3D modeling of composite material in ANSYS
Submitted by Basak on Tue, 2008-07-15 21:52.
Hi,
I am trying to model a composite material in ANSYS. I have used ANSYS for simple simulations before but I have never done composite material analysis. I have attached a simple schematic of what I am trying to model. Can you guys please help me? Any tip you can give will help. I have limited time.
Thank you,
Basak
| Attachment | Size |
|---|---|
| schematic1.JPG | 40.19 KB |
»
- Basak's blog
- Login or register to post comments
- 1661 reads
Should I use SOLID46 for the
Should I use SOLID46 for the outer material and SOLID45 for the inner material?
You can, in principle,
You can, in principle, use SOLID46 for composite layers. It lets you define the orientation and material of each layer directly. But then your freedom to mesh as you want is hindered (as I remember you can have only one element per layer in SOLID46) and if you have a complex geometry, you would need a finer mesh.
On the other hand, you can always use SOLID45 elements even for composites. It will be more accurate. Just define the relevant material properties and use a different coordinate system (CSYS) to define orientation for each layer. So, for your case, you will have 5 such cylinders - 1 innermost for isotropic material and 4 for the 4 layers of composite material. Create the 3D model in this way, mesh it and define CSYS 21-24 (rectangular) with orientations 0,45,-45,90 etc. Select elements in each cylindrical layer and modify its CSYS and material to the required one.
e.g., Use this series of commands after defining an volume component for +45 layer:
1. cmsel,s,vol_p45 ==> Selects the volume vol_p45
2. alls,belo,volu ==> Select everything below selected volume (i.e. select elements)
3. local,21,1,0,0,0,0,0,0,45 ==> Define a cylindrical CSYS no. 21 rotated at 45 deg w.r.t. z-axis (you need to see how your lamina are oriented)
4. emodif,all,mat,2 ==> Modify all selected elements to have material no. 2
5. emodif,all,esys,21 ==> Modify the coordinate system for selected elements
Read these commands for details.
I hope this helps. Good luck!
----------------------------
Chandra Veer Singh,
Aerospace Engineering,
Texas A&M University
Thank you!
Hi Chandra,
Thank you very much for your suggestions. They helped a lot! One quick question : What do you mean by one element per layer in SOLID46? Do you think my geometry is simple enough to still use SOLID46?
Thanks again,
Basak Oguz
Mechanical Engineering
Michigan State University
Chad has raised an
Chad has raised an important question. You can solve it using 2-D stress analysis, for which analytical solutions are avaialble.
However, if you want to do a 3-D analysis then:
Although this geometry is simple, I would suggest to use SOLID45.
Although you can get around "one element per layer issue in SOLID46" by
dividing a given layer into N imaginary sub-layers of same orientation
and thickness=layer thickness/N.SOLID46 can take upto 250 layers. SOLID46 is actually useful for modeling sandwitched structures with thin layers.
I have some modeling and formulation issues with SOLID46 in general
applications, e.g., if you have a variable layer thickness, what would
you do. SOLID45 are based on full 3-D formulation, so much better and
easier to use.
Using SOLID45 and refined meshing with current computational
power shouldn't be a problem. But you need to make sure that you define
and orient CSYS correctly. Once you understand this approach, you can
model complex geometry as well.
Chandra Veer Singh,
Aerospace Engineering,
Texas A&M University
SOLID46
Hi Chandra,
I am kind of confused with the "one element per layer" thing. Ansys says that you can use upto 250 layers/element with SOLID46. Today I tried 80 layers per element (each layer 10 microns) and it worked. I am using an element size of 0.0008 on my mesh which gives me a total of 800 layers in the whole geometry. Am I getting the idea wrong?
Thanks,
Basak
Question
Basak,
Why do you want to analyze this geometry with finite elements? The geometry and loading that are shown in the picture are simple enough to study analytically. That is unless you are treating this as a 3D problem.
Chad
I agree unless Basak has
I agree unless Basak has some specific reason (loading/geometry) to warrant a 3-D analysis.
Chandra
why FEA
Hi Chad,
We are treating this as a 3D problem and we would also like to find out the best composite lay-up that will give the least amount of stresses on the hole. I will not be doing only [0/45/-45/90]s. I will try out a bunch of different combinations.
What stresses are you interested in?
Are you interested in the inter-laminar shear stresses? If this is the case then 3D is the only way to treat this. It still might be useful to look at the 2D analysis, even if it is just a sanity check for your 3D results.