In you software setup directory like this: C\SIMULIA\Abaqus\6.13-1\code\bin

you can find this file: mkl_avx2.dll

change the file suffix to: mkl_avx2.dll.13.0.0.1

if you use other version like 6.12, you can change the file mkl_avx2.dll.12.0.0.1

and so on

Change your element size ( make it coarse) or change your computer and re-run it again .

Check the msg file and there will be the error

Hello every one

I could manage to solve the problem by involving more cpu percantage.

it is in the job module

Thanks anyway.

How much percentage did you go with? The default is 90%. Did you choose 100%?

I have this same problem... Thank you for your help!

the analysis aborts with error code of 1073741819 performed on an Intel I7 4th generation processor

you could possibly getting bug

reroute your directory/code/bin

the analysis aborts with error code of 1073741819 performed on an Intel I7 4th generation processor

you could possibly getting bug

reroute your directory/code/bin

the analysis aborts with error code of 1073741819 performed on an Intel i7, 4th generation processor

you could possibly getting bug

reroute your directory/code/bin

the analysis aborts with error code of 1073741819 performed on an Intel i7, 4th generation processor

you could possibly getting bug

reroute your directory/code/bin

the analysis aborts with error code of 1073741819 performed on an Intel i7, 4th generation processor

you could possibly getting bug

reroute your directory/code/bin

Dear Seyyed

I have the same problem

can you help me?

Thanks in advance

It's an internal error. Sometimes it means modelling issues and some time memory management problem. I will recommend to rerun on some other version of abaqus

Dear Sanan H Khan,

Thanks

I have stumbled upon this error while using subroutines. This usually occurs with me when i do mistake in coding dealing with access violation. If you are using subroutines i recommend you to go the through the code. look for any missing "end if"s or someplace where variables are wrongly passed or called.

Hello,

I encountered this error yesterday when analyzing an 2D square RVE problem. This error is due to improper definition of the periodic boundary condition. To be specific, the four nodes on the four corners of the square were overly constrained. After removing the extra constraint, the analysis ran through.

Hope it helps

For me it worked changing the material input data

For me it worked when I provided an enough storage memory to the analysis .

The best way to eliminate this error is: toggle off the "GPGPU" in "Use acceleration processors"...Job>job edit>paralellization>...

It does not work for me. Any other solution?

In you software setup directory like this: C\SIMULIA\Abaqus\6.13-1\code\bin

you can find this file: mkl_avx2.dll

change the file suffix to: mkl_avx2.dll.13.0.0.1

if you use other version like 6.12, you can change the file mkl_avx2.dll.12.0.0.1

and so on

It's an internal error, depending on the versions of ABAQUS you're working with. It seems I only have that issues with ABAQUS 6.13-1. You may either upgrade to ABAQUS 6.14 or change the file suffix of mkl_avx2.dll to mkl_avx2.dll.13.0.0.1 as Zhang Wen mentioned.

For me, the solution recommended by Mr. Zhang Wen worked out. Thank you so much.

hello

i have the same error

can anybody helps me?

i change the name of bin file , but still i have this error

https://www.researchgate.net/post/How_do_you_solve_the_system_error_code_1073741819_in_Abaqus_613

The question is old, but I see it seems to be a frequent occurrence. I do too sometimes incur in this message.

The first thing to pay attention to is the following: system error code 1073741819 is a Windows error exit code, not an Abaqus one! It is due to an access violation, i.e. the program is trying to access a location in memory (RAM or storage) which it is not allowed to.

Thus, there are in general many reasons why Abaqus is causing this error. Here a few of them, in order of likelihood.

1. Your model is too big: the memory requirement is greater than the available, given by the sum of RAM + pagefile.sys (usually equal to the installed RAM).

2. Some error in the model formulation that escapes pre.exe's checks and thus gets translated into an incoherent model in standard.exe. It is usually a feature that is syntactically correct but physically inconsistent (problems in boundary conditions, material properties' definition).

3. Incompatibility with the CPU's architecture. This is usually fixed by changing the suffix of the .dll file, as previously suggested. If you're using a recent version of Abaqus on a recent computer (I'd dare say versions of both published after 2010), it's very unlikely that this is the reason.

