Creep calculation and results

For the creep calculation, I have had a problem with Calculix results comparing with Abaqus results.
In this example, the Abaqus results for the PE seems seasonable. But the Calculix results for PE (CEEQ) are not right. I appreciate it very much if someone can have an answer. Is this a bug from Calculix?
The .INP file is following:
BASIC VERIFICATION OF CREEP (CREEP TEST)
*NODE
1,1.,0.
2,2.,0.
101,1.,10.
102,2.,10.
*NSET,NSET=BOT
1,2
*NSET,NSET=TOP
101,102
*NSET,NSET=LEFT
1,101
*ELEMENT,TYPE=CPS4
1,1,2,102,101
*ELSET,ELSET=DATTIM
1
*ELSET,ELSET=CREEPERS
1
*SOLID SECTION,ELSET=DATTIM,MATERIAL=A1
*MATERIAL,NAME= A1
*ELASTIC
20E6,.3
*PLASTIC
0.,0.
0.,10.
*CREEP,LAW=NORTON
2.5E-27,5.,-0.2
*BOUNDARY
BOT,2
LEFT,1

*STEP
*STATIC
1.0E-7,1.0E-7
1,P3,-20000.
*EL FILE,FREQUENCY=20
SDV,
S,
CEEQ
*NODE FILE, FREQUENCY=20
U
*END STEP
*STEP,INC=25000
** STEP 2 ----- CREEP TEST
*VISCO,CETOL=5.E-5
1.e-7,10000.,1.E-10
**PRINT,FREQUENCY=5,RESIDUAL=NO
*EL PRINT,ELSET=CREEPERS,FREQUENCY=20
SDV,S
CEEQ,
*EL FILE,ELSET=CREEPERS,FREQUENCY=20
SDV,S,CEEQ,
*NODE FILE,FREQUENCY=20
RF,U
*END STEP

By the way, The Calculix is not easy to get convergence solutions. It may need to change the CETOL or the initial step value for *VISCO.
Thanks.

What are the exact differences ? Which CalculiX version and solver (Spooles, Pardiso, PaStiX, other) do you use ?

The ccx analysis run from this input file doesnâ€™t converge so we canâ€™t evaluate the results. If you obtained the results for the same simulation setup in both Abaqus and CalculiX then please share the appropriate input file.

Have you tried using different element types, like a hexahedron typically used for single element tests of material behavior (with symmetry BCs applied) ?

I use Calulix v2.17 with Pardiso solver.
Change CETO = 5.e-4, it can be run through.

The PE results are very large and more than 100. In fact, the exact solution for 10000 s, the PE from Abaqus is 0.1.

I use Calulix v2.17 with Pardiso solver.
Change CETO = 5.e-4, it can be run through.

The PE results are very large and more than 100. In fact, the exact solution for 10000 s, the PE from Abaqus is 0.1.

Zhifa

CETOL in *VISCO. Typo.
For Calculix v2.18, it cannot run through for all time but the first a few iterations for *VISCO step will be convergence. However, the PE value is very large. and the stress also is not changed with time. That is not right.
Thanks.

For ABAQUS run, it only need to change the *CREEP, LAW=TIME

After changing CETOL to 5.e-4 it still doesnâ€™t run to completion in ccx 2.17, at least when using Spooles solver. It stops on total time = 0.997577E-03. Where are these creep constants taken from ? Inputs for this analysis may require some modification so that tests can be carried out using different solvers without issues.

Calc_em:
I get this from this site,
https://abaqus-docs.mit.edu/2017/English/SIMACAEBMKRefMap/simabmk-c-creep.htm
It has the closed form solution for this problem.
I think it may not be the solver issue.
Thanks.

Disla:

I am very carefully checking the time unit. The time unit in the creep calculation should be independent with the motion time unit. It is only the calculation procedure time as I understand, so it will be consistent with the Norton lawâ€™s time unit.
The Abaqus results are consistent with the graph even at T=10s.
This is a very simple problem. The closed form solution can be found:
https://abaqus-docs.mit.edu/2017/English/SIMACAEBMKRefMap/simabmk-c-creep.htm
The strain and stress in Calculix are very strange, they are not changed with the creep time that are totally different with Abaqus results.
Thanks.

Calc_em:

Do you know which part in Calculix doing the creep calculation? I just notice the reading Creep file and didnâ€™t find where the creep calculation do the analysis.
I think it very possible there is something wrong in creep calculation. For this example, the convergence should not be very difficulty. For a creep solution, most time it is still a static solution, not a dynamic solution.
Thanks.

Recently, I was working on a creep analysis with more complexity (thick cylinder subjected to internal pressure, example based on another part of Abaqus documentation) and the results obtained with CalculiX were in very good agreement with the analytical solution. So I donâ€™t think that the creep procedure in ccx is incorrect. In your case, thereâ€™s probably some error or itâ€™s just a matter of adjusting the settings until convergence is obtained (I must admit that CalculiX seems to have convergence issues in cases that Abaqus can solve without struggling but it should be possible to overcome these problems).

