Output of forces at nodes.

[mugged]

Hello,

I am trying to model deformation of an elastic material with an epoxy glued to the side. I have been attempting for the past week or so to extract nodal forces along an interaction surface but these turn out to be zero.

Browsing many online queries on the subject, I've found that the RF reaction force output only applies when dealing with boundary conditions. Also NFORC doesn't work because the model is in equilibrium and the forces sum to zero.

The closest I have gotten is when using CFT to output the force due to contact pressure and frictional stress. The huge problem with this is that the forces don't balance in the end. (The sum of the forces in the y-direction is not equal to 0). So I think I am missing something somewhere.

I am providing an input file. I really need to know how to output the forces on the triangular piece so that the forces balance in the y-direction. Thank you

Please help

 

[IceBreakerSours]

Concerns with your model:

1. ABAQUS has no way of knowing if your units are consistent or not. If your geometric dimensions are in mm, then, your modulus must be in MPa. So, the Young's modulus must be defined as 115000 (not 115000000000!!).

2. The quality of the mesh is not great, particularly given the simple nature of the geometry. Play with the partitions and different mesh generating algorithms to generate a better quality mesh.

3. In all probability, you have too many elements (in both regions) than are necessary to give you an accurate enough solution. Start with fewer elements (a few hundred, tops), watch the solution, and see if it converges to a number within some small error-bound.

4. Are you sure about the interaction property definition? For example, do you need finite sliding formulation? Or the node-to-surface discretization? What about the tangential behavior?

5. CPRESS is the variable you are looking for.

Finally, as discussed here, FEA is a time bomb in the wrong hands. You MUST know what you are doing, why you are doing it, and what potential problems your choices may cause in your application.

http://www.eng-tips.com/faqs.cfm?fid=376

 

[mugged]

Well im not sure about the interaction property. In all honesty the triangular region is supposed to be an epoxy material with modulus 2.4 GPA, v = 0.4

So the epoxy material is supposed to be "glued" to the other portion.

I haven't done cohesive behavior before, but currently I am just defining the interaction to be cohesive with normal behavior, and the node to surface discretization is because I get an error when running otherwise. I am also not sure what finite sliding even means.

A better way to glue the epoxy to the other portion would be very helpful. Thank you

 

[mugged]

Also, I am using Abaqus 6.11 and I cannot find the CPRESS variable. The closest I can find are CSTRESS and PPRESS.

 

[IceBreakerSours]

I am also not sure what finite sliding even means.

That's precisely what the documentation is for!

More concerns with your model:

Why is the:

a) static step being run up to 0.6?
b) NLGEOM parameter turned ON?

http://www.eng-tips.com/faqs.cfm?fid=376

 

[mugged]

its up to 0.6 because I have convergence problems past 0.65. I tried refining the mesh but that didn't help - this is why the triangle mesh is much finer than the other portion.

as for NLGEOM, I'm not sure. I thought it would help for convergence. I don't really know what it does either.

 

[IceBreakerSours]

Like I said before, Abaqus documentation is a great resource for modeling purposes.

http://www.eng-tips.com/faqs.cfm?fid=376

 

[mugged]

well my question still stands. Why is it I cant resolve the forces in the y-direction?

I should mention I have tried two other extreme cases. Suppose the angle of the line of interaction in my input file is 45 degrees with respect to the horizontal (the hypotenuse of the triangle). I have tried models of two blocks glued together where the line of interaction is at 0 and at 90 degrees and in both cases the forces work out perfectly with CFT, RF output.

 

[IceBreakerSours]

Is this for coursework?

http://www.eng-tips.com/faqs.cfm?fid=376

 

[mugged]

Nope, im doing summer research. I've been stuck on this problem for the past week or so. But im not doing the problem in the input file, it just has the same characteristics but much simpler geometry and I made it solely so someone could help me.

I know the forces should be equal to each other around the body since this is a static problem. Its just that I can't get the proper output so I can take the data, put it in my MATLAB code and see the forces summed nicely.

All im asking is how do I ask abaqus to output the forces since CFT doesn't work properly.

 

[IceBreakerSours]

Force equilibrium: If you request NFORC output at a few nodes at the interface, you could see if the forces from neighboring elements at a node or two balance out or not (if the model converges, then they have to.) That's static equilibrium.

If you are really interested in forces at the interface, then you have to request SOF for the surface that must be created out of the elements at the surface. But, if you are applying a displacement at the nodes on top,

I ran the model you provided and I could see CPRESS (in the Viewer). It is in the list of Primary Variables (S, U, ..).

Finally, try running the job in the attached file. This is, perhaps, a good first step for you to get comfortable with. Mesh is of high quality (higher order elements arranged well), small sliding formulation, linear geometric analysis, both brass and epoxy linear elastic materials are defined. The model runs just fine.

http://www.eng-tips.com/faqs.cfm?fid=376

 

[mugged]

Thanks for all your help so far icebreaker,

I also see the CPRESS variable in the viewer...the only problem is is that I dont see it in the history output menu or the field output menu, so I can't extract the numbers.

I tried your CAE file. The thing that struck me the most peculiar is that you didn't create a 2nd part but created two 'meshed' parts and split them up into an epoxy and brass section. I was wondering if you can explain how to do this, why there are two meshed parts, and if you can do this if you create an axisymmetric part first.

 

[IceBreakerSours]

I dont see it in the history output menu or the field output menu

If it's the brassonbrasstest.odb that you are talking about, then it is there. Create XY Data -> ODB Field Output -> Position = Unique Nodal -> CPRESS

What I found most odd both from your odb and the one I generated myself is S. It is noisy! See the attached with a very different modeling strategy. Linear elements are used and a constraint equation is used to constrain the nodes. Read the documentation for details.

Note that:

a) in finite sliding, you can not have cohesive behavior.
b) finite sliding causes the two surfaces to come out of contact near the stress concentration. This probably is unrealistic but I don't know the application. Only you can tell.
c) small sliding makes the most sense; shear stress plot is interesting. If the value of the stress is important, you'll have to refine the mesh in that region. CPRESSERI values are high where CPRESS is high; that is a warning sign. Read the documentation for more.

.. you didn't create a 2nd part but created two 'meshed' parts and split them up into an epoxy and brass section.

Nope. I created a part, partitioned it, and then meshed the two regions separately. But, I guess, if the two parts are slipping against each other, then I did not do it right. You'll be better off creating two different parts (although there is a workaround, but its a pain in the neck.)

if you can do this if you create an axisymmetric part first.

I can't foresee any reason why not. Have fun with it!

~!ce.

http://www.eng-tips.com/faqs.cfm?fid=376