Abaqus 6.10 - Abaqus/CFD and Abaqus/Standard Co-execution problem 4

[Jlog50]

I have two model in one Abaqus/CAE model. One is an Abaqus/Standard structural model and the other is a Abaqus/CFD fluid model.

In both models I have selected the fluid-structural interaction surfaces and defined those surfaces as "Fluid-Structure Co-simulation boundary" in step 1 for the structural model and step 1 for the fluid model.

I am trying to run a co-execution but when I try to run the analysis I obtain an error message saying....

"There is no active Fluid-Structural co-simultation boundary interaction defined in model Model-1_Struct.

The input file was not generated, and the co-execution was not submitted."

I am new to Abaqus 6.10 and would really appreciate some input. Thanks.

 

[Jlog50]

Anyone else come across the problem describe below, any input would be much appreciated, thanks.

 

[Jlog50]

Here is the relevant part of my input file, is there anything in the interaction section causing the problem described above, thanks.

**
** STEP: Step-1
**
*Step, name=Step-1, nlgeom=YES
*Static
0.5, 0.5, 5e-06, 0.5
**
** BOUNDARY CONDITIONS
**
** Name: Pipe Type: Displacement/Rotation
*Boundary
_PickedSet12, 1, 1
_PickedSet12, 2, 2
_PickedSet12, 3, 3
_PickedSet12, 4, 4
_PickedSet12, 5, 5
_PickedSet12, 6, 6
** Interaction: Pipe
*Co-simulation, name=Pipe, controls=Pipe_Ctrls, program=ABAQUS
*Co-simulation Region, type=SURFACE
Fluid_co,
*Co-simulation Controls, name=Pipe_Ctrls, time incrementation=subcycle
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field, variable=PRESELECT
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step

 

[Jlog50]

Hello all,

I have been through the Abaqus documentation with no progress to solving this problem, I have attached the CAE file and Input file at the following link

http://my.engineering.com/pg/file/Jlog50

Any input would be much appreciated.

 

[rstupplebeen]

Check with your local office. I'm sure they have a couple of toy problems that they have worked though. I personally have not had time to dig into Abaqus/CFD or FSI and I assume most others have not also. Sorry for the bad news. Please post any progress you make though.

Rob Stupplebeen

 

[tgrimley]

Can you do a Abaqus/Standard-Static? co-ex with CFD? Does it require Explicit?

 

[Jlog50]

As far as I understand and according to the abaqus manuals you can go abaqus/standard with Abaqus/CFD. Thanks for your input. Apart from the inlet example on the abqaqus 6.10 promotional video from Simulia, I can't seem to find any other example like it or anyone apart from Simulia who have used Abaqus/Standard with Abaqus/CFD fror a co simulation.

Thanks again

 

[oriol]

Well, I was testing quickly how is co-simulation working on an example last week. I succeeded runing it but still a lot to do in order to get what I really want but if it helps, here you go:

