DC-FSI error of undefined external node

Cui

Hello everyone,

I followed the procedures for  5.13 ACU-T: 5403 Piezoelectric Flow Energy Harvester: A Fluid-Structure Interaction in AcuSolve tutorial to do a DC-FSI analysis.

However, I had errors 'ERROR: Undefined external node' for all the nodes in the coupling surfaces in OptiStruct model.

I attach the log file and inp file here.

Does any one know why this happen?

Thanks a lot!

Unable to find an attachment - read this blog

acupro

I just ran through this tutorial, and it seems to work correctly as written.  (I did notice that you had left Simple BC active for the Beam surface, where it should be inactive/off since it's handled by the External Code Surface command.  In any case, it still ran when I did leave it active as you had it.)  Is it possible you assigned the BCs to the wrong surface sets?

 

Can you attach the slab_dcfsi.out and cci.txt files from your run?

 

Which versions of AcuSolve/OptiStruct are you using?  (I have HyperWorks CFD Solvers 2019.1 and HyperWorks Solver 2019.2.)

Cui

Thanks acupro,

I updated OS to the 2019.2 and it works now.

However, I met a new error:

acuSolve: *** TCP socket write error; Permission denied
acuRun: *** ERROR: error occurred executing acuSolve

Do you know what is the reason for this error?

BTW thanks for telling me that I didn't turn off the Simple BC for beam.

Thanks!

And I really appreciate your help!

Unable to find an attachment - read this blog

acupro

I'm not very good on the OptiStruct side, but apparently the OptiStruct side has finished and closed the connection to AcuSolve.  I now see you've made changes to the tutorial model - or whichever model you're running.  But whatever you've done on the OptiStruct side does not appear to be consistent with what you've done on the AcuSolve side.

Tarek Bouabidi

<?xml version="1.0" encoding="UTF-8"?>hello everyone,

I have to run a tutorial about Direct Coupling Fluid structure interaction between Acusolve and optistruct.It is not the  Piezoelectric Flow Energy Harvester one but it is a similar to this.

I got an error in Acusolve which is 'unable to match with the external surface at 22 quadrature points'.

Do you know what is the reason for this error ?

Can Anyone help me please ?

thank you in advance !!

 

 

 

 

 

acupro

That generally means the surfaces on the AcuSolve side and the OptiStruct side are not co-located.  Make sure both models have the DC-FSI surfaces in the same location and are the same size/scale and shape.  Just above the assertion you have in the Log file:  Ave distance = 9.367829e-004; Max distance = 2.350710e-002.  This means the maximum distance between the OptiStruct and AcuSolve surfaces is 2.350710e-02, larger than the Max allowed gap of 5.486660e-003.  Check to ensure the surfaces are the same size, shape, and location in both models.

Lucia R

Hi!

I have the same error but the max distance of my model is smaller than the max allowed gap. 

I have checked that the surfaces are the same size, shape and location in both models, so I dont know what to do.

Anyone knows how to solve this error?

 

Thanks!

 

acupro

Can you post the complete .Log file - along with the AcuSolve .inp file?

I see your time increment is 1.0 sec.  This may allow lots of motion on the structural side, making it difficult for AcuSolve to track the movement of the structure.  You need to make sure the time increment is adequate to resolve any transient nature to the flow itself, along with any possible motion of the structure/FSI surfaces.  Doe it behave better if you use a smaller time increment - say 0.01 to test?  You may also want to add a multiplier function to the External_Code command.

Lucia R

Thanks for your answer!

Yesterday before your answer, I tried to delete de cfd geometry and do it again based on the optistruct geometry. The error dissappeared and the results may be acceptable, but I am going to apply your advice and use a time icrement of 0.01 to improve the results.

Thanks for your help

Sobir Basith

Cui said:

Thanks acupro,

I updated OS to the 2019.2 and it works now.

However, I met a new error:

acuSolve: *** TCP socket write error; Permission denied
acuRun: *** ERROR: error occurred executing acuSolve

Do you know what is the reason for this error?

BTW thanks for telling me that I didn't turn off the Simple BC for beam.

Thanks!

And I really appreciate your help!

Unable to find an attachment - read this blog

Have you solve this issue? I cannot solve it yet. Same error come out

acupro

Sobir Basith said:

Have you solve this issue? I cannot solve it yet. Same error come out

The Simple BC for z_neg and z_pos surfaces need to have mesh-displacement-type = slip.  This appears to have been missed - and they are left as the default fixed.  Thus, none of the nodes in the AcuSolve model can move, while the OptiStruct model does move.  Eventually the run fails.

The hint that the mesh motion was a problem - all the zeroes in the Mesh Displacement Stagger in the AcuSolve .Log file.

The next issue is with the surface groups.  The only surfaces that should be in the 'cylinder' group/set are those that are cylindrical in shape.  The others - the long surfaces of the beam, and the tip - should be in the 'beam' set/group that was renamed from 'default' in the instructions.  These are the cosimulation surfaces that will deform.