Running Abaqus in Matlab environment

In some cases, we need to perform a parametric study: how certain parameters affect the stress/strain/displacement at certain point or certain region in a model, or doing certain structural optimization. For such a circumstance, combining Abaqus with an additional programming language , which has an optimization capability would be unavoidable. Following shows you a snip how to perform the analysis repeatedly in Matlab.

for i = 1 : 10
istatus = dos('abq661 job=filename interactive'); % Run Abaqus,
if ~(istatus) exit; end
% Call a function to parse the necessary outcome.
% Call an optimization algorithm. See. help optim
% Call a function to modify the Abaqus input file
end

FeG-

The End of ABAQUS/Viewer User’s Manual

If you are using the old version of ABAQUS, for example version 6.2, you can find the ABAQUS/Viewer User’s Manual which provides you a complete guidance in using the Viewer. The manual, about 15 mm thick, is not difficult to read, but it may take a few hours to finish. It cost me about four hours to read from cover to cover. If you have a limited amount of time, then you should directly read Chapter 2: a Tutorial, and then, spend 5 minutes to read Chapter 10: Printing Canvas Object which will teach you how to produce a figure.

In the ABAQUS Version 6.6-1, you wouldn’t find the ABAQUS/Viewer User’s Manual, but dont worry, because the User’s Guide has been broken down into a number of manuals in the new version. The Chapter 2: Tutorial is now given in the Appendix D of the Getting Started Manual for ABAQUS 6.6-1, and the rest materials of the ABAQUS/Viewer User’s Manual are now presented as a part of the ABAQUS/CAE User’s Guide.

FeG-

ANSYS-APDL to Abaqus input: Plate with hole

Abaqus input file is easy, easier than the LS-Dyna input file. Following shows how to produce the input file by using ANSYS.


/clear
/prep7
et, 1, plane42,,, 3
mp, ex, 1, 1000.0
mp, nuxy, 1, 0.3
r, 1, 0.1
rectng, 0, 10, 0, 10
pcirc, 2.5
asba, 1, 2
amesh, all
nsel,, loc, x, 0.0, 0.0
cm, cNodeLeft, node
nsel,, loc, y, 0.0, 0.0
cm, cNodeBottom, node
alls
nsel,, loc, y, 10, 10
cm, cNodeTop, node
alls
lsel,, loc, y, 10, 10
sfl, all, pres, -1.0
alls
sftran
alls
finish
!*** PRODUCING ABAQUS INPUT FILE ***
*cfopen, abqPlateWithHole, inp ! Open file
*vwrite ! Write the header
('*heading')
*get, NOD, node,, count ! Write node location
*vwrite
('*node, nset = all')
*do, i, 1, NOD
*vwrite, i, nx(i), ny(i), nz(i)
(F6.0, TL1, ',', E16.9, ',', E16.9, ',', E16.9)
*enddo
*get, NOE, elem,, count ! Write element topology
*vwrite
('*element, type = cps4, elset = all')
*do, i, 1, NOE
*vwrite, i, nelem(i,1), nelem(i,2), nelem(i,3), nelem(i,4)
(F7.0,TL1,4(',',F7.0,TL1),' ')
*enddo
*vwrite ! Write element property
('*solid section, elset = all, material = steel, elset = all')
*vwrite
('0.1')
*vwrite ! Write material
('*material, name = steel')
*vwrite
('*elastic')
*vwrite
('1000.0, 0.3')
*vwrite ! Write a group of nodes
('*nset, nset = nodeLeft')
nsel,, node,, cNodeLeft
*get, nn, node,, count
presentNode = 0
*do, i, 1, nn
presentNode = ndnext(presentNode)
*vwrite, presentNode
(F7.0,TL1,',')
*enddo
*vwrite ! Write other group of nodes
('*nset, nset = nodeBottom')
nsel,, node,, cNodeBottom
*get, nn, node,, count
presentNode = 0
*do, i, 1, nn
presentNode = ndnext(presentNode)
*vwrite, presentNode
(F7.0,TL1,',')
*enddo
*vwrite ! Write one more group
('*nset, nset = nodeTop')
nsel,, node,, cNodeTop
*get, nn, node,, count
presentNode = 0
*do, i, 1, nn
presentNode = ndnext(presentNode)
*vwrite, presentNode
(F7.0,TL1,',')
*enddo
*vwrite ! Write history section
('*step')
*vwrite
('*static')
*vwrite
('*boundary')
*vwrite
('nodeLeft, 1')
*vwrite
('nodeBottom, 2')
*vwrite
('*cload')
*vwrite
('nodeTop, 2, 1')
*vwrite
('*node print, nset = all')
*vwrite
('u')
*vwrite
('*el print, elset = all')
*vwrite
('s')
*vwrite
('*end step')
*cfclose