.inp for CDF:
*Surface, type=ELEMENT, name=_PickedSurf7, internal
__PickedSurf7_S4, S4
__PickedSurf7_S6, S6
__PickedSurf7_S5, S5
__PickedSurf7_S3, S3
*Elset, elset=_PDF_WholeModel, internal, instance=Fluid-1, generate
1, 13298, 1
*End Assembly
**
** MATERIALS
**
*Material, name=Material-1
*Density
1e-09,
*Expansion
0.0008,
*Specific Heat, type=CONSTANTPRESSURE
4.21e+06,
**
** PREDEFINED FIELDS
**
** Name: Predefined Field-1 Type: Fluid density
*Initial Conditions, type=Density
_PDF_WholeModel, 1e-09
** Name: Predefined Field-2 Type: Fluid thermal energy
*Initial Conditions, type=TEMPERATURE, Element Average
_PDF_WholeModel, 300.
** ----------------------------------------------------------------
**
** STEP: Step-1
**
*Step, name=Step-1
*CFD, incompressible navier stokes, energy equation=TEMPERATURE
0.01, 0.3, 0.025, 0.45, 1
1e-10, 0.5, , , 0.5
*Momentum Equation Solver
50, 2, 1e-05
*Pressure Equation Solver
250, 2, 1e-05
ICC, 1, 1, CG
*Transport Equation Solver
50, 2, 1e-05
**
** BOUNDARY CONDITIONS
**
** Name: BC-1 Type: Fluid inlet/outlet
*Dsload
_PickedSurf5, P, 16.
*Dsload
_PickedSurf5, TEMP, 300.
** Name: BC-2 Type: Fluid inlet/outlet
*Dsload
_PickedSurf6, P, 0.
** Name: BC-3 Type: Fluid wall condition
*Dsload
_PickedSurf7, VELX, 0.
_PickedSurf7, VELY, 0.
_PickedSurf7, VELZ, 0.
**
** LOADS
**
** Name: Load-1 Type: Gravity
*Dload
, GRAV, 9810., 0., -1., 0.
** Interaction: Int-1
*Co-simulation, name=Int-1, controls=Int-1_Ctrls, program=MULTIPHYSICS
*Co-simulation Region, import, type=SURFACE
_PickedSurf4, TEMP
*Co-simulation Region, export, type=SURFACE
_PickedSurf4, HFL
*Co-simulation Controls, name=Int-1_Ctrls, coupling scheme=gauss-seidel, time incrementation=lockstep, time marks=yes,
step size=min, scheme modifier=lag
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field
*Node Output
DENSITY, PRESSURE, TEMP, TURBNU, U, V
*Output, history, frequency=0
*End Step


