Have you come across this error-"DURING THE CONVERSION FROM CRUSHING TO PLASTIC STRAIN Abaqus FOUND NEGATIVE AND/OR DECREASING VALUES OF PLASTIC STRAIN. VERIFY THAT THE DEGRADATION DATA UNDER *CONCRETE COMPRESSION DAMAGE IS CORRECT?"
DURING THE CONVERSION FROM CRACKING TO PLASTIC STRAIN Abaqus FOUND NEGATIVE AND/OR DECREASING VALUES OF PLASTIC STRAIN. VERIFY THAT THE DEGRADATION DATA UNDER *CONCRETE TENSION DAMAGE IS CORRECT
How to overcome this error , I was trying to replicate the problem as mentioned in the attached paper
That error occurs when the equations to calculate the plastic strain gives a negative or a value smaller than the inelastic strain.
To avoid it you need to calculate the plastic strain using the equation and check that the value are always ascendant. remember that the first line of damage parameter and inelastic strain needs 0 as values, so develop the rest of the points based on the coordinates of your 0 inelastic strain point with no damage.
this error is related to to concrete damage which you filled
in your case you did mistake in both Tension damage, and compression damage
you have to calculate that carefully, by using Loading-unloading compression test then calculate the compression damage factor and the tension damage factor
in case that you couldn't do it may i can give you a ready computed data
the error is related to the damage input . If having the damage in your simulation is not required, you can simply solve this issue by deleting concrete compression damage.
@Mohammad Samaaneh, I have the same problem, can you give me a ready computed data for check ?
@Unnikrishnan Bm - Were you able to resolve this matter ? I have also come across a similar issue , unfortunately.
"DURING THE CONVERSION FROM CRUSHING TO PLASTIC STRAIN Abaqus FOUND NEGATIVE AND/OR DECREASING VALUES OF PLASTIC STRAIN. VERIFY THAT THE DEGRADATION DATA UNDER *CONCRETE COMPRESSION DAMAGE IS CORRECT?"
cracking strain = (total strain) - (total stress)/E0
plastic strain = (cracking strain) - (d*(total strain))/((1-d)*E0)
E0 - Elastic modulus
total strain and stress values as given in the txt file attached
I have checked the plastic strain values prior to adding them in ABAQUS. If I use the same values in the txt file the plastic strain fluctuates around a very small value 10^-20 (expected).
This value can sometimes be negative or positive. So I round the total strain and stress values to around 6 decimal places and input the values to ABAQUS.
But the problem still persists.
Regards
Dear Unnikrishnan Bm,
This error due to the plastic strain is negative and/or descending values. So must be a check on the value of ɛc pl damage attached in Figure and the values of (dc and dt) = 1-(stress of descending part / stress due to undamped response).
Kind Regards
Waleed
Agree with Alireza Afaghi ... and Mohammad Samaaneh ...
Good question.. Please share me the best answer might you trust...
Regards…
That error occurs when the equations to calculate the plastic strain gives a negative or a value smaller than the inelastic strain.
To avoid it you need to calculate the plastic strain using the equation and check that the value are always ascendant. remember that the first line of damage parameter and inelastic strain needs 0 as values, so develop the rest of the points based on the coordinates of your 0 inelastic strain point with no damage.
Hi Dilina Dissanayake ,
I am working on similar concrete material card. In the attachment that you shared above, is that the *concrete compression hardening that you used in your model ?
If so, Is that the correct way to enter the strain rate dependent data ? I have compression stress strain data at 4 different strain rates. The curves are much stiffer as the strain rate increases. How do we input this kind of strain rate dependent data in Abaqus concrete damaged plasticity model? I tried to arrange the stress in ascending order then strains were off.
And when I tried to arrange strains in ascending order, the stresses were not in ascending order .
When I selectively picked data so that strains are in ascending order , stresses are also in ascending order , then the strain rates are not in ascending order. How to input strain rate dependent hardening data in Abaqus ?
PS: Any help will be greatly appreciated.
Thanks,
Vaidehi
Hi, I had the same problem, and after checking that damage values, crushing strain values and plastic strain values were all positive and in ascending order, I removed all the values of the damage parameter greater than 0.98, and the error message disappeared. Also try to ensure that the diference between two consecutive values of the damage is greater than 0.001
- Badges
- Science topic