i am applying a load of 50KN gradually on a reinforced concrete beam,
i'm unloading this load using an amplitude to get the loading and unloading versus deflection graph.
i have used concrete damaged plasticity to model concrete.
the problem is with the run , it has reached the maximum load but after few increments in the unloading stage i have got this message "too many attempts made for this increment"
noting the problem was in the loading stage first , but i played a little with the solution controls, so it delayed this message to the unloading stage.
what i have done is as the following:
changed the solution technique from full newton to quasi newton
used discontinuous analysis in the time increment
in search algorithm , i have changed N from default of 5 to 10 and etha(accuracy) from 0.1 to 0.01
in the attached figure, the analysis stops at 0.56029 sec which is in the unloading stage.
attached is the displacement vs time graph , as you can see after 0.5 seconds (where the unloading starts and the deflection starts to decrease) the graph stops at 0.56029 sec because of the message that i have got that error message.
what to do?! i need help please
How did you define the load?with tabular amplitude or smooth amplitude?
@behnam Karami
Tabular load
0 0
0.5 1
1 0
This means that the first 0.5 seconds represents loading, and from 0.5 sec to 1sec represents unloading
change tabular load to smooth load and increase amplitude date.sometimes it can be effected. check this.
oh okay i will change it to smooth load and see what happens
but what do you mean with amplitude date?
you mean amplitude time not amplitude value , right?
Look at the final warning message; that may give you a hint of what is going wrong (deformation too large, material calculation not working etc.)
"played a little with the solution controls"
Which controls did you touch? Do not touch the precision of the field calculation unless you know exactly what you are doing and how this will affect your results.
Please check job diagnosis to figure out the type of the error you have in your model. and try viscous parameter to improve the convergence if necessary. What viscosity parameter for concrete did you use?
Dear yasmeen
your model show divergence and according to my experience this most probably due to the parameters of CDP you used. please don't make any change in solution control it wouldn't help much. what kind of step are you sing ? is it dynamic implicit or explecit or general static. contact me for details
best of luck
Dear Yasmeen Ghassan,
Decrease initial and minimum increment value.
thank you all for your great suggestions
what i have done in the last couple days is that i have used stabilization with damping ration option and it worked!
but now i'm facing new problem , i have small deflections compared to literature, i increased my damping factor and the deflections got better, but still not really accurate.
how much should i decrease my damping factor? noting that that when the more i decrease it the longer time it takes to get results.
i read in one of the forums that there is energy output calculation that would help me to determine the accurate value of damping ratio
what should i do now?
@Rafaat E S Ismael
thank you for your reply professor, it is static general, i have used stabilization option with damping factor and it worked but my problem now is how to choose this damping factor to get accurate deflections? as explained in my comment above
@martin Beaker
thank you for your answer, i've got my solution controls back to default, i have solved the convergence problem with stabilization option, my step is static general, but now i'm facing another problem as described in the above comment
JD Nzabonimpa
i'm using 0.01 as viscosity parameter , i noticed when i decrease it the run takes very long time!!
what do you recommend , my problem is 5 m simply supported beam with 50 KN static load at its L/3 length , the load is increased gradually using an amplitude.
beam is T section with 650mm flange width and 415 mm web height.
i will add another 50KN at its 2L/3 location later.
i want to verify the deflections with literature.
Dear Yasmeen
how are you? sorry to be late in answering you cause i was in vacation.
have you solved your problem?
i can send you my lecture which may help you. we compared abaqus results with experimental data for several simply supported RC beam. we used 2-D and 3-D
my students submitted the final report about these comparisons with deteailed steps
@Raafat E S Ismail
thank you for your reply!
well yeah i have solved the probelm
I have used is stabilization option in the static step using damping factor, i have used a very small damping factor so it wouldn't affect deflections.
it really worked!
yeah i would love to if you can send me a copy of these comparisons! it would be a really good insight
thank you
You can try:
1. Increase IA (Step-Other-General solution control-edit step-specify-Time increment-more- change IA to the maximum value 30)
2. Refine the mesh in the contact regions to reduce the percentage of elements flipping in and out of contact.
3. Using mass scaling in Dynamic/Explicit to control the stable time increment.
- Badges
- Science topic
- Similar topics
- Mathematical Sciences
- Graphs