Discussion:
Force vs. Displacement data for a Flat Spring
jongyonkim
2006-08-15 20:24:48 UTC
Permalink
Hi,

I'm running a simulation of unrolling a flat spring made of silicon to
obtain the system's reaction force (spring force) vs. displacement graph.

See the picture at :
Loading Image...
Loading Image...

I am currently using ABAQUS/Explicit to run the stretching analysis.
Basically, I apply a constant force on either end of the spiral and stretch
it until it completely unwinds.

Before I can dive into postprocessing, I need to know how to calculate the
(spring reaction) force vs. (spiral end) displacement of this particular
structure.

Does anyone know how to do the calculation of my flat spring? Any
recommendation on online sources / books regarding a similar spring
structure?

Also, ABAQUS/Explicit can spit out a number of data including nodal
displacement, External Work, Kinetic Energy, Internal Energy, etc.

I tried differentiating Internal Energy (of the entire structure) with
respect to displacement to get force, but that seems wrong somehow...

Thank you.
--
View this message in context: http://www.nabble.com/Force-vs.-Displacement-data-for-a-Flat-Spring-tf2111316.html#a5821378
Sent from the Abaqus Users forum at Nabble.com.
Fernando
2006-08-17 06:30:17 UTC
Permalink
Hi jongyonkim,
Post by jongyonkim
I'm running a simulation of unrolling a flat spring made of silicon
to obtain the system's reaction force (spring force) vs.
displacement graph.
I took a look at the pictures and the first thing that called my
attention was the poor mesh at the transition between the solid "disc"
and the spiral coils of your springs, you really need to improve the
mesh at those regions. Also, the elements in the coils seem very flat,
I guess you are trying to keep the mesh size reasonably slow. Bear in
mind that if the coils are subjected to bending, the solution you get
may be really bad... try to reduce the aspect ratio of those elements
if you can (measured as max dim/min dim of the element)
Post by jongyonkim
I am currently using ABAQUS/Explicit to run the stretching analysis.
Basically, I apply a constant force on either end of the spiral and
stretch it until it completely unwinds.
Just out of curiosity, why /Explicit? If you fix the center node/axis
and apply loads or displacements to the coil ends, you should be able
to solve your problem in /Standard (this is "safer", and has been
discussed extensively in the past, see the archives).
Post by jongyonkim
Before I can dive into postprocessing, I need to know how to
calculate the (spring reaction) force vs. (spiral end) displacement
of this particular structure.
Well you said you are doing a force-control simulation. So the force
is simply what you apply (assuming the center of the spring remains
fixed), and the displacement is that of the nodes where you apply the
force.

If you want the reactions, you need to impose a displacement. This
will probably be more stable, by the way.

Hope this helps,
Fernando
Ryan S
2006-08-17 13:04:10 UTC
Permalink
Hi,

FYI, there is an option in V6.6 to generate integrated output (called
Integrated Section Output, I think) across a user-specified cross section.
You should be able to ask for a total force magnitude or something.

In this particular problem though, this option is not needed. Fernando is
right: i.e. applied load equals integrated internal force since your cross
section transmits the entire load through.

Also as Fernando mentioned, you're going to get poor bending behavior unless
you modeled the thin spiral layers using continuum shells. Alternatively you
could use real shells, and transition to the solid stem via a shell-to-solid
coupling.

Very interesting-looking model, BTW.

