific commands by right-clicking on CCX for 'model definition' & 'step contents' & 'don't gen kw'. However, it doesn't appear that I can use any of these to input a custom material. Is there a trick to making this happen without having to leave the Mecway program?

Thank you very much.

By the way, Victor, this program is really excellent! I'm blown away by it!!!

Comments

  • scottr99scottr99
    Also, I noticed that Eq. Plastic Strain will show up for BISO and BIKN, but not for R-O.
  • SergioSergio
    Hi, you can do it by means of the remove kw feature, you need to remove MATERIAL, ELASTIC and DENSITY keywords. Then create a name selection of elements containing al the elements that will have the specific material. Give a meaningful name. Then add a custom model definition and write your own material definition and make the assignment to the named selection created before
  • VictorVictor
    It's a little simpler than that if you don't define the material in Mecway's own way too. There's an ELSET already there for each component so just add *MATERIAL, *ELASTIC, etc. See p126 of the manual ( http://mecway.com/manual.pdf ) for an example.

    CCX won't generate equivalent plastic strain for Ramberg-Osgood. I'm not sure why.
  • scottr99scottr99
    Thanks Sergio and Victor!

    I'll see if I can get a hold of someone from CCX about why the don't output eq. pl. strn. That's disappointing because R-O is my preferred way to represent my nonlinear material data and equivalent plastic strain is invaluable for plastic failure imo.

    With that in mind, can one of you guys tell me how you enter material props for a plastic material, say some Ultramid gf nylon? Any will do an example.

    Thank you!!
  • VictorVictor
    You can use a set of stress and plastic strain points to approximate the R-O curve. The example in the manual shows that. I'm assuming the plastic is isotropic despite the fiber reinforcement. Sergio would know more about materials than me though.
  • SergioSergio
    Hi, in fact I have experience working with non lineal material (plasticity analysis for crash tests), in Abaqus and CCX for alumiium and steel sheet parts. I always introduce the (true) stress vs (logaritmic) strain curve points in the material definition card, taking in mind that the first point of the serie is the yield point. The solver will take the lineal part of the curve from the elastic modulus, and will allow to postprocess PEEQ.

    For your material you can take the engineering stress/strain curves from Campus Plastics (for example http://www.campusplastics.com/campus/en/datasheet/Ultramid®+1503-2+NF2004/BASF/20/f349878d/SI?pos=7)

    Then there are some formulas to convert to engineering to true stress and normal so logaritmic strain that is what the solver is waiting for.
  • scottr99scottr99
    Sergio, thank you! So you use the *ELASTIC & *PLASTIC cards and enter the true stress-strain curve for these thermoplastics too?

    Victor, thank you! I was successful with what the manual showed on page 126-127, however, I didn't see the PEEQ show up, so I added to my Custom Step Contents the following:

    *DLOAD
    Meshed_Geometry,CENTRIF,100000.,0.,0.,0.,0.,0.,1.
    *EL FILE
    S,PEEQ

    ..and this produced the Equivalent Plastic Strain! So now I am happy! :)
  • SergioSergio
    A little more of info

    http://www.npl.co.uk/upload/pdf/elastic-plastic-materials-manual.pdf
  • scottr99scottr99
    I saw that manual, good stuff!!
  • SergioSergio
    Yes, now I realize that what I was using was the "hardening curve"
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