ANSYS to ABAQUS

[andreashellstrand]

Folks,

I am wondering if any of you have a good idea how to go from ANSYS
format to ABAQUS format? I have a .db file created in ANSYS that I need
in ABAQUS format - including elements, nodes, material, and contact.
Is there an easy way to do this? My understanding is that there is a
way which includes writing scripts...is this correct? And if so, for a
person who don't know what ABAQUS format looks like, where can I find
this information? Thanks for your replies and help.

Andreas Hellstrand
Thule Sweden AB

[Dave Lindeman]

You can find an example of such an ANSYS script on www.ansys.net
(perform a search on "ABAQUS" and follow the link called "ANS2ABA").
This example includes contacts, material properties, etc. If I were to
rewrite the script today I would use C-style formatting on the *VWRITE
commands (rather than the FORTRAN style shown), and would also make use
of *VGET to retrieve node and element definitions in blocks (much faster
than the *DO loops shown). In any case, the script should give you the
basic idea -- customize as necessary.

As for learning the ABAQUS input deck format, you'll need to have access
the ABAQUS documentation -- hardcopy or on-line. If you have some
example ABAQUS input (*.inp) decks, you can learn a lot just by looking
at them. If the input decks were generated using ABAQUS/CAE, however,
they will likely have a part/assembly format that makes them somewhat
more difficult to understand (and you most likely won't use this format
if you're directly generating them using scripts in ANSYS).

Good luck,

Dave

-------------------------
Dave Lindeman
Lead Research Specialist
3M Company
3M Center 235-3F-08
St. Paul, MN 55144
651-733-6383

Post by andreashellstrand
Folks,
I am wondering if any of you have a good idea how to go from ANSYS
format to ABAQUS format? I have a .db file created in ANSYS that I need
in ABAQUS format - including elements, nodes, material, and contact.
Is there an easy way to do this? My understanding is that there is a
way which includes writing scripts...is this correct? And if so, for a
person who don't know what ABAQUS format looks like, where can I find
this information? Thanks for your replies and help.
Andreas Hellstrand
Thule Sweden AB

[Milton Deherrera]

Andreas,

It has been my experience that nodes, elements and sets typically
comprise 99% of any input file, so if you can capture those three (or
even the first two), you will be in pretty good shape.

ABAQUS takes free field format input. For nodes, the format is as follows:

*node
<node number>, <x-coord>, <y-coord>, <z-coord>

For example,

*node
1, 1.24628, -9.19251, -0.09153
2, 1.20236, -9.19334, -0.08233
3, 1.44197, -9.19243, -0.09403


You can have element sets (called elsets) or node sets (called nsets).
The syntax for those is similar. For example, to create an nset
named "harry", you would have an entry like:

*nset, nset=harry
23, 256, 12, 30, 22, 1002, 67, 876,
33, 400, 566

(There is a maximum of eight entries per input line). If you have a
sequential set of nodes, the syntax is as follows:

*nset, nset=harry, generate
1, 20001, 1
9005, 120045, 5
(the third number is the node generation increment)

The syntax for elsets is similar, except that instead of *nset, nset=
, you have *else,elset=

To define elements, the syntax is:

*elements, type=xxx, elset=yyy
<element number>, < node number>, <node number>,....
<element number>, < node number>, <node number>,....
<element number>, < node number>, <node number>,....
.
.
.
Type is the ABAQUS element type; for example, 3D bricks can be c3d8,
c3d8r, c3d8i, and so on. Elset puts the created elements in elset
"yyy". The only caveat in the format is that elements that have more
than six nodes have their input continued on to a second line. For
example, the input for a "Wedge" element is something like

*element, type=c3d6, elset=part2
158069, 35990, 36044, 36043, 132253, 132176, 132254
158070, 36786, 36785, 36847, 134106, 134210, 134055

whereas for an 8-noded "brick" element, the input looks like this:

*element, type=c3d8r, elset=stent
1, 13, 29, 16, 15, 96317, 96320,
96319, 96318
2, 1, 13, 15, 2, 96321, 96317,
96318, 96322
3, 13, 14, 28, 29, 96317, 96324,
96323, 96320

Note the last two nodes spill onto a second line.

Hope this helps!

Milton D.

Post by andreashellstrand
Folks,
I am wondering if any of you have a good idea how to go from ANSYS
format to ABAQUS format? I have a .db file created in ANSYS that I need
in ABAQUS format - including elements, nodes, material, and contact.
Is there an easy way to do this? My understanding is that there is a
way which includes writing scripts...is this correct? And if so, for a
person who don't know what ABAQUS format looks like, where can I find
this information? Thanks for your replies and help.
Andreas Hellstrand
Thule Sweden AB

[AARASH]

Andreas,

Milton is right but I think node number of three dimensional elements
is different in abaqus. first check it. I had same problem before.

Post by Milton Deherrera
Andreas,
It has been my experience that nodes, elements and sets typically
comprise 99% of any input file, so if you can capture those three (or
even the first two), you will be in pretty good shape.
*node
<node number>, <x-coord>, <y-coord>, <z-coord>
For example,
*node
1, 1.24628, -9.19251, -0.09153
2, 1.20236, -9.19334, -0.08233
3, 1.44197, -9.19243, -0.09403
You can have element sets (called elsets) or node sets (called nsets).
The syntax for those is similar. For example, to create an nset
*nset, nset=harry
23, 256, 12, 30, 22, 1002, 67, 876,
33, 400, 566
(There is a maximum of eight entries per input line). If you have a
*nset, nset=harry, generate
1, 20001, 1
9005, 120045, 5
(the third number is the node generation increment)
The syntax for elsets is similar, except that instead of *nset, nset=
, you have *else,elset=
*elements, type=xxx, elset=yyy
<element number>, < node number>, <node number>,....
<element number>, < node number>, <node number>,....
<element number>, < node number>, <node number>,....
.
.
.
Type is the ABAQUS element type; for example, 3D bricks can be c3d8,
c3d8r, c3d8i, and so on. Elset puts the created elements in elset
"yyy". The only caveat in the format is that elements that have more
than six nodes have their input continued on to a second line. For
example, the input for a "Wedge" element is something like
*element, type=c3d6, elset=part2
158069, 35990, 36044, 36043, 132253, 132176, 132254
158070, 36786, 36785, 36847, 134106, 134210, 134055
*element, type=c3d8r, elset=stent
1, 13, 29, 16, 15, 96317, 96320,
96319, 96318
2, 1, 13, 15, 2, 96321, 96317,
96318, 96322
3, 13, 14, 28, 29, 96317, 96324,
96323, 96320
Note the last two nodes spill onto a second line.
Hope this helps!
Milton D.

Post by andreashellstrand
Folks,
I am wondering if any of you have a good idea how to go from ANSYS
format to ABAQUS format? I have a .db file created in ANSYS that I need
in ABAQUS format - including elements, nodes, material, and contact.
Is there an easy way to do this? My understanding is that there is a
way which includes writing scripts...is this correct? And if so, for a
person who don't know what ABAQUS format looks like, where can I find
this information? Thanks for your replies and help.
Andreas Hellstrand
Thule Sweden AB

[Gregory Yow]

There is a much easier way now with workbench. Use FE modeler. It
can import & export Abaqus input decks. FE modeler is available to
everyone.

Post by Milton Deherrera
Andreas,
It has been my experience that nodes, elements and sets typically
comprise 99% of any input file, so if you can capture those three (or
even the first two), you will be in pretty good shape.
*node
<node number>, <x-coord>, <y-coord>, <z-coord>
For example,
*node
1, 1.24628, -9.19251, -0.09153
2, 1.20236, -9.19334, -0.08233
3, 1.44197, -9.19243, -0.09403
You can have element sets (called elsets) or node sets (called nsets).
The syntax for those is similar. For example, to create an nset
*nset, nset=harry
23, 256, 12, 30, 22, 1002, 67, 876,
33, 400, 566
(There is a maximum of eight entries per input line). If you have a
*nset, nset=harry, generate
1, 20001, 1
9005, 120045, 5
(the third number is the node generation increment)
The syntax for elsets is similar, except that instead of *nset, nset=
, you have *else,elset=
*elements, type=xxx, elset=yyy
<element number>, < node number>, <node number>,....
<element number>, < node number>, <node number>,....
<element number>, < node number>, <node number>,....
.
.
.
Type is the ABAQUS element type; for example, 3D bricks can be c3d8,
c3d8r, c3d8i, and so on. Elset puts the created elements in elset
"yyy". The only caveat in the format is that elements that have more
than six nodes have their input continued on to a second line. For
example, the input for a "Wedge" element is something like
*element, type=c3d6, elset=part2
158069, 35990, 36044, 36043, 132253, 132176, 132254
158070, 36786, 36785, 36847, 134106, 134210, 134055
*element, type=c3d8r, elset=stent
1, 13, 29, 16, 15, 96317, 96320,
96319, 96318
2, 1, 13, 15, 2, 96321, 96317,
96318, 96322
3, 13, 14, 28, 29, 96317, 96324,
96323, 96320
Note the last two nodes spill onto a second line.
Hope this helps!
Milton D.

Post by andreashellstrand
Folks,
I am wondering if any of you have a good idea how to go from ANSYS
format to ABAQUS format? I have a .db file created in ANSYS that I need
in ABAQUS format - including elements, nodes, material, and contact.
Is there an easy way to do this? My understanding is that there is a
way which includes writing scripts...is this correct? And if so, for a
person who don't know what ABAQUS format looks like, where can I find
this information? Thanks for your replies and help.
Andreas Hellstrand
Thule Sweden AB

[Hellstrand, Andreas]

Thanks for your replies regarding the subject. I have access to
Workbench, and I have tried that option. However, it seems like the
contact and boundary conditions don't transfers....do you know if that
requires some extra step to include these? Thanks for your reply.

Best Regards,
Andreas Hellstrand



[Non-text portions of this message have been removed]