Regards,
Ryan.
Post by Fernando
Hi jongyonkim,
Post by jongyonkim
I'm running a simulation of unrolling a flat spring made of silicon
to obtain the system's reaction force (spring force) vs.
displacement graph.
I took a look at the pictures and the first thing that called my
attention was the poor mesh at the transition between the solid "disc"
and the spiral coils of your springs, you really need to improve the
mesh at those regions. Also, the elements in the coils seem very flat,
I guess you are trying to keep the mesh size reasonably slow. Bear in
mind that if the coils are subjected to bending, the solution you get
may be really bad... try to reduce the aspect ratio of those elements
if you can (measured as max dim/min dim of the element)
Post by jongyonkim
I am currently using ABAQUS/Explicit to run the stretching analysis.
Basically, I apply a constant force on either end of the spiral and
stretch it until it completely unwinds.
Just out of curiosity, why /Explicit? If you fix the center node/axis
and apply loads or displacements to the coil ends, you should be able
to solve your problem in /Standard (this is "safer", and has been
discussed extensively in the past, see the archives).
Post by jongyonkim
Before I can dive into postprocessing, I need to know how to
calculate the (spring reaction) force vs. (spiral end) displacement
of this particular structure.
Well you said you are doing a force-control simulation. So the force
is simply what you apply (assuming the center of the spring remains
fixed), and the displacement is that of the nodes where you apply the
force.
If you want the reactions, you need to impose a displacement. This
will probably be more stable, by the way.
Hope this helps,
Fernando
[Non-text portions of this message have been removed]
BenZ
2006-08-17 23:11:35 UTC
Permalink
One can generate sections prints even with version 6.5 and older :
*SECTION PRINT,etc....

About the mesh, it may be a start point to identify the area of
interest (despite they are already known, thx Fern). The element to
use here is the C3D8I because the mesh is regular and not skewed. I
think this element has a good bending behavior...

BenZ.
Post by Ryan S
Hi,
FYI, there is an option in V6.6 to generate integrated output
(called
Post by Ryan S
Integrated Section Output, I think) across a user-specified cross section.
You should be able to ask for a total force magnitude or something.
In this particular problem though, this option is not needed.
Fernando is
Post by Ryan S
right: i.e. applied load equals integrated internal force since your cross
section transmits the entire load through.
Also as Fernando mentioned, you're going to get poor bending
behavior unless
Post by Ryan S
you modeled the thin spiral layers using continuum shells.
Alternatively you
Post by Ryan S
could use real shells, and transition to the solid stem via a
shell-to-solid
Post by Ryan S
coupling.
Very interesting-looking model, BTW.
Regards,
Ryan.
Post by Fernando
Hi jongyonkim,
Post by jongyonkim
I'm running a simulation of unrolling a flat spring made of silicon
to obtain the system's reaction force (spring force) vs.
displacement graph.
I took a look at the pictures and the first thing that called my
attention was the poor mesh at the transition between the
solid "disc"
Post by Ryan S
Post by Fernando
and the spiral coils of your springs, you really need to improve the
mesh at those regions. Also, the elements in the coils seem very flat,
I guess you are trying to keep the mesh size reasonably slow. Bear in
mind that if the coils are subjected to bending, the solution you get
may be really bad... try to reduce the aspect ratio of those
elements
Post by Ryan S
Post by Fernando
if you can (measured as max dim/min dim of the element)
Post by jongyonkim
I am currently using ABAQUS/Explicit to run the stretching
analysis.
Post by Ryan S
Post by Fernando
Post by jongyonkim
Basically, I apply a constant force on either end of the
spiral and
Post by Ryan S
Post by Fernando
Post by jongyonkim
stretch it until it completely unwinds.
Just out of curiosity, why /Explicit? If you fix the center
node/axis
Post by Ryan S
Post by Fernando
and apply loads or displacements to the coil ends, you should be able
to solve your problem in /Standard (this is "safer", and has been
discussed extensively in the past, see the archives).
Post by jongyonkim
Before I can dive into postprocessing, I need to know how to
calculate the (spring reaction) force vs. (spiral end)
displacement
Post by Ryan S
Post by Fernando
Post by jongyonkim
of this particular structure.
Well you said you are doing a force-control simulation. So the force
is simply what you apply (assuming the center of the spring
remains
Post by Ryan S
Post by Fernando
fixed), and the displacement is that of the nodes where you
apply the
Post by Ryan S
Post by Fernando
force.
If you want the reactions, you need to impose a displacement. This
will probably be more stable, by the way.
Hope this helps,
Fernando
[Non-text portions of this message have been removed]
jongyonkim
2006-08-20 01:16:23 UTC
Permalink
Thank you for all the feedback, but I would like to make clear something.

I spent a lot of time trying to figure out this seemiingly simple problem of
finding the spring force of my structure, however, I am still in need of
help.

In order to clarify what I need, I've made a simple model of a cantilever
shown in the following online photo (link)

Loading Image...

