Abaqus, distributions of thicknesses and plies

[headcroco]

Hi. I am using Abaqus to perform an anlysis on a variable tow angle laminate, and I am having some problems when I start the simulation. The errors are:
1) THE DEFAULT SHELL THICKNESS DEFINED IN DISTRIBUTION ASSEMBLY_PART-1-1_PART-1_THICKPLY1 MUST BE POSITIVE AND HAVE MAGNITUDE GREATER THAN MACHINE PRECISION
2) 81 elements have missing property definitions. The elements have been identified in element set ErrElemMissingSection.

I have attached the .inp file to this thread, in case you want to give it a look:
Open Abaqus, click on 'Import', then 'Model', select the .inp file extension and then select 'SSSS-0000-000VAT.inp'.

Here's the link to the file:

https://files.engineering.com/getfi...-a76f-7179bb953e3c&file=SSSS-0000-0000VAT.inp

Thank you in advance.

Edit: for now, the simulation regards a plate made by only one ply, of thickness 1 mm. the thickness is supposed to be constant along the surface,
while the rotation angle of the ply changes along it.

 

[FEA way]

Just change the value that you specified as the default one in distributions from -99999.99 to something more realistic (it can be the same or similar to other values defined in the distribution) and it will work.

 

[headcroco]

@FEA way
How do you change the default value?

 

[FEA way]

In the input file you can specify it using the first line of *Distribution keyword, with an empty space instead of an element number. For example:

*Distribution, name=PART-1_ORIANGLEPLY, location=ELEMENT, Table=PART-1_ORIANGLEPLY_Table
, 150.
1, 165.
2, 165.
3, 165.
...

In this case 150 will be the default value.

 

[headcroco]

@FEA way
Ok. What about the elements? How can I define them in sets before giving them to the *distribution? As you can see in my file, I have put the elements in the distribution in a very non-efficient way. For example, instead of:
1,165
2,165
3,165
4,165
something more convenient would be:
set name, 165

 

[FEA way]

This can be easily done in Abaqus/CAE, then you could export the input file and keep working with it using a text editor.

 

[headcroco]

@FEA way
I've already tried exporting the interested sets, and put them in this shape in the .inp file:
*Elset, elset=SETVAT1, instance=plate-1
1, 2, 3, 4, 5, 6, 7, 8, 9

or :

*Elset, elset=SETVAT1, instance=plate-1, generate
1, 9, 1

and I put the instruction right before the *Distribution, and wrote 'SETVAT1,165' in the *Distribution, but it gave me the following error:
'Unknown assembly level element set SETVAT1.'

 

[FEA way]

Try exporting the input file without the use of instances (there is an option for that in Abaqus/CAE when you enter Model Attributes).

 

[headcroco]

@FEA way
I removed all the instances names, and obtained expressions like this:
*Elset, elset=SETVAT1, generate
1, 9, 1

but the error is still the same.

 

[FEA way]

It should work if you check this option ("Do not use parts and assemblies in input files") and then export and edit the input file.

 

[headcroco]

@FEA way
I also tried to check the box of: 'Do not use parts and assemblies in input files' but, again, nothing changed.

 

[FEA way]

Can you attach the input file written this way (and then edited as we discussed before) ?

 

[headcroco]

@FEA way
of course. Here it is:

https://files.engineering.com/getfi...3a41771&file=SSSS-0000-0000VAT_simplified.inp

edit: In this version, there are 8 plies assembled together. I hope it will not complicate too much the vision.

 

[FEA way]

This time the errors were different. You used repeating name for distribution tables, skipped the default values and used wrong integers in boundary condition definition. Here's the corrected input file:

 

[headcroco]

@FEA way
I have submitted the .inp file you just gave me, and I received the same error as before, plus a new one:
1) Unknown assembly level element set SETVAT1.
2) AbaqusException: Invalid variables are specified in an output request. An output request cannot be created in a step where some variables are invalid. This occurred while creating an output request for variables NT, U in step buckling_step.
The model "SSSS-0000-0000VAT_simplified_v2" has been imported from an input file.
Please scroll up to check for error and warning messages.

 

[FEA way]

Try running this directly from the command line instead of importing to CAE (inp import may not work properly in some cases).

 

[headcroco]

@FEA way
Excuse me, which are the command lines to open directly the .inp file in Abaqus? Thank you.

 

[FEA way]

Open the command window in the location of the input file (on Windows you can use Shift + RMB and then select "Open command window here" or "Open PowerShell window here", depending on the system version). Then type the following command:

abaqus job=input_file_name interactive

This will run the analysis and generate output files, including odb file with results (you can open it in Abaqus/Viewer).

 

[headcroco]

@FEA way
the simulation appeared, but the results are different from the version I used. I will check deeper. Thank you very much for you help!