.inp for standard:
**
** MATERIALS
**
** SA182 Gr F304 or 316
** SA351 Gr CF8A or CF8M
*Material, name=Austenitic_High_Alloy_Steel_COL
*Conductivity
14.5, 21.11
14.5, 37.78
15., 65.56
15.4, 93.33
15.8, 121.11
16.2, 148.89
16.5, 176.67
17., 204.44
17.3, 232.22
17.7, 260.
18.1, 287.78
18.5, 315.56
18.9, 343.33
19.2, 371.11
19.6, 398.89
20., 426.67
20.4, 454.44
20.7, 482.22
21.1, 510.
21.5, 537.78
22., 565.56
22.3, 593.33
22.7, 621.11
23., 648.89
23.5, 676.67
23.9, 704.44
24.2, 732.22
24.6, 760.
24.9, 787.78
25.4, 815.56
*Density
7.92e-09, 21.11
7.91784e-09, 37.78
7.91421e-09, 65.56
7.91055e-09, 93.33
7.90686e-09, 121.11
7.90314e-09, 148.89
7.8994e-09, 176.67
7.89564e-09, 204.44
7.89186e-09, 232.22
7.88805e-09, 260.
7.88423e-09, 287.78
7.88038e-09, 315.56
7.87651e-09, 343.33
7.87263e-09, 371.11
7.86872e-09, 398.89
7.86479e-09, 426.67
*Elastic
209601., 0.3, -198.33
206153., 0.3, -128.89
202706., 0.3, -73.33
195122., 0.3, 21.11
190985., 0.3, 93.33
186848., 0.3, 148.89
183401., 0.3, 204.44
179953., 0.3, 260.
175127., 0.3, 315.56
170990., 0.3, 371.11
166164., 0.3, 426.67
*Expansion
1.64e-05, 21.11
1.65e-05, 37.78
1.67e-05, 65.56
1.68e-05, 93.33
1.69e-05, 121.11
1.7e-05, 148.89
1.72e-05, 176.67
1.73e-05, 204.44
1.74e-05, 232.22
1.75e-05, 260.
1.76e-05, 287.78
1.77e-05, 315.56
1.78e-05, 343.33
1.79e-05, 371.11
1.8e-05, 398.89
1.81e-05, 426.67
*Specific Heat
4.7201e+08, 21.11
4.7592e+08, 37.78
4.8178e+08, 65.56
4.8743e+08, 93.33
4.9334e+08, 121.11
4.9933e+08, 148.89
5.0696e+08, 176.67
5.1069e+08, 204.44
5.185e+08, 232.22
5.2428e+08, 260.
5.2786e+08, 287.78
5.3347e+08, 315.56
5.3928e+08, 343.33
5.447e+08, 371.11
5.5058e+08, 398.89
5.5394e+08, 426.67
** SA182 Gr F304 or 316
** SA351 Gr CF8A or CF8M
*Material, name=Austenitic_High_Alloy_Steel_COL_sup
*Conductivity
14.5, 21.11
14.5, 37.78
15., 65.56
15.4, 93.33
15.8, 121.11
16.2, 148.89
16.5, 176.67
17., 204.44
17.3, 232.22
17.7, 260.
18.1, 287.78
18.5, 315.56
18.9, 343.33
19.2, 371.11
19.6, 398.89
20., 426.67
20.4, 454.44
20.7, 482.22
21.1, 510.
21.5, 537.78
22., 565.56
22.3, 593.33
22.7, 621.11
23., 648.89
23.5, 676.67
23.9, 704.44
24.2, 732.22
24.6, 760.
24.9, 787.78
25.4, 815.56
*Density
7.92e-09, 21.11
7.91784e-09, 37.78
7.91421e-09, 65.56
7.91055e-09, 93.33
7.90686e-09, 121.11
7.90314e-09, 148.89
7.8994e-09, 176.67
7.89564e-09, 204.44
7.89186e-09, 232.22
7.88805e-09, 260.
7.88423e-09, 287.78
7.88038e-09, 315.56
7.87651e-09, 343.33
7.87263e-09, 371.11
7.86872e-09, 398.89
7.86479e-09, 426.67
*Elastic
209601., 0.3, -198.33
206153., 0.3, -128.89
202706., 0.3, -73.33
195122., 0.3, 21.11
190985., 0.3, 93.33
186848., 0.3, 148.89
183401., 0.3, 204.44
179953., 0.3, 260.
175127., 0.3, 315.56
170990., 0.3, 371.11
166164., 0.3, 426.67
*Expansion
1.64e-05, 21.11
1.65e-05, 37.78
1.67e-05, 65.56
1.68e-05, 93.33
1.69e-05, 121.11
1.7e-05, 148.89
1.72e-05, 176.67
1.73e-05, 204.44
1.74e-05, 232.22
1.75e-05, 260.
1.76e-05, 287.78
1.77e-05, 315.56
1.78e-05, 343.33
1.79e-05, 371.11
1.8e-05, 398.89
1.81e-05, 426.67
*Specific Heat
4.7201e+08, 21.11
4.7592e+08, 37.78
4.8178e+08, 65.56
4.8743e+08, 93.33
4.9334e+08, 121.11
4.9933e+08, 148.89
5.0696e+08, 176.67
5.1069e+08, 204.44
5.185e+08, 232.22
5.2428e+08, 260.
5.2786e+08, 287.78
5.3347e+08, 315.56
5.3928e+08, 343.33
5.447e+08, 371.11
5.5058e+08, 398.89
5.5394e+08, 426.67
**
** INTERACTION PROPERTIES
**
*Surface Interaction, name=Contact_COL_COLsup
1.,
*Friction, slip tolerance=0.005
0.3,
*Surface Behavior, no separation, pressure-overclosure=HARD
*Gap Conductance
15., 0.
0., 0.01
*Surface Interaction, name=Contact_COLsup_ShimPlate
1.,
*Friction, slip tolerance=0.005
0.3,
*Surface Behavior, pressure-overclosure=HARD
*Clearance, master=COL-1.OUT, slave=COL_sup-3.Contact_COL, value=0.
*Clearance, master=COL-1.OUT, slave=COL_sup-4.Contact_COL, value=0.
**
** BOUNDARY CONDITIONS
**
** Name: BC-3 Type: Displacement/Rotation
*Boundary
_PickedSet13, 2, 2
_PickedSet13, 3, 3
** Name: BC-4 Type: Displacement/Rotation
*Boundary
_PickedSet14, 2, 2
_PickedSet14, 3, 3
**
** PREDEFINED FIELDS
**
** Name: Predefined Field-4 Type: Temperature
*Initial Conditions, type=TEMPERATURE
COL-1.Complete, 30.
**
** INTERACTIONS
**
** Interaction: COL_COLsup3
*Contact Pair, interaction=Contact_COL_COLsup, small sliding, type=SURFACE TO SURFACE
COL_sup-3.Contact_COL, COL-1.OUT
** Interaction: COL_COLsup4
*Contact Pair, interaction=Contact_COL_COLsup, small sliding, type=SURFACE TO SURFACE
COL_sup-4.Contact_COL, COL-1.OUT
** ----------------------------------------------------------------
**
** STEP: Step-10
**
*Step, name=Step-10, inc=1000
*Heat Transfer, end=SS, deltmx=30.
0.3, 0.3, 3e-06, 0.3, 0.0002
** Interaction: Int-6
*Co-simulation, name=Int-6, controls=Int-6_Ctrls, program=MULTIPHYSICS
*Co-simulation Region, import, type=SURFACE
COL-1.IN, CFL
*Co-simulation Region, export, type=SURFACE
COL-1.IN, NT
*Co-simulation Controls, name=Int-6_Ctrls, coupling scheme=gauss-seidel, time incrementation=subcycle, time marks=yes,
step size=min, scheme modifier=lead
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-2
**
*Output, field
*Node Output
NT,
*Contact Output
PPRESS,
*Output, history, frequency=0
*End Step