I would like to obtain data for the red-colored vector Reaction Force.

I've tried the following:
1) use Boundary Condition (fix the velocity/displacement) to pull and
extract "RF1"
-Apparently, one can extract "Reaction Forces" only if the surfaces are
bounded under a BC. My original structure, when subject to such BC,
experiences too much inertia (the heavy centerpiece mass rotates faster than
the spirals unroll, forcing the centerpiece to push the spirals out :
undesirable) for it to give accurate results.

2) use Force to pull and extract Stress, which then you can integrate to
find the force.
-There are so many kinds of stress (Mises, Equivalent Pressure Stress,
Stress Components, etc) that I don't know which of them is appropriate for
my calculation.
-If I get stress from the surface which I pull with some fixed amt of
force, how do I go about finding the "reaction force"? This should be
pointing the other direction, because the more the spirals unroll, the
greater the spring/reaction force becomes...

*I got "Section Integrated Output" to find out the total amount of force on
a surface, but unfortunately it only gives you the values of the load, not
the reaction force pointing the other direction. For example, If I have 100N
in the four corners of the surface, Section Integrated Output Total Force
gives me 400N, which is an obvious result, but this is not what I need.
So this isn't very useful to me...
Post by BenZ
*SECTION PRINT,etc....
About the mesh, it may be a start point to identify the area of
interest (despite they are already known, thx Fern). The element to
use here is the C3D8I because the mesh is regular and not skewed. I
think this element has a good bending behavior...
BenZ.
Post by Ryan S
Hi,
FYI, there is an option in V6.6 to generate integrated output
(called
Post by Ryan S
Integrated Section Output, I think) across a user-specified cross
section.
Post by Ryan S
You should be able to ask for a total force magnitude or something.
In this particular problem though, this option is not needed.
Fernando is
Post by Ryan S
right: i.e. applied load equals integrated internal force since
your cross
Post by Ryan S
section transmits the entire load through.
Also as Fernando mentioned, you're going to get poor bending
behavior unless
Post by Ryan S
you modeled the thin spiral layers using continuum shells.
Alternatively you
Post by Ryan S
could use real shells, and transition to the solid stem via a
shell-to-solid
Post by Ryan S
coupling.
Very interesting-looking model, BTW.
Regards,
Ryan.
Post by Fernando
Hi jongyonkim,
Post by jongyonkim
I'm running a simulation of unrolling a flat spring made of
silicon
Post by Ryan S
Post by Fernando
Post by jongyonkim
to obtain the system's reaction force (spring force) vs.
displacement graph.
I took a look at the pictures and the first thing that called my
attention was the poor mesh at the transition between the
solid "disc"
Post by Ryan S
Post by Fernando
and the spiral coils of your springs, you really need to improve
the
Post by Ryan S
Post by Fernando
mesh at those regions. Also, the elements in the coils seem very
flat,
Post by Ryan S
Post by Fernando
I guess you are trying to keep the mesh size reasonably slow.
Bear in
Post by Ryan S
Post by Fernando
mind that if the coils are subjected to bending, the solution
you get
Post by Ryan S
Post by Fernando
may be really bad... try to reduce the aspect ratio of those
elements
Post by Ryan S
Post by Fernando
if you can (measured as max dim/min dim of the element)
Post by jongyonkim
I am currently using ABAQUS/Explicit to run the stretching
analysis.
Post by Ryan S
Post by Fernando
Post by jongyonkim
Basically, I apply a constant force on either end of the
spiral and
Post by Ryan S
Post by Fernando
Post by jongyonkim
stretch it until it completely unwinds.
Just out of curiosity, why /Explicit? If you fix the center
node/axis
Post by Ryan S
Post by Fernando
and apply loads or displacements to the coil ends, you should be
able
Post by Ryan S
Post by Fernando
to solve your problem in /Standard (this is "safer", and has been
discussed extensively in the past, see the archives).
Post by jongyonkim
Before I can dive into postprocessing, I need to know how to
calculate the (spring reaction) force vs. (spiral end)
displacement
Post by Ryan S
Post by Fernando
Post by jongyonkim
of this particular structure.
Well you said you are doing a force-control simulation. So the
force
Post by Ryan S
Post by Fernando
is simply what you apply (assuming the center of the spring
remains
Post by Ryan S
Post by Fernando
fixed), and the displacement is that of the nodes where you
apply the
Post by Ryan S
Post by Fernando
force.
If you want the reactions, you need to impose a displacement.
This
Post by Ryan S
Post by Fernando
will probably be more stable, by the way.
Hope this helps,
Fernando
[Non-text portions of this message have been removed]
http://groups.yahoo.com/group/abaqus
Yahoo! Groups Links
--
View this message in context: http://www.nabble.com/Force-vs.-Displacement-data-for-a-Flat-Spring-tf2111316.html#a5889913
Sent from the Abaqus Users forum at Nabble.com.
BenZ
2006-08-20 11:18:01 UTC
Permalink
reactions forces are dual to BC's. In other words, there are RFs
only where there are BCs, no need to find them elsewhere.

