warning messages in implicit analysis

[DKGajjar]

hello everyone,

I am modeling the axisymmetric tube hydroforming of aluminium tube by implicit analysis, the pressure is varied upto 22 MPa
For higher pressure from 15 MPa onwards I get the warning messages
The strain increment has exceeded fifty times the strain to cause first yield at 1331 points
The plasticity/creep/connector friction algorithm did not converge at 877 points
Convergence judged unlikely. Increment will be attempted again with a time increment of 2.25508e-03
FORCE equilibrium accepted using the alternate tolerance.

I have tried using a fixed time increment of 0.0001 but job is aborted
Is there any problem in material properties or in the step?

Thank you in advance

 

[IceBreakerSours]

Check to ensure your units are consistent.

Are you new to this forum? If so, please read these FAQ:

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

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[DKGajjar]

I have double checked everything and I also read the previous posts regarding the same warning messages but it is not working,if I further decrease fixed time increment to 1e-5 it takes much time.

 

[IceBreakerSours]

Do you have a back-of-the-envelope or a hand calculation to use as a reference? Try stepping back (a few steps, if the need be) by making simplifications until the response makes perfect sense to you and then build layers of complexity on top of it, one at a time.

Are you new to this forum? If so, please read these FAQ:

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

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[DKGajjar]

thank you for your reply
I'll try your suggestion

 

[Mustaine3]

It seems that the material behavior and the load don't fit together. The load is too high or the material too weak.

Make sure that the maximum stress of your plasticity data isn't reached in the analysis.

 

[DKGajjar]

the peak stress is around 260 MPa but I am putting upto 280 MPa. I applied max load increment of 0.0005 and no warning occured(linear variation of load) but as I changed the amplitude curve warnings appear again. Do I need to adjust proper amplitude curve? everything seems fine otherwise

 

[Mustaine3]

What is the definition of your own amplitude? Maybe the load gets scaled up with that definition.

 

[DKGajjar]

For a step time of 1
amplitude curve is tabular type
time amp
0 0
1 1
no warning appears here for max load increment of 0.0005
now i changed the amp curve
time amp
0 0
0.4 1
1 1
warning appears here for max load increment of 0.00025

 

[Mustaine3]

In the second case the load is applied in a shorter time period, so with a higher rate. Depending on the analysis and other settings, that might create a different behavior. 'hard to say without knowing the model.

 

[jmetzy34]

Are you running it as an implicit static analysis or a quasistatic analysis using implicit dynamic? If you are running it as a static analysis, then the time period won't have any effect unless you are using material properties with rate-dependent plasticity. For instance, if your run your analysis with a time period of 1 s and it takes 2000 increments to solve, then each increment will be 0.0005 s. If you shorten the same exact problem to a time period of 0.4 s, it will still take 2000 increments to solve, and each increment will be 0.0002 s. So in this case, decreasing the time period does not speed up the analysis.

 

[DKGajjar]

Thank you for replies

I have resolved the warning problem by limiting the max time increment to 1e-4 but for peak pressure the mises stress is around 291.8 MPa and PEEQ = 0.2 whereas my input stress = 263 Mpa and strain = 0.25. I am not applying rate dependent plasticity, the material obeys hill's normal anisotropy so I have used potential for R11,R22,etc. how is this possible?

 

[jmetzy34]

Looking in the Abaqus Analysis User's Guide for 6.14 you can see in section 23.2.6 "Anisotropic yield/creep" an explanation of how hill's potential function is implemented. You will see that your input stress of 263 MPa is the user defined reference yield stress σ⁰. So depending on the values you've used for the yield stress ratios, R11, R22, etc., it will have the effect of either increasing or decreasing the computed von Mises stress versus the computed von Mises stress without using the yield stress ratios and only the reference yield stress. So if you reran the analysis without the yield stress ratio's, you would get results that line up with your input stress and strain values.