I'm having problem with ABAQUS simulation of shell model

[fariz838]

Hi everyone...

I'm rookie to this forum. I'm having problem with my simulation of shell element for ABAQUS. I'm currently doing a heat transfer analysis. I keep getting this error: ERROR: ***TIME INCREMENT REQUIRED IS LESS THAN THE MINIMUM SPECIFIED and ***TOO MANY ATTEMPTS MADE FOR THIS INCREMENT.

Currrently, I modeled an I-steel beam beam that were expose to standard fire curve which is time temperature dependant. on top of the beam is concrete slab. But the concrete slab does not contribute to the analysis. It acts as a attachment to the beam. For material properties of the steel, I included conductivity, density, elastic, plastic,specific heat. for predefined fields, i included initial temperature of 21 degree Celsius. In assembly module, i created instances to attach together all the parts to become the I-beam.

For the heat transfer step, I included:

Step, name="Heat transfer", nlgeom=NO, inc=1000
*Heat Transfer, end=PERIOD, deltmx=10., mxdem=0.5
1., 3600., 1e-05, 500.,

For boundary conditions, I included:

Name: BC-3 Type: Temperature
*Boundary, amplitude=Amp-1
Set-4, 11, 11, 1000.

For loads, I included:

Name: Load-1 Type: Surface heat flux
*Dsflux, amplitude=Amp-1
Surf-12, S, 1000.

I would really appreciate if anyone could help me with these problems of ABAQUS. Many thanks again.

Cheers.

 

[corus]

Presumably you have temperature dependent material properties. Check you have the right units and not made a mistake in the definition.

 

[fariz838]

Thank's again corus for your reply. I will look into detailed the material definitions for both steel and concrete.

 

[rogersma]

Check this man page:
[URL unfurl="true"]http://www.egr.msu.edu/software/abaqus/Documentation/docs/v6.7/books/key/default.htm?startat=ch08abk03.html[/url]

 

[fariz838]

I have check all the units to be consistent but does not help the model to converge. I use transient step due to fire effects. For the nlgeom, were switch off. In the load step, I apply body heat flux that were exposed with with fire temperature dependent in Amplitudes. Also, I apply temperature boundary conditions for the whole beam using temperature dependent in Amplitudes. In the load step,

A SUGGESTED INITIAL TIME INCREMENT OF 1.00
AND A TOTAL TIME PERIOD OF 3.600E+03
THE MINIMUM TIME INCREMENT ALLOWED IS 1.000E-05
THE MAXIMUM TIME INCREMENT ALLOWED IS 100.

THE SIZE OF THE TIME INCREMENT IS CONTROLLED BY -
THE TEMPERATURE CHANGE PER INCREMENT NOT EXCEEDING 10.0

In the mesh step, I have refine the mesh up global size = 0.01. Previously, i use more course mesh and still getting the same error. I have no idea what when wrong with the simulation.

Thanks

 

[corus]

The increment used must be less than the value of 10 you specified. Try changing that.

 

[Mustaine3]

That value means that between increment x and x+1 no node can have a larger temperature change than 10 degree. Maybe that value is too low when a very fast and large change in temperature happens in your model.


>Also, I apply temperature boundary conditions for the whole beam using temperature dependent in Amplitudes.

I hope you mean it different than you've written that. Because when you apply temperature BC, the temperature cannot change free on those regions. So any loads or film conditions will be useless, since you assign the temperature.
It's like fixing all movement in a structural model. A load cannot deform such a body.

 

[fariz838]

Hi Corus and Mustaine3...

I was able to overcome the problem and manage to get the results. Seems to be the problems comes from the fire load configuration applied on the beam surface. Thanks again for your help. I added contact stabilizer and interaction properties due heat contact. The model was finally converge. But, now I'm having another problem. When I want to retrieve the beam temperature against time, the value of the temperature was negative value. I added predefined field which refers to initial temperature condition of 21 degree Celsius for each of the beam surface. I was able to increase the maximum negative temperature to positive temperature but below than 10 degree Celsius. I also applied cavity radiation on all the beam surface due to warning sign (no cavity contact define) when the Job 1 was completed. Do you have any idea to help me this problem?
Really appreciate again to help to solve this problem.

Thanks

 

[corus]

In very rapid transients you can get some initial instability in the temperatures, perhaps even showing negative values. These eventually prove to be more stable as time goes on. For these initial changes in temperatures, perhaps where you've fixed some boundary condition to instantly change in temperature, then you'd need a very very small time step to capture this change. Alternatively, apply a boundary condition so that the change in temperature is ramped up over a small period.