Abaqus Exporter Heat Transfer Study Bugs

Coreform Cubit
#1

Coreform Cubit Version: 2025.1
Platform: Windows

Issue
I am testing out the Abaqus Writer for a simple heat transfer study of a rod. Here are the commands to create the inp.

brick x 10 y 1 z 1
move vol 1 x 5 y 0.6 z 0.5
curve 2  interval 10
curve 2  scheme equal
curve 12  interval 1
curve 12  scheme equal
curve 1  interval 1
curve 1  scheme equal
block 1 vol 1
block 1 name "ht-beam"
create bcset name "ht-study" analysistype heat
modify bcset "ht-study" nonlinear_geometry off
modify bcset "ht-study" steadystate on
create temperature name "cold" on surface 6 value 380
create temperature name "hot" on surface 4 value 500
modify bcset "ht-study" add temperature 1 2
mesh vol 1
create material "Copper" property_group "CUBIT-ABAQUS" 
modify material "Copper" scalar_properties "CONDUCTIVITY" 370 
block 1 material 'Copper'
export Abaqus "Heat-Transfer-Study-Cubit.inp" overwrite

I also created the inp using Abaqus CAE for comparison. A few things to note:

  1. Element Type is C3D8RT where it should be DC3D8. One is a coupled element. The other is just for heat transfer.
  2. Assembly section is missing for Cubit generated file. Not sure how to generate this. Though for this single part, it is not required to run.
  3. For a heat transfer only study, I still get isotropic elastic material properties as well as density and specific heat where they are not necessary. Not sure if this prevents running.
  4. Steady state, nlgeom are missing even though they are added to the BCset.

Lastly, here is the message from Abaqus when I submit this inp as a job.

The job input file “Heat-Transfer-Study-Cubit.inp” has been submitted for analysis.
Error in job Heat-Transfer-Study-Cubit: in keyword *ELASTIC, file “Heat-Transfer-Study-Cubit.inp”, line 96: OdbError: Tabular data for at least one option or suboption has either blank or zero valued row(s).
Error in job Heat-Transfer-Study-Cubit: in keyword *SPECIFICHEAT, file “Heat-Transfer-Study-Cubit.inp”, line 102: OdbError: Tabular data for at least one option or suboption has either blank or zero valued row(s).
Error in job Heat-Transfer-Study-Cubit: MODULUS OF ELASTICITY MAY NOT BE ZERO FOR ISOTROPIC ELASTICITY
Error in job Heat-Transfer-Study-Cubit: 10 elements have been defined with zero hour glass stiffness. You may use *hourglass stiffness or change the element type. The elements have been identified in element set ErrElemZeroHourGlassStiffness.
Error in job Heat-Transfer-Study-Cubit: END=SS HAS BEEN SPECIFIED BUT THE STEADY STATE DEFINITION HAS NOT BEEN GIVEN
Error in job Heat-Transfer-Study-Cubit: ONLY DEGREES OF FREEDOM 11 AND ABOVE CAN BE ACTIVE IN THE MODEL FOR THIS PROCEDURE. CHECK THE PROCEDURE AND ELEMENT TYPES USED IN THIS MODEL.
Job Heat-Transfer-Study-Cubit: Analysis Input File Processor aborted due to errors.
Error in job Heat-Transfer-Study-Cubit: Analysis Input File Processor exited with an error - Please see the Heat-Transfer-Study-Cubit.dat file for possible error messages if the file exists.
Job Heat-Transfer-Study-Cubit aborted due to errors.

I am more than willing to provide additional information for this process.

Heat-Transfer-Study-Native.inp (3.9 KB)
Heat-Transfer-Study-Cubit.inp (5.1 KB)

#3

Hi @ccarranza,
unfortunately you can’t change the element type from C3D8RT to DC3D8 on export.
But you can generate the assembly section with instancing blocks.

I will discuss the behavior that the undefined material properties are also exported with the dev’s.

The nlgeom parameter will get exported when you set “on” instead of “off”. With the steady state option the parameter “END=SS” gets exported. That’s most likely why abaqus needs a specific heat.

You could also export the mesh and append custom lines to the inp with python.

reset
brick x 10 y 1 z 1
move vol 1 x 5 y 0.6 z 0.5
curve 2  interval 10
curve 2  scheme equal
curve 12  interval 1
curve 12  scheme equal
curve 1  interval 1
curve 1  scheme equal
block 1 vol 1
block 1 name "ht-beam"
create bcset name "ht-study" analysistype heat
modify bcset "ht-study" nonlinear_geometry on
modify bcset "ht-study" steadystate on
create temperature name "cold" on surface 6 value 380
create temperature name "hot" on surface 4 value 500
modify bcset "ht-study" add temperature 1 2
mesh vol 1
create material "Copper" property_group "CUBIT-ABAQUS" 
modify material "Copper" scalar_properties "CONDUCTIVITY" 370 
modify material "Copper" scalar_properties "SPECIFIC_HEAT" 10
block 1 material 'Copper'
export Abaqus "Heat-Transfer-Study-Cubit.inp" overwrite Instance Block 1 Target_csys 0
#4

Actually, for Abaqus there is an ability to set the solver element type. You can use the command

create solver_element "abaqus" "DC3D8" from "HEX8"

The command maps a Cubit HEX8 to a specified Abaqus element type. This will create an element card that looks like
*ELEMENT, TYPE=DC3D8, ELSET=EB1

I created this command for a specific customer and I have not had funding or time to generalize this for all solvers. It does however, work for Abaqus.

Karl