You are not logged in. Please login or register.
Cervenka Consulting Forums → ATENA → Error Massage
Pages 1
I am using Shell/Plate layer for FRP sheet at bottom of beam, as sujessted in ATENA 3D user manual, I followed the prosedure.
At 396 Analysis Step, following massage came.
CCMaterials Extended AExc:
CC5ParamYield F: project_stress_on_f_division by zero.
What should I do?
Thank You
Hard to say without seeing your model...
Somewhere in post-peak this can happen. It basically means there is very large damage in a material point. Are you really interested in results in that step and later, or is the structure already almost destroyed?
If this happens at an early stage, the reason is usually a too long loading step, or wrong boundary conditions. It also might be too high local damage (regionally restricted - far before global failure). In that case, we should be able to help you modify the material or solution parameters to prevent/reduce the numerical problems.
Thank you
Actually after howmuch load step I have to stop! It is very difficult to juge from the result, as different beam requires different analysis step, Weather from the graph I have to predict that my beam is failed or is there any other criteria.
Is there any provision in ATENA that, it stop the work by providing massage.
Also, after each step. The massage come
(*) Warning convergence criteria not satisfied.
Is this warning effects the results.
The dicision where to stop of course depends on the type of problem and of the kind of results you are interested in.
Basically, if you are interested in the max. load and you see in the monitor L-D graph that the force/reaction has reached the peak and decreases, you can stop.
Please read the paragraph "I get the warning "Convergence criteria (within line search) not satisfied due to eta limit, continuing superordinate iteration" during analysis, what does it mean?" in the Known Issues page of our Web (Products » ATENA » Known problems)
http://www.cervenka.cz/products/atena/known-problems
thank you
there is an another error generated, when I was interested for generating FE mesh int the beam.
an internal error has occured
ID: A3 MasterSlave.pas/13
Module: C/PROGRA~1/CERVEN~1/ATENAV4/A3Pre_1.dll
If I am continuing with out solving this error, then massage comes
(x) Internal error while preparing mesh generator input!
Group3 i.e. Steel plate which is attached to beam for loading, not generated.
I am afraid it is not possible to determine the problem source without seeing the model. Please send it to our general support email (cervenka@...).
Sir,
I also face similar problem when this massage appear
CCMaterials Extended AExc:
CC5ParamYield F: project_stress_on_f_division by zero.
I model the 3D RC Square RC column and introduced the swelling at load case in the concrete to mimic the effect of expansion. I tried with value of swelling of 0.001 and 0.002 (strain), Atena can complete the analysis, beyond the value 0.002 Atena unable to complete the analysis.
Please help.
Well, I can only say the same as in a previous message in this thread (2010-09-02 11:04:43) - hard to guess without seeing the model.
In how many steps do you apply the swelling strain? 1 per mill = 1000 microstrain is already quite a lot - you may need more than 10 load steps for that. And, of course, double the number of steps when you apply two times more strain.
Hello Everybody,
seeing your discussion about the CC5ParamYield F: project_stress_on_f_division by zero problem, I want to comment on the following. This error means the following:
- the stress is so far outside the failure criterion that it cannot compute the return direction to return to the failure/yield surface.
The cause of the error is usually due to:
- either wrong definition of material parameters, if you modified some parameters by hand manually then you should check
if your compressive strength or tensile strength or the onset of the compression FC0 are meaningfull. If your parameters were
generated by ATENA, this is not probably the reason.
- the next reason is the divergence of your problem. Due to divergence of the solution, the stresses are now so big that the program
cannot find a solution. The reasons for divergence could be again many, but most common situations are:
- wrong boundary conditions
- wrong loading, load is for instance applied at a single point and not distributed by some loading plate. Please, understand
that in reality there is nothing like a point load or support. Point load or support is a singularity and your stresses will
go to infinity there if you make a sufficiently small mesh.
- loading is applied by too large steps
- loading is so high the structure cannot survive it. Then you should use and arc-length method or check the expected load
level and reduce the load.
Well if you are not able to solve the problem, I suggest that you send us your input file, without the results and we can
check what is wrong.
Regards
Jan Cervenka
Dear Sir,
I tryed to model the Beam with
external cables (EXTC), as it is
explained in the example manual,
but there are some errors and the
analysis can't be executed.
Also when I try to change the messing
to some macroelements, there is an
internal error.
I have already send to the cervenka@
an e-mail with my model and a pdf with
the error messages.
Thank you for your time.
Please understand that loads are incremental in ATENA. In the model, you apply the prestressing and prescribed displacements in all steps, which means you increase both the cable stress and the deformations at the same time.
Regarding the warnings, I recommend to read about the Conditional Break Criteria in section 3.8.5.1 Solution parameters of the ATENA 3D User's Manual.
With respect to the meshing, there are joints which do not belong to any line. Basically, there are 2 ways to include the loading point in the loading plate macroelement:
1. compose the top surface from 2 or 4 surfaces, such that the loading point belongs to the lines composing the surfaces. This will not allow using brick elements for the plate, but it is usually not a problem.
2. (as in some of our examples) the point does not belong to any line of the ME. Then, you have to pay attention that the generated mesh has a node at that point.
In any case, it does not make sense to divide the plate into 2 macroelements.
Regards,
Pages 1
Cervenka Consulting Forums → ATENA → Error Massage
Powered by PunBB, supported by Informer Technologies, Inc.
