Discussion Closed This discussion was created more than 6 months ago and has been closed. To start a new discussion with a link back to this one, click here.
Using Norton Bailey Law: How to determine the Reference stress
Posted 19 mar 2014, 04:04 GMT-4 Parameters, Variables, & Functions, Structural Mechanics 3 Replies
Please login with a confirmed email address before reporting spam
Hello all;
Can anyone tell me that what does that mean by "Reference stress" in Creep modeling?
How to determine it? Usually, Material constant "A" and "m" are used for creep.
Can anyone tell me that what does that mean by "Reference stress" in Creep modeling?
How to determine it? Usually, Material constant "A" and "m" are used for creep.
3 Replies Last Post 20 mar 2014, 06:09 GMT-4
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
As you say, Norton's law is commonly expresses the strain rate
where
is the stress. When given material data on this form it is necessary that you explicitly say in what unit the stress is measured, e.g. [MPa]. The unit of A' is usually not explicitly stated, since with m being a real number, the constant A' will have a weird unit, like MPa^(-5.2)s^-1. This means that converting A' to another set of units (even within the SI system) is difficult.
Since COMSOL is aware of units, and does internal unit conversions, this form of entering the creep data is not suitable. Instead we use an auxiliary reference stress for making the power function nondimensional.
If your material law is given with respect to [MPa], the easiest reference stress to use is 1[MPa], since the numerical value of A is then the same as A' in your original data. The unit of A is however 1/s.
There is also another common set of data for the creep law: In addition to the exponent, you get the stress which gives a certain creep strain rate. E.g.
is the stress that gives a creep strain rate of 10^-7 h^-1. Data on this form is also easy to enter: You set the reference stress to , and A to 1E-7[h^-1].
Regards,
Henrik
As you say, Norton's law is commonly expresses the strain rate
where
is the stress. When given material data on this form it is necessary that you explicitly say in what unit the stress is measured, e.g. [MPa]. The unit of A' is usually not explicitly stated, since with m being a real number, the constant A' will have a weird unit, like MPa^(-5.2)s^-1. This means that converting A' to another set of units (even within the SI system) is difficult.Since COMSOL is aware of units, and does internal unit conversions, this form of entering the creep data is not suitable. Instead we use an auxiliary reference stress for making the power function nondimensional.
If your material law is given with respect to [MPa], the easiest reference stress to use is 1[MPa], since the numerical value of A is then the same as A' in your original data. The unit of A is however 1/s.
There is also another common set of data for the creep law: In addition to the exponent, you get the stress which gives a certain creep strain rate. E.g.
is the stress that gives a creep strain rate of 10^-7 h^-1. Data on this form is also easy to enter: You set the reference stress to , and A to 1E-7[h^-1].Regards,
Henrik
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Dear Henrik,
Your detailed answer is highly appreciated! Does the same apply to "Reference Time" when using the Time hardening formulations? Why we use the "Time Offset"?
Lastly, does the auto setting for solver always work well when solving these kind of problems OR we need to set the solver settings?
Thanks again.
Your detailed answer is highly appreciated! Does the same apply to "Reference Time" when using the Time hardening formulations? Why we use the "Time Offset"?
Lastly, does the auto setting for solver always work well when solving these kind of problems OR we need to set the solver settings?
Thanks again.
Please login with a confirmed email address before reporting spam
Posted:
1 decade ago
Hi,
Yes, the idea with the reference time, is the same. Using it avoids non-integer time units in the coefficient.
The offset in time serves two purposes, both related to that the Norton-Bailey law has very fast changes in the strain rate for small times.
1. A small value can be used to avoid the infinite strain rates that you could get at t=0. That part of the Norton-Bailey law is not well behaved in the numerical sense. Note that the time integral of the strain rate is still bounded, since the singularity is weak, so the physics is sound. The solver will however experience severe problems with infinite strain rates.
2. It is possible to start up a simulation for a material which has already been subjected to part of the primary creep period.
For anything but linear problems it would be optimistic to say that the default solver settings always work. For a creep problem the default settings will however in most cases work well. Just keep in mind that you should not have too large creep strain increments within a single time step. If required, this can be controlled either by limiting time steps, or by sharpening tolerances.
Regards,
Henrik
Yes, the idea with the reference time, is the same. Using it avoids non-integer time units in the coefficient.
The offset in time serves two purposes, both related to that the Norton-Bailey law has very fast changes in the strain rate for small times.
1. A small value can be used to avoid the infinite strain rates that you could get at t=0. That part of the Norton-Bailey law is not well behaved in the numerical sense. Note that the time integral of the strain rate is still bounded, since the singularity is weak, so the physics is sound. The solver will however experience severe problems with infinite strain rates.
2. It is possible to start up a simulation for a material which has already been subjected to part of the primary creep period.
For anything but linear problems it would be optimistic to say that the default solver settings always work. For a creep problem the default settings will however in most cases work well. Just keep in mind that you should not have too large creep strain increments within a single time step. If required, this can be controlled either by limiting time