Hi all,
I am currently working on a project where I have a 3D model. This one is composed by :
-core : wood
-fiber layer : top and buttom
-HDPE layer : top and buttom
I modelize my materials with :
fiber : elastic-lamina
wood : elastic-orthotropic
HPDE : hyperelastic
I use skin option for fiber and HDPE. I launched the calculation this morning but the first problem I got was : LAMINA CAN ONLY BE USED WITH PLANE STRESS ELEMENTS
In order to sort out that (I can't use a 2D model), can I use elastic-engineering constant for fiber knowing I am working with UD fiber? Thereby E3=E2 and G23=E2/2(1+v23).
Moreover concerning the option FAIL STRESS. I can get MSTRS, TSAIH, TSAIW and ASSI-TSAI-HILL. I use the option for fiber. But what happens for wood and HPDE? Should I add a damage criteria for each?
Then how does Abaqus know if the fiber is 420 gm or 300 gm, only with the thick, right?
At last I would like to use some symmetry conditions in order to save calculation time. I know that the symmetry condition works with boundary condition for example but could it work with skin?
Thanks a lot for your help
Dear Antonin,
Yes, you can use "engineering constant" option for 3D model. The elastic modulus of E2 and E3 equal to each other but the other engineering constant such as poisson's ratio and shear modulus should be taken from the data sheet. Generally, poisson's ratios nu12 and nu13 and shear modulus G12 and G13 equal to each other according to your material axis and your composite system.
You can use USDFLD subroutine for the failure criteria. For example you can implement any failure criteria to your model for different materials.
What do you mean by "fiber is 420 gm or 300 gm"? During calculation or measurement of elastic properties fiber volume fraction is taken into consideration. In the model you can change the thickness of different plies if they are different.
Symmetry conditions can also be assigned to the skin.
Best Regards.
Kenan
Dear Kenan,
Thanks a lot for answering. Could you just tell me if you agree also with the formula for G23?
Concerning the failure criteria I wanted absolutely to avoid using a subroutine. Indeed I have no skill in programmation and that would be the first time... But if it's the only way I will use it. I thought that I could use the FAIL STRESS OPTION for fibers and another one for wood and HPDE, the question is which one(s)? There is some failure criterion already in Abaqus(like fail stress option). Actually I am also wondering if you need to use a failure criteria for wood and HDPE. I am not sure but maybe fibers would break before wood and HDPE and thereby no need to apply a criteria for the last ones. What do you think?
Concerning 420 g/m², 300 g/m² I mean when you buy a fiber you have to choose the density of this one. A 420 g/m² fiber will not the same properties than a 300 g/m² fiber. I was wondering how Abaqus knows this density. I guess it's only with the thickness like you say.
Thanks a lot again Kenan for answering,
Regards,
Antonin
Hi, you could use continuum shell stacked manually for composite and solid or contiuum shell elements for wood. It is true that composite layers are not supported for solid elements, specifically witj abaqus (i don t know if it is what you use). By using shell elements, it will be possible to use fail strain or stress for the composite. For wood hdpe, i would use either a plasticity model for polymers. For fiber density, it is not taken into account, it is the mechanical porperties and the ply dimensions, as mentionned by Kenan, that will be used. Pay attention, you will not be able to use fail stress or fail strain with solid elements, this is why you need to use a plane stress formulation for composite plys.
Thanks ! What do you mean by plane stress formulation for composite plies? I am trying to modelize a bending test. Moreover if I use only plastic models for polymers I cannot know when that will break, right? I have to use a damage criteria. Indeed, for instance, if I apply a elastic+plastic behavior to aluminium for a bending test, my stress/strain curve will go on without stopping as Abaqus doesn't know where is my failure point(I am not sure, maybe I am telleing something wrong...).
to use continuum shell, you can model your part as a solid but create a C-shell section. This section will then use eng constant and fail-stress strain. You might also need to define cohesive contact at the interface between wood and composites
Ok understood. Thanks a lot Philippe. I use a skin on my top and bottom. I assign a shell section to those ones. Looks working with eng constant and fail-stress strain. What about the wood and HPDE?
- Badges
- Science topic