Nonlinear fea showing permanent deformation

barrti

Hi

I am very pleased with Mecway and I am looking forward to learning more about utilising its ccx capabilities.

Have just started using the elastic plastic model utilising ccx as the solver. I was curious to see if after experiencing yielding a model would show residual stress and permanent deformation. I used ten node tets with a bilinear model. I ran the model and after the loading was reduced to zero I could not see any evidence of residual stress even though I had exceeded the yield by some margin.

How do I model in order to see residual stresses? Clearly what is happening now is that as the load is reduced to zero the model deflection simply follows the stress strain curve back to zero (as it should). I.e. How do I tell the model to differentiate between plastic and elastic deformation and show the plastic deformation?

Cheers and thanks

Sergio

Guess that you must ask by means of a custom step line to save it and postprocess PEEQ (plastic equivalent strains).

http://mecway.com/forum/discussion/comment/591/#Comment_591

Victor

In version 5, PEEQ ("Equivalent plastic strain" in Mecway) comes through automatically if one of the plastic material types is set. For hand-made material definitions though, you'd have to do as Sergio said.

barrti

Hi
I did use an isotropic bilinear hardening model from the plastic material type I also set the isotopic properties on the mechanical section eg E etc.

It still exhibits the above behaviour. I am missing something I think.

Sergio

Tomorrow will try a simple model with loading and unloading, in fact never did it with CCX.

Victor

It should still show deformation after you release the load, so maybe it's not really being loaded all the way or somehow losing the plastic material data. Feel free to attach the liml file to the forum here.

VMH

Barrti, see attachments.

Hope this help. I did it quick test on a simple free-standing column on Mecway version 5.0, CCX2.8p2 using 4"x4"x36"; E=29e3ksi, Poisson ratio=0.3, Yield=36ksi, Tangent Modulus=210.3ksi, Horizontal Force at top of column ramped from 0 to 15kips to 0.

Mecway version 5 is really nice with the graphs (see attachments).

VMH

Forgot to mention: click on the interested node and the graph will appear. The popup window will indicate the value of the selected node at the selected time. Move the scroll to a different time and click on the selected node again and the popup window will indicate the value at that selected time.

Sergio

Great example VMH! Will try to reproduce tomorrow. I really like the timed plot feature. I need to explore the table option for loading as well, I always use a second step but this can be usefull as well.

Sergio

Hi, I just repeat the VMH sample and just add a custom step content to ask for the load on the fixed side and displacement in one node on the movil side (two node sets must be defined) to an external file, then plot the results on Excel to see the load deflection curve, where we can see clearly the non lineal behavieur and the permanent deflection (1mm) after the part is compleatly unloaded.

This is the custom step content:

********************************************************
*NODE PRINT , TOTALS=ONLY, NSET=MOVIL
U
*NODE PRINT , TOTALS=ONLY, NSET=FIXE
RF
********************************************************

I have added manually the 0,0 point and then extrapolate (linealy) the final point also at zero load.

barrti

Victor, VMH and Sergio

Thanks for the terrific response everybody.

Victor - I will post my liml and inp files below. I have cleared the solution data because the complete file is 1GB! It should show plastic strain data as peeq is in the inp file. Stresses and strains are shown but no plastic stress/strain.

Since this , I have gotten a much simpler model to show plastic strain. I don't know what the difference is..I did the same things (i think) in each model.

VMH and Sergio - thanks for your work. It worked great.

Sergio - I entered the custom step content but did not know how or where to enter the two node sets. Would you please be able to post the inp file? Where does the deflection data get saved?

Thanks again

barrti

I retried my model in the Liml file above in the last post using 100 time steps. It eventually froze the whole machine partway thru the process (about 10% I think). The solution seemed to be diverging and this froze all processes. I could not even use Ctrl-Alt-Delete!


This freezing has occurred three or four times while I have been playing with NL elastic-plastic models. Any ideas? The element count was approximately 31500 10 node tets using 53,300 nodes. Simpler models with less elements like VMH's above work fine.

I am guessing that much of the problem may lie in the model itself. If you look at where I have placed the force (along the Y-axis) near a sharp edge, it will result in a sharp lip forming as the metal distorts??

The top image with missing elements shows what the model looked like after it had crashed. Once I reopened it later, the bottom image shows the force placement.

Sergio

Hi Barrti, you just need to select all the nodes in the fixed side and create a new named selection, and one node in the movil and again create a new named selection. Then CCX will output the results in an external .dat file that you can import in Excel to plot.

Regards

Sergio

By the way, can I ask you why the mesh has this wierd shapes on the base? Have never seen before netgen giving such results.

barrti

Hi Sergio
Thanks for that. I will try it out tomorrow. I used automesh and then refined several times.

VMH

barrti, when running a full geometric and material nonlinear analysis with +50 steps and larger model, it requires a much stronger CPU and a fast solver. The CCX2.10_MT complied by kwip solve about 3 times faster than bConverged ccx 2.8p2 on my new machine. Windows 10 Pro, Intel i7-6820HQ, 32 GB RAM (for model in the range of 200k=300k nodes, only 50% of the RAM is used so for your case, it doesn't matter). You could try less number of steps and then increase from there to see if there are much different (just like mesh convergence study). Most of the time, you may find that you don't need to use that much steps to capture all of the critical nonlinearities. Again, this all depends on your model.