I didn't paste geometry or assemblies...

Hope it helps.
oriol

 

[Jlog50]

Thank-you so much for your input Oriol,

I think I have found the problem my input file for my CFD does not have the following inputs. How can I add these through CAE?

*Co-simulation Region, import, type=SURFACE
_PickedSurf4, TEMP
*Co-simulation Region, export, type=SURFACE
_PickedSurf4, HFL

 

[Jlog50]

I should have mentioned, I have tried to do this through CAE but not found the way to do this. I currently have a CAE file with with both the CFD and Standard model in it. Any further help would be appreciated.

 

[Jlog50]

My CFD input file has only the following statements

** Interaction: Pipe_Fluid_Int-2
*Co-simulation, name=Pipe_Fluid_Int-2, controls=Pipe_Fluid_Int-2_Ctrls, program=MULTIPHYSICS
*Co-simulation Controls, name=Pipe_Fluid_Int-2_Ctrls

 

[oriol]

Hello Jlog50,

In fact I followed step by step the example from the presentation of abaqus 6.10 in simulia but anyway, as far as I understand we have:

- For the stuctural model:

** Interaction: Int-6*Co-simulation, name=Int-6, controls=Int-6_Ctrls, program=MULTIPHYSICS*Co-simulation Region, import, type=SURFACECOL-1.IN, CFL*Co-simulation Region, export, type=SURFACECOL-1.IN, NT

- For the CFD model:
** Interaction: Int-1*Co-simulation, name=Int-1, controls=Int-1_Ctrls, program=MULTIPHYSICS*Co-simulation Region, import, type=SURFACE_PickedSurf4, TEMP*Co-simulation Region, export, type=SURFACE_PickedSurf4, HFL

You get that by defining in boths models an interaction which surface is the one in common to boths models. In the CFD model there is just one type of interaction available. For the structural model, in a heat transfer step, you must choose a 'Fluid-Structure Co-simulation Boundary' interaction.

Hope it helps!
Oriol

 

[Jlog50]

Problem solved thanks Oriol.

For anyone reading this post in the future, please note that the problem in this post was caused by not selecting the appropriate step type as per the Abaqus/CAE user manual 6.10 section 15.3.

"Within the fluid model (Abaqus/CFD) the FSI co-simulation interaction can be created only in a flow step. Within the structural model (Abaqus/Standard or Abaqus/Explicit), the FSI co-simulation interaction can be created only in an implicit dynamic, explicit dynamic, or heat transfer step."

Then you can select a co-simulation boundary on the Abaqus/Standard or Explicit model. This then allows for a co-simualtion.

Another exmaple of how good this forum is an how helpful people are in the world