Once again, you have to study the equilibrium of your spring and to
understand it because the only way to get the stiffness is to plot a
RF/BC graph.
If you have inertia effects this is because you do not simulate a
quasistatic process with /Explicit. So switch to /Standard !


BenZ.
Post by jongyonkim
Thank you for all the feedback, but I would like to make clear
something.
Post by jongyonkim
I spent a lot of time trying to figure out this seemiingly simple problem of
finding the spring force of my structure, however, I am still in need of
help.
In order to clarify what I need, I've made a simple model of a
cantilever
Post by jongyonkim
shown in the following online photo (link)
http://i102.photobucket.com/albums/m97/jongyonkim/reactionforce.jpg
I would like to obtain data for the red-colored vector Reaction Force.
1) use Boundary Condition (fix the velocity/displacement) to pull and
extract "RF1"
-Apparently, one can extract "Reaction Forces" only if the
surfaces are
Post by jongyonkim
bounded under a BC. My original structure, when subject to such BC,
experiences too much inertia (the heavy centerpiece mass rotates faster than
undesirable) for it to give accurate results.
2) use Force to pull and extract Stress, which then you can
integrate to
Post by jongyonkim
find the force.
-There are so many kinds of stress (Mises, Equivalent Pressure Stress,
Stress Components, etc) that I don't know which of them is
appropriate for
Post by jongyonkim
my calculation.
-If I get stress from the surface which I pull with some fixed amt of
force, how do I go about finding the "reaction force"? This should be
pointing the other direction, because the more the spirals unroll, the
greater the spring/reaction force becomes...
*I got "Section Integrated Output" to find out the total amount of force on
a surface, but unfortunately it only gives you the values of the load, not
the reaction force pointing the other direction. For example, If I have 100N
in the four corners of the surface, Section Integrated Output
Total Force
Post by jongyonkim
gives me 400N, which is an obvious result, but this is not what I need.
So this isn't very useful to me...
Post by BenZ
One can generate sections prints even with version 6.5 and
*SECTION PRINT,etc....
About the mesh, it may be a start point to identify the area of
interest (despite they are already known, thx Fern). The element to
use here is the C3D8I because the mesh is regular and not
skewed. I
Post by jongyonkim
Post by BenZ
think this element has a good bending behavior...
BenZ.
Post by Ryan S
Hi,
FYI, there is an option in V6.6 to generate integrated output
(called
Post by Ryan S
Integrated Section Output, I think) across a user-specified
cross
Post by jongyonkim
Post by BenZ
section.
Post by Ryan S
You should be able to ask for a total force magnitude or
something.
Post by jongyonkim
Post by BenZ
Post by Ryan S
In this particular problem though, this option is not needed.
Fernando is
Post by Ryan S
right: i.e. applied load equals integrated internal force since
your cross
Post by Ryan S
section transmits the entire load through.
Also as Fernando mentioned, you're going to get poor bending
behavior unless
Post by Ryan S
you modeled the thin spiral layers using continuum shells.
Alternatively you
Post by Ryan S
could use real shells, and transition to the solid stem via a
shell-to-solid
Post by Ryan S
coupling.
Very interesting-looking model, BTW.
Regards,
Ryan.
Post by Fernando
Hi jongyonkim,
Post by jongyonkim
I'm running a simulation of unrolling a flat spring made of
silicon
Post by Ryan S
Post by Fernando
Post by jongyonkim
to obtain the system's reaction force (spring force) vs.
displacement graph.
I took a look at the pictures and the first thing that called my
attention was the poor mesh at the transition between the
solid "disc"
Post by Ryan S
Post by Fernando
and the spiral coils of your springs, you really need to
improve
Post by jongyonkim
Post by BenZ
the
Post by Ryan S
Post by Fernando
mesh at those regions. Also, the elements in the coils seem very
flat,
Post by Ryan S
Post by Fernando
I guess you are trying to keep the mesh size reasonably slow.
Bear in
Post by Ryan S
Post by Fernando
mind that if the coils are subjected to bending, the solution
you get
Post by Ryan S
Post by Fernando
may be really bad... try to reduce the aspect ratio of those
elements
Post by Ryan S
Post by Fernando
if you can (measured as max dim/min dim of the element)
Post by jongyonkim
I am currently using ABAQUS/Explicit to run the stretching
analysis.
Post by Ryan S
Post by Fernando
Post by jongyonkim
Basically, I apply a constant force on either end of the
spiral and
Post by Ryan S
Post by Fernando
Post by jongyonkim
stretch it until it completely unwinds.
Just out of curiosity, why /Explicit? If you fix the center
node/axis
Post by Ryan S
Post by Fernando
and apply loads or displacements to the coil ends, you should be
able
Post by Ryan S
Post by Fernando
to solve your problem in /Standard (this is "safer", and has been
discussed extensively in the past, see the archives).
Post by jongyonkim
Before I can dive into postprocessing, I need to know how to
calculate the (spring reaction) force vs. (spiral end)
displacement
Post by Ryan S
Post by Fernando
Post by jongyonkim
of this particular structure.
Well you said you are doing a force-control simulation. So the
force
Post by Ryan S
Post by Fernando
is simply what you apply (assuming the center of the spring
remains
Post by Ryan S
Post by Fernando
fixed), and the displacement is that of the nodes where you
apply the
Post by Ryan S
Post by Fernando
force.
If you want the reactions, you need to impose a displacement.
This
Post by Ryan S
Post by Fernando
will probably be more stable, by the way.
Hope this helps,
Fernando
[Non-text portions of this message have been removed]
http://groups.yahoo.com/group/abaqus
Yahoo! Groups Links
--
View this message in context: http://www.nabble.com/Force-vs.-
Displacement-data-for-a-Flat-Spring-tf2111316.html#a5889913
Post by jongyonkim
Sent from the Abaqus Users forum at Nabble.com.
Fernando
2006-08-21 06:52:12 UTC
Permalink
Hi Yongyokim,
Post by BenZ
reactions forces are dual to BC's. In other words, there are RFs
only where there are BCs, no need to find them elsewhere.
Once again, you have to study the equilibrium of your spring and to
understand it because the only way to get the stiffness is to plot a
RF/BC graph.
If you have inertia effects this is because you do not simulate a
quasistatic process with /Explicit. So switch to /Standard !
I fully agree with Ben and support switching to /Standard, if you want
a "clean" force-displacement curve. Try the following (in /Standard):
fix the axis of your spring, so that, if left alone, it can rotate.
This should be easy, given that you have a swept mesh (2.5D). If you
don't have a node at the axis location, it is easy to define a
reference node and remesh (tip: use the chance to improve the
transition regions as well). Then apply displacement BC to the ends of
the coils. This way you impose a quasistatic loading on the spring and
mass/inertial effects disappear (in fact, you don't even need to
define the mass then!). As a result of imposing displacements on the
coils, you will get reaction forces there, which what you need.

Regarding the stresses, if your spring is made of metal (which I
assume), stick with Mises stresses. The whole point of a coil is that
it remains in elastic range, so I don't think plasticity is an issue
here...

Hope this helps,
Fernando
Christer Gustafsson
2006-08-21 08:23:39 UTC
Permalink
Hi Yongyokim,

The model suggested by BenZ and Fernando has the advantage that is has
been treated analytically, so you can verify the outcome of your FEM
analysis.

You find the theory e.g. in A.E.H. Love "A treatise on the mathematical
theory of elasticity" in paragraphs 270 and 271 and fig 59, which book
is usually found in academic library. You find expressions both for the
axial reaction force and the reacting bending moment in addition to
those for the displacement of the centre line.

ChG
Post by BenZ
http://groups.yahoo.com/group/abaqus
Yahoo! Groups Links
jongyonkim
2006-08-21 19:57:35 UTC
Permalink
It looks like rather than /Explicit, /Standard is recommended.

However, I have no experience with using /Standard, because the biggest
reason why I considered /Explicit was its automatic stability.

After hearing from Fernado-15, I tried using /Standard (Dynamic, Implicit),
but to my horror, the structure failed to converge due to many "negative
eigenvalue" problems.

Judging from the geometry and nonlinear stretching behavior of the
structure, I don't think I can succeed with /Standard.

1) Any more suggestions with /Explicit? If I use Force to pull the ends, I
can't get the "reaction force" output/vectors... If I use BC (fix
velocity/displacement), the centerpiece inertia messes up the unwinding...

Also, the "reaction force" vectors seem to point the opposite way...when
looking at RF, does it mean "reaction force ON the structure by the external
entity" or "reaction force caused BY the structure on the external entity?"
It seems like ABAQUS is showing the former, but the latter is what I need
since I'm measuring the spring reaction force. If it's the former, can I
simply flip the sign (change the direction of the vector) and consider it as
the spring reaction force?

2) If you have experience dealing with this kind of coil structure using
/Standard, how do you stabilize the simulation (i.e. not get "negative
eigenvalue" error messages)?

Thank you for showing interest in my inquiry.
I appreciate your help.
Post by Fernando
Hi Yongyokim,
The model suggested by BenZ and Fernando has the advantage that is has
been treated analytically, so you can verify the outcome of your FEM
analysis.
You find the theory e.g. in A.E.H. Love "A treatise on the mathematical
theory of elasticity" in paragraphs 270 and 271 and fig 59, which book
is usually found in academic library. You find expressions both for the
axial reaction force and the reacting bending moment in addition to
those for the displacement of the centre line.
ChG
Post by BenZ
http://groups.yahoo.com/group/abaqus
Yahoo! Groups Links
http://groups.yahoo.com/group/abaqus
Yahoo! Groups Links
--
View this message in context: http://www.nabble.com/Force-vs.-Displacement-data-for-a-Flat-Spring-tf2111316.html#a5913737
Sent from the Abaqus Users forum at Nabble.com.
Fernando
2006-08-22 14:28:51 UTC
Permalink
Yongyokim,
Post by jongyonkim
However, I have no experience with using /Standard, because the
biggest reason why I considered /Explicit was its automatic
stability.
After hearing from Fernado-15, I tried using /Standard (Dynamic,
Implicit), but to my horror, the structure failed to converge due to
many "negative eigenvalue" problems.
Judging from the geometry and nonlinear stretching behavior of the
structure, I don't think I can succeed with /Standard.
/Standard corresponds exactly with what basic textbooks in numerical
analysis and FE try to teach. Of course it includes more advanced
materials, interactions and procedures, but the essentials are the
same. /Explicit uses a completely different technique (which requires
*much* more advanced knowledge to harness).

Also, don't be tempted by the "automatic stability" of /Explicit: it
will *always* give you results, and not tell you whether you can trust
that solution at all! With /Standard, at least you have the warranty
that, if you get a solution, it corresponds to the problem you input
(of course, you can always input the wrong problem, but there's
nothing the code can do about that!). If you are still lost, I would
strongly recommend you attend some seminar or class on basic FEM
before you go any further with ABAQUS.