So, how to proceed? Here's a step-by-step debugging procedure.

1. Run one of the examples provided by Abaqus, possibly a simple one. Does it complete correctly?

2. If not, try to change the dll's suffix. Does it work? if yes, it's problem 3. If not, it's probably some installation/hardware architecture/hardware failure (like faulty hard disk) issue. Try to re-install Abaqus and/or run a system check.

3. Run your model with a very coarse mesh: does the simulation complete? If yes, it's a size problem, i.e. the memory required by your model exceeds the available one. Move to a more powerful system or optimize your model: can you reduce the number of elements? Can you use lower-order or reduced-order elements?

4. If the simulation with the coarse mesh doesn't complete, it's a problem in the model formulation. It's not a syntactic error, but a physical one: you defined a parameter that Abaqus can read but it doesn't make sense physically. Check geometry, materials' definitions, boundary, and initial conditions.

For me it worked changing the material input data

In my case, it was due to an inconsistency in the element type definition: some elements of the same part had temperature degree of freedom enabled while others not. Using element type with temperature degree of freedom enabled (because I need it) for all the elements of that part solved the problem.

It was indeed a modelling error not detected by the data check of Abaqus.

https://www.researchgate.net/post/how_can_i_solve_error_code_1073740940_in_ABAQYS

I'm using ABAQUS 2018 and the above resolution did not work for me. I had to remove the CPU specification (CPUS 4 for instance) and it worked.

I have the same problem.

The problem is that forgetting a variable in the called routine causes an error, so it is recommended to drain the program and the model problem before considering other reasons.

When I implement the UMAT, the same problem happened. The problem was solved by making sure that all of utilized variables in the UMAT was declared in correct data types.

Hi

rename the file mkl_avx2.dll to this: mkl_avx2.dll.11.0.0.1 

Hi seyyed Hamed Shojaeddin

did you solve your problem?

I have the same error in Abaqus when I run UEL subroutine:

"Unexpected LoadLibraryA error 193

Abaqus Error: The executable standard.exe

aborted with system error code 1073741571.

Please check the .dat, .msg, and .sta files for error messages if the files exist.

this subroutine has been run in older version of Abaqus (6.5); but in the newer version (6.14.2) has an error.

Hossein

The system error in std_findcutshape3d8_xfem -- nodal level set values might not be correct for element 11576 instances part-1-1

The executable standard.exe aborted with system error code 1073741819. Please check the .dat, .msg, and .sta files for error messages if the files exist. If there are no error messages and you cannot resolve the problem, please run the command "Abaqus job=support information=support" to report and save your system information. Use the same command to run Abaqus that you used when the problem occurred. Please contact your local Abaqus support office and send them the input file, the file support.log which you just created the executable name, and the error code.

My Advice:

•This is error is not due to ABAQUS/modelling strategy in ABAQUS.

• It is due to the low configuration of the system.

• Older systems/Laptops cant handle big models.

• Model can still run on Older systems/Laptops if no of elements can be reduced

• This error will not appear with High-end workstations

• High RAM and more CORES should be there in the system

In you software setup directory like this: C\SIMULIA\Abaqus\2018\code\bin

you can find this file: mkl_avx2.dll

change the file suffix to: mkl_avx2.dll.2018.0.0.1

There must be a NaN number in your user subroutine. Try to use write(*,*) command to debug every variable in your subroutine.

Hi,

Error code 1073741819 is repaired in my models with suppressing the “General Contact”.

Kind Regards

Busra

Hello everyone,

obviously, the reasons for this error could be different.

I am using a UMAT subroutine and I got this error for a programming error which was made during debugging.

In the code, where I handled a vector, I had:

STRESS(K) = STRESSold(K) + DSTRESS(K)

instead of:

DO K = 1,NTENS

STRESS(K) = STRESSold(K) + DSTRESS(K)

END DO

So forgot to add DO and END DO.

The problem could be sometimes associated with errors of the model itself. Actually for my case it occurred due to lack of property definition for some parts, which was really odd as it didn't come along with a "missing property definition" error. Check the error messages in your Data File and you can probably find some clues!