Automatic meshing impossible, need C3D8

[Frank Richter]

Dear Group,

we want to simulate the loading of a specimen of circular cross section which is tapered in the central section and has additional notches on two vertical opposing faces in that central section. Hence, the specimen is not axisymmetric any longer. I have to use continuum elements.

I import the geometry from a iges file and obtain: "The Part UFTE_SN contains imprecise geometry, which is highlighted. Partitioning and quad/hex meshing using the medial axis algorithm may fail on imprecise parts."


I switch to Module 'Mesh' and execute 'Seed Part', then 'Mesh - Part': "The selected regions cannot be meshed automatically using the assigned element shapes. They must either be partitioned, assigned a tet shape, or manually meshed using the Create Bottom-Up Mesh tool."

Thus, I have 3 options:

1) I did achieve to have the structure meshed with tetrahedral elements C3D10 or C3D4. The simulation results are miserable. Part of the central section is radially squeezed out. The material is elastic-plastic, and the message file states the typical
***WARNING: THE STRAIN INCREMENT HAS EXCEEDED FIFTY TIMES THE STRAIN TO CAUSE FIRST YIELD AT 1397 POINTS

Element selection guidelines recommend second order elements, possibly reduced, for this type of loading. Thus, I'd need to have the stucture meshed using C3D8.

2) Bottom-up technique:
Manual 17.11.5 Creating the boundary mesh for a bottom-up region
Creating a boundary mesh: From the main menu bar, select Mesh - Region.
I end up with the same message as above and cannot continue here.

3) I did not succeed using the partitioning technique as I am totally new to these features, and options abound therein. ABAQUS is not specific in whether I have to partition edges, faces or cells. Hence I am confronted with solving a problem which I cannot clearly identify. Can anyone advise me how to proceed here ?


Other options:
Should I import the geometry from another CAD file type ? Which one is best suited ?
Can I have the structure meshed with C3D8 elements in an external meshing software ? If so, why does ABAQUS fail ?
For symmetry reasons it is sufficient to import only one eigth of the total geometry and then use Sweep/Extrude. Will that do the trick ?

Thank you for sharing your expertise

Frank
-----------------------------------------------------------------------
Frank Richter
Institute of Materials Science
Ruhr-Universitaet Bochum
Bochum
Germany

[fcn_public]

Hi Frank,

Post by Frank Richter
we want to simulate the loading of a specimen of circular cross
section which is tapered in the central section and has additional
notches on two vertical opposing faces in that central section.
Hence, the specimen is not axisymmetric any longer. I have to use
continuum elements.
I import the geometry from a iges file and obtain: "The Part
UFTE_SN contains imprecise geometry, which is highlighted.
Partitioning and quad/hex meshing using the medial axis algorithm
may fail on imprecise parts."

[...]

Post by Frank Richter
Should I import the geometry from another CAD file type ? Which one is best suited ?

ABAQUS uses parasolid (*.sat) for its geometry, so use that if possible. Generally speaking, avoid IGES if possible (use STEP if there is no other choice). IGES is about the worst geometry format on earth, as it is different from vendor to vendor (it is a very ambiguous standard!).

Post by Frank Richter
Can I have the structure meshed with C3D8 elements in an external meshing software ?

Definitely, many people do that by default. Hypermesh, Patran and many other preprocessors produce valid ABAQUS input files.

If so, why does ABAQUS fail ?

Probably due to the errors of the geometry import. The native geometry primitives are much more compact and represent the solid more accurately.

Post by Frank Richter
For symmetry reasons it is sufficient to import only one eigth of
the total geometry and then use Sweep/Extrude. Will that do the
trick?

Probably, yes. But try getting a *.sat version of your model and using that first, it will save you many headaches.

Hope this helps,
Fernando

[Danny Levine]

Minor point, but *.sat is not Parasolid.

Parasolid files have a *.x_t file naming convention. The ACIS modeling kernel uses filenames of the form *.sat.

I agree that IGES is often problematic, and use Parasolid models almost exclusively. Note that some CAD import options require an extra-cost license from Simulia.

DLL

Danny L. Levine, Ph.D., P.E.
Principal Engineer
Zimmer, Inc.

//www.zimmer.com<//www.zimmer.com/>
[phone] - Office
[phone] - Cell

From: ***@yahoogroups.com [mailto:***@yahoogroups.com] On Behalf Of fcn_public
Sent: Sunday, August 18, 2013 9:46 AM
To: ***@yahoogroups.com
Subject: [Caution: Message contains Suspicious URL content] [Abaqus] Re: Automatic meshing impossible, need C3D8



Hi Frank,

Post by Frank Richter
we want to simulate the loading of a specimen of circular cross
section which is tapered in the central section and has additional
notches on two vertical opposing faces in that central section.
Hence, the specimen is not axisymmetric any longer. I have to use
continuum elements.
I import the geometry from a iges file and obtain: "The Part
UFTE_SN contains imprecise geometry, which is highlighted.
Partitioning and quad/hex meshing using the medial axis algorithm
may fail on imprecise parts."

[...]

Post by Frank Richter
Should I import the geometry from another CAD file type ? Which one is best suited ?

ABAQUS uses parasolid (*.sat) for its geometry, so use that if possible. Generally speaking, avoid IGES if possible (use STEP if there is no other choice). IGES is about the worst geometry format on earth, as it is different from vendor to vendor (it is a very ambiguous standard!).

Post by Frank Richter
Can I have the structure meshed with C3D8 elements in an external meshing software ?

Definitely, many people do that by default. Hypermesh, Patran and many other preprocessors produce valid ABAQUS input files.

If so, why does ABAQUS fail ?

Probably due to the errors of the geometry import. The native geometry primitives are much more compact and represent the solid more accurately.

Post by Frank Richter
For symmetry reasons it is sufficient to import only one eigth of
the total geometry and then use Sweep/Extrude. Will that do the
trick?

Probably, yes. But try getting a *.sat version of your model and using that first, it will save you many headaches.

Hope this helps,
Fernando



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

[fcn_public]

Dave,

Post by Danny Levine
Minor point, but *.sat is not Parasolid.
Parasolid files have a *.x_t file naming convention. The ACIS
modeling kernel uses filenames of the form *.sat.
I agree that IGES is often problematic, and use Parasolid models
almost exclusively. Note that some CAD import options require an
extra-cost license from Simulia.

You are right, of course, Parasolid is not ACIS (what was I thinking of??). Just to clarify, ABAQUS uses ACIS internally, so it will open *.sat files as native geometry.

To summarize: When using external software for modeling, use ACIS *.sat to open it natively with ABAQUS. If you need to import, use Parasolid if available, otherwise STEP. And avoid IGES as much as possible.

Sorry about the confusion with formats and extensions.
Fernando

[vikas_hcl2001]

Frank:

STEP files worked best for me; I tried SAT a few times but gave up on it. More importantly, however, I noticed that Abaqus would - on its own - decide to create tiny partitions on some faces which could only be seen after zooming in quite a bit. One easy way to tell is to use the Virtual Topology feature in the Mesh module. It lets Abaqus ignore certain features in the geometry. After ignoring those automatically generated partitions, c3d8 meshing became straightforward.

Vikas

Post by Frank Richter
Dear Group,
we want to simulate the loading of a specimen of circular cross section which is tapered in the central section and has additional notches on two vertical opposing faces in that central section. Hence, the specimen is not axisymmetric any longer. I have to use continuum elements.
I import the geometry from a iges file and obtain: "The Part UFTE_SN contains imprecise geometry, which is highlighted. Partitioning and quad/hex meshing using the medial axis algorithm may fail on imprecise parts."
I switch to Module 'Mesh' and execute 'Seed Part', then 'Mesh - Part': "The selected regions cannot be meshed automatically using the assigned element shapes. They must either be partitioned, assigned a tet shape, or manually meshed using the Create Bottom-Up Mesh tool."
1) I did achieve to have the structure meshed with tetrahedral elements C3D10 or C3D4. The simulation results are miserable. Part of the central section is radially squeezed out. The material is elastic-plastic, and the message file states the typical
***WARNING: THE STRAIN INCREMENT HAS EXCEEDED FIFTY TIMES THE STRAIN TO CAUSE FIRST YIELD AT 1397 POINTS
Element selection guidelines recommend second order elements, possibly reduced, for this type of loading. Thus, I'd need to have the stucture meshed using C3D8.
Manual 17.11.5 Creating the boundary mesh for a bottom-up region
Creating a boundary mesh: From the main menu bar, select Mesh - Region.
I end up with the same message as above and cannot continue here.
3) I did not succeed using the partitioning technique as I am totally new to these features, and options abound therein. ABAQUS is not specific in whether I have to partition edges, faces or cells. Hence I am confronted with solving a problem which I cannot clearly identify. Can anyone advise me how to proceed here ?
Should I import the geometry from another CAD file type ? Which one is best suited ?
Can I have the structure meshed with C3D8 elements in an external meshing software ? If so, why does ABAQUS fail ?
For symmetry reasons it is sufficient to import only one eigth of the total geometry and then use Sweep/Extrude. Will that do the trick ?
Thank you for sharing your expertise
Frank
-----------------------------------------------------------------------
Frank Richter
Institute of Materials Science
Ruhr-Universitaet Bochum
Bochum
Germany