After the small rant/defense of /Standard, let's go back to your
problem. Is there any reason at all that you need to consider
mass/inertial effects? I understand you want a force-displacement
curve. In that case, use /Standard in a STATIC analysis, and get rid
of all the mass definitions (or comment them out adding a ** at the
beginning of each relevant line in the *inp file). As I suggested in
my previous post, do the following: use BC to fix all the displacement
GDL's of the nodes at the rotation axis of the spring. If you don't
define any additional BC's, you will get errors saying there are
negative eigenvalues. In /Standard, under these circumstances, this
means you have rigid body motions, which is true as your spring can
rotate around its axis. Now impose displacement BC's on the spring
coils. As a result, the rigid body motions disappear. As you are
imposing displacement BC's, you get reaction forces on those nodes.
That's the output you want (the displacement part of the curve is what
you impose).

As an added bonus, you also get reactions at the axis, so you can
analyze what happens if you set, for example, "uneven uncoiling" by
imposing a different displacement on each coil...

By the way, even if you *do* need the inertial effects, the usual
approach in an engineering problem is to look at the static behavior
of the system first. Once you know how that works, you go on with the
next step: define mass properties and analyze the dynamic behavior,
obtaining eigenfrequencies and eigenmodes.

Hope this helps,
Fernando
BenZ
2006-08-22 22:35:12 UTC
Permalink
I do agree with you Fern. But let's remember that even in /Standard
the solution may depend on the size of increments for path-dependent
formulations (plasticity, contact definition...) and for large
strains (linear approximation of the rotation and strain rates
within the increment).

About the initial discussion, Yongyokim has clarify if he wants or
not the dynamic effects and why he uses /Explicit. /Explicit has
NO "automatic stability", /Explicit works with a supposed "stable"
time increment, so it is only "stable under conditions". /Standard
is always stable, but, of course as Fern said, with regard to the
formulations used.

Now I think this topic is nearly closed because Fern has given the
whole analysis technique for the spring !! Thx to him !

BenZ.
Post by Fernando
Yongyokim,
Post by jongyonkim
However, I have no experience with using /Standard, because the
biggest reason why I considered /Explicit was its automatic
stability.
After hearing from Fernado-15, I tried using /Standard (Dynamic,
Implicit), but to my horror, the structure failed to converge due to
many "negative eigenvalue" problems.
Judging from the geometry and nonlinear stretching behavior of the
structure, I don't think I can succeed with /Standard.
/Standard corresponds exactly with what basic textbooks in
numerical
Post by Fernando
analysis and FE try to teach. Of course it includes more advanced
materials, interactions and procedures, but the essentials are the
same. /Explicit uses a completely different technique (which
requires
Post by Fernando
*much* more advanced knowledge to harness).
Also, don't be tempted by the "automatic stability" of /Explicit: it
will *always* give you results, and not tell you whether you can trust
that solution at all! With /Standard, at least you have the
warranty
Post by Fernando
that, if you get a solution, it corresponds to the problem you
input
Post by Fernando
(of course, you can always input the wrong problem, but there's
nothing the code can do about that!). If you are still lost, I
would
Post by Fernando
strongly recommend you attend some seminar or class on basic FEM
before you go any further with ABAQUS.
After the small rant/defense of /Standard, let's go back to your
problem. Is there any reason at all that you need to consider
mass/inertial effects? I understand you want a force-displacement
curve. In that case, use /Standard in a STATIC analysis, and get rid
of all the mass definitions (or comment them out adding a ** at the
beginning of each relevant line in the *inp file). As I suggested in
my previous post, do the following: use BC to fix all the
displacement
Post by Fernando
GDL's of the nodes at the rotation axis of the spring. If you don't
define any additional BC's, you will get errors saying there are
negative eigenvalues. In /Standard, under these circumstances, this
means you have rigid body motions, which is true as your spring can
rotate around its axis. Now impose displacement BC's on the spring
coils. As a result, the rigid body motions disappear. As you are
imposing displacement BC's, you get reaction forces on those nodes.
That's the output you want (the displacement part of the curve is what
you impose).
As an added bonus, you also get reactions at the axis, so you can
analyze what happens if you set, for example, "uneven uncoiling" by
imposing a different displacement on each coil...
By the way, even if you *do* need the inertial effects, the usual
approach in an engineering problem is to look at the static
behavior
Post by Fernando
of the system first. Once you know how that works, you go on with the
next step: define mass properties and analyze the dynamic behavior,
obtaining eigenfrequencies and eigenmodes.
Hope this helps,
Fernando
Loading...