I remeshed your model (24313 nodes), reapplied the boundary conditions, and then rerun CCX by kwip using 6 threads (you can customized this on your machine to use multi-threads if avaiable). It took about 15-20min to run that model. My CPU was used about 78% at each iterations. See attachments. I couldn't attach the model with the results because it's about 450MB.

As for the refinement, I personally don't use the refine button unless it's a very simple model. I find that the changing the mesh density in the meshing option to be alot better and uniform and use the local refinement option to do local refine in area with higher stress gradient.

I was wondering how was the .step/.stp file be attached to your .liml file. I usually have to save and relink them each time when moving, which is a little inconvenience.

Victor, notice my screen is now cluttered which wasn't before in version 4 using the same setting.

barrti

VMH
Thanks very much for your effort and help. I'll try this out thankyou.

barrti

VMH and others

RE STP file - before I sent the liml file, I right clicked on "Solution" on the tree and clicked clear. That removed all the solution data and left everything else.

I found CCX2.10_MT from https://github.com/ddfem/ccx_mingw64 (kwip??) and ran it on your model previous post). It was really fast as you say and did the model in 9 minutes! I have an i7-3770K running at 4.2 Ghz with 32GB so thats about right. Thanks to you and kwip.

I then built my own 20mmx3mmx500mm steel flat bar model loaded with 25N on the end. I could not stop it diverging and quitting. In frustration I went back to ccx2.8 and still no good.

I've tried what I know. It seems to go divergent just about when it yields?

Thanks

barrti

Hi

I think that I've just solved my own problem. The solution diverges just after yielding I think because of the low Tangent modulus (2 GPa). It is 1% of the Youngs Modulus (200 GPa). Assuming that the force I have applied to the end of the metal bar provides more bending moment than is required to bend the bar, then at some point after yielding, the bending moment is excessive and the metal bar would accelerate if it could. This means that the solution process becomes unstable and divergence occurs.

Thats my guess anyway. If, I progressively reduce the force and hence the bending moment, then the solution gets closer and closer to finishing. At some point, I found that if the force is reduced enough, then the solution process completes.

Victor: Is it possible to apply a "follower force" to the bar that stays perpendicular to the bar? In this way, a constant bending moment can be applied? I could apply a pressure i Guess.

The motivation for this messing around is to see if I can use mecway/ccx for metal forming operations.

Another thing that the Calculix error message kept suggesting was to use "automated increments" or something similar. Is this easily implemented.

cheers

Victor

That sounds like a likely reason for not converging. Good to hear you got it working.


Yes, use pressure for a follower load.


Automatic time stepping is generally a good idea. To turn it on:

1) Right click CCX in the outline tree and click "don't generate keyword"

2) Choose *STATIC

3) Right click CCX in the outline tree and click "custom step contents"

4) Enter these two lines:

*STATIC
0.1,1

where 0.1 is the initial time step size and 1 is the total duration, both in seconds.

barrti

Thanks Victor,
I tried your suggestion exactly (*STATIC 0.1,1) and got what you see in the attachment. I also tried *STATIC 0.1,100 with the same result.

In Mecway, i specified 100 sec run time with 1 sec increments. Basically, the run finished very early.

Cheers

VMH

barrti,

In the analysis option for the convergence criteria, I noticed that you only have "Work" checked. Check either "Default" and "Work" (default) or "Displacement" and "Work" or "Force" and "Work".

Victor

The convergence are currently ignored for output to CCX. You would need to specify that as custom step contents using CCX keywords.

barrti

VMH and Victor

Thankyou for that. I ended up using
*Static
0.1,100
instead of
*Static
0.1,1
because the solution quit early.

VMH's tip of ticking Displacement and work in convergence criteria also fixed the issue

Thanks all for you input. I am now getting very large deflections with plastic strain.

Cheers

VMH

Great to hear that!

barrti

Hi Victor,
I must have missed this post "The convergence are currently ignored for output to CCX. You would need to specify that as custom step contents using CCX keywords. "

Do you mean that settings ticked in mecway for convergence are ignored when using ccx and that custom step contents using CCX keywords must be specified?

Is this described in the CCX manual? What are some of the keywords used?

Thankyou

Victor

That's right. CCX has a *CONTROLS keyword for convergence parameters. I've never used it and I don't think you should unless you have a very special type of problem. If something's not converging, then tweaking the tolerance often just covers over the problem rather than finding the real cause.

VMH

Victor, Thanks for letting us know on the convergence criteria in Mecway analysis option. I was under the impression that they were applicable to CCX because changing them did give different results when I tested them with barrti model.

barrti

Thanks gents

Victor

VMH, I had a look in the code and there's no use of convergence criteria for generating the .inp file. Perhaps you got different results when it didn't converge, where it could potentially give a very different result on each run due to numerical error.

VMH

Victor, thanks for your explanations and helps.