Calc_em:
When you works on the cylinder creep, have you checked this model also in the Abaqus example?
https://help.3ds.com/2019/english/DSSIMULIA_Established/SIMACAEBMKRefMap/HelpViewerDS.aspx?version=2019&prod=DSSIMULIA_Established&lang=english&path=SIMACAEBMKRefMap%2Fsimabmk-c-creepthickcylinder.htm&ContextScope=all&id=8dd61073fec24b1ab3f47b8a24c6f928
I still cannot run a correct answer for this model.
The creep solution from Calculix is very strange.
Thanks.

Calc_em:

Do you have any good idea to do the creep analysis in Calculix?
Thanks.

Here are the results for a modified version of a thick cylinder example obtained with CalculiX (PrePoMax as pre- and postprocessor) and Abaqus, respectively:

As you can see, thereâ€™s a very good agreement.

In fact, creep analyses are hard to converge in CalculiX (and sometimes in Abaqus). Keep in mind that Abaqus uses special integration scheme (explicit mixed with implicit) for such simulations and CalculiX doesnâ€™t offer this capability.

1 Like

Calc_em:
This result looks good. However, for my such a simple model, the Calculix cannot get a reasonable solution. It is really unbelievable.
Thanks.

If you need some simple working example of creep calculation in CalculiX, check the beamcr.inp file in test examples database. Verification cases available in Abaqus documentation were designed to be solved without issues in that software (using its specific mixed integration algorithm). Itâ€™s true that there are convergence issues when trying to solve them in CalculiX but I think that proper modification of settings (mesh, incrementation parameters and other inputs) would let you get expected results. Iâ€™ve noticed that, for example, some elements in CalculiX give incorrect results when plasticity is defined and the user should change the element type or increase the number of elements. Maybe thatâ€™s also the case with creep.

If you have any input file that works in both CalculiX and Abaqus (runs to completion without stopping before the specified step time due to convergence issues) but gives incorrect results in CalculiX then please share it and I will keep running tests to see if it can be fixed.

Calc_em:

Yes. I have this example that can run through both Calculix and Abaqus, but the results are different. The Abaqus results are exactly the closed form solution, but the Calculix results are not good.
Thanks.

(Attachment Creep_mises.inp is missing)

(Attachment Creep_misescurve.inp is missing)

BASIC VERIFICATION OF MISES CREEP AND PLASTICITY INTEGRATION
*NODE,NSET=ALLN
1,0.,0.
2,1.,0.
3,1.,1.
4,0.,1.
*ELEMENT,TYPE=CPS4,ELSET=ALLE
1,1,2,3,4
*SOLID SECTION,ELSET=ALLE,MATERIAL=ALLE
*MATERIAL,NAME=ALLE
*ELASTIC
20.0E6,0.3
** Include hardening data *PLASTIC
*INCLUDE,INPUT=creep_misescurve.inp
*CREEP, LAW=NORTON
2.5e-23,5,-0.2
*BOUNDARY
** 1,PINNED
1,1,3
2,2
4,1
*AMPLITUDE, NAME=RAMP
0.0,0.0,50.0,0.5,100.0,1.0
**
*STEP, INC=20000
*VISCO, CETOL=1.0e-4
** 0.01,100.
0.00001,100.
1,P3,-20000.
*NODE FILE, FREQUENCY=20
U
**EL FILE,frequency=20
** PE,CE,E,EE,
**OUTPUT,FIELD,VARIABLE=PRESELECT,FREQUENCY=9999
**OUTPUT,HISTORY,Frequency=1
**ELEMENT OUTPUT, ELSET=ALLE
*EL FILE,ELSET=ALLE ,FREQUENCY=20
S,CEEQ,E
**CONTROLS,PARAMETERS=FIELD
**,0.0,
*END STEP

https://help.3ds.com/2019/english/DSSIMULIA_Established/SIMACAEBMKRefMap/simabmk-c-creep.htm?ContextScope=all&id=3465e08584b4486a9ea6493edeb2259f#Pg0

You can get the plastic curve file from this site.
Thanks.

With the default settings, it doesnâ€™t converge in CalculiX (no error message, just stops after a few increments). Interestingly, it runs to completion when CETOL is decreased to 1e-5 (I expected the opposite behavior).

Stress is correctly calculated in both programs but the strain is wrong in CalculiX. The element used here is CPS4, I would definitely try with more accurate types of elements and finer meshes - that might be the key to getting correct results here. I try to solve this using mesh consisting of 8x8 CPS8R elements but so far itâ€™s not converging.

By the way, note that if you request CEEQ in CalculiX, it becomes internally converted into PEEQ (according to the documentation, the viscoplastic theory doesnâ€™t distinguish between the two). But in Abaqus, you get both CEEQ and PEEQ and their values differâ€¦