turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- CAE Simulation - Femap Forum
- Behavior of aluminum under severe compression load...

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-12-2016 01:32 PM

Hi,

the model I'm working on is loaded in compression (buckling is NOT critical though,I checked it). When I plot the Min Principal Stresses of my linear run (aluminum), I see a wide region below the -(Tension Yield Stress).

I don't know if I can consider that my model is getting plastic or not. Some references I've seen argue that the compression stress-strain curve is the symetric of the tension curve, some other argue that the part in compression can go way further than the tension yield stress.

Should I run a non-linear material analysis with the tension stress-strain curve? Or can I just consider that my part is fine and safe and won't go plastic?

Thank you,

Florian

Solved! Go to Solution.

8 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-14-2016 11:20 AM

Hello Fl-sim,

If I understood the email you run linear analysis and you see large region exceeding the yield stress. If the large stresses are coming from:

- Singularities like boundary conditions or loads application you may skip this region and say that you are ok. It depends on the approach for the boundary conditions and loads. This task it is user responsibility
- from “real” stresses then you have to perform a non linear analysis. Linear buckling analysis does not take into account this. About if yield is larger or not in compression I would say that for steel (I think also aluminum) same value it is taken for tensile/compression. Normally if you take the same you are in the conservative side. Sometimes it is difficult to make proper measurements under compression. If you do not have more precise data it keeping always in the conservative side

If the stresses are “real” and the whole section is exceeding the yield probably the structure is close to its limit and you will have convergence problems. Plotting the curve load-displacement you can see the actual buckling load limit

I hope it is helpful .

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-14-2016 12:37 PM

indeed I used the conservative tension yield stress as limit even in compression. However, I don't want to ask my customer to redesign everything because of an overlimit stress in compression, cause I know it is not as critical as it is in tension (in tension -> failure, in compression -> ?), thus my question.

I tried to run a NL analysis (sol106), defining a plastic stress-strain curve. Oddly, I didn't see any plastic strain. Don't know if it is because my curve was going from 0 to +0.007 in/in (curve not defined in the negative) or if the analysis doesn't consider compression NL strain, or if I did something wrong in my post-processing...

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-15-2016 02:24 AM

If you used the simplest setting for SOL106, plasticity will only occur if the Von Mises stress exceeds the specified yield stress. The most common situation where Min Principal stress could be "very large", without plasticity occurring, is in high hydrosatitc loads. For example, an item placed at the bottom of the deepest ocean is subject to full hydrostatic stresses. The Min Principal stress (and Max Principal and Intermediate Principal) could be, say, -100MPa, whilst the Von Mises stress will be zero. The same can happen in tension as well. So if your stress state is quite "hydrostatic", then the Von Mises stress will be much less than the worst (absolute) principal stresses.

So, if you had high negative min principal stresses (more in absolute value than the yield), then you are probably getting no plastic strain becasue the VM stress is less than yield. You would need to use an alternate yield criteria, and you may observe a difference. I think there are a few yield criteria which separate the hydrostatic aspects of a stress state.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-15-2016 02:31 AM

The von mises criteria takes plasticity as a number . It does not depend on compression or tensile. So the curve defintion is enough with the tensile part. At least in other solvers.

If you are using sol106 it seems to be that you are not reaching von mises stress. As EndZ explained it.

Maybe you should provide some images of tension (von mises and min) to see the problem

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-15-2016 10:51 AM

Thank you EndZ,

I knew about the hydrostatic component and how the VM criterion doesn't fit with this stress state. I would have zero VM stress is my part was, for example, a cylinder completely filled with material. In the case of a hollow cylinder (my case), the walls are bending under pressure, and VM stress appear.

I'm done some reserach on alternative Yield Criteria, there are a few (Tresca, Mohr-Coulomb), but all based on shear (which makes sense, metals are failing by plane sliding).

Bottom line, I think it's ok to consider VM stresses as a criterion in my case, and not consider Min principal Stress.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-15-2016 11:27 AM

Analyzing the information:

- You run linear analysis
- You see high compressive stresses and von mises. That means s1,s2,s3 are different not corresponding to hydrostatic state
- Type of stress: Bending stress
- The issue: after running nonlinear analysis with sol106 you are not able to see any plastic strain. The material does not go beyond the yield you define.

Questions about the model

- Modeling with shell of solid?
- If you are modeling with solid maybe you need more along the thickness to detect the plastic behavior. Plasticity is only detected at gauss points which area at a distance from the surface. As you mentioned bending I guess you are getting high stresses at the outer surfaces. ????
- If you are modelling with shell plasticity should be detected.

- Which stresses are getting from this nonlinear analysis?. If it is elastoplastic perfect the maximum should be this yield in the region, where you have defined plasticity

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-15-2016 02:30 PM

you've pointed something important I think: my model is a TET10 mesh, but since I don't have a powerful machine, I meshed with only one element in thickness. So my model is probably not accurate enough to capture the plastic strains.

Moreover and to complete the analysis description, I'm using as Contour 60183 Non Linear Solid VM Strains and 60184 Non Linear Plastic Strain. VM strains give 0.00155 in/in (which match with my Young modulus of 71000 MPa and Yield stress of 110 MPa), and Plastic strains give around 0.0003. So, there ARE plastic strains, but they are very low.

I'll dig a bit more into the meaning of the different outputs (Max shear strains for example) and reconsider my analysis with more elements.

Thank you all for your support.

FL

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

06-16-2016 02:17 AM

Ok. I know this problem. No time no powerful machine... Meshing with hexaedral takes time.

From my experience pure bending needs at least 3 elements through thickness. 4 better of course.

Take into account that pure bending the maximum stress is at the outer surfaces. And the gauss points do not locete at these locations

Great if the posts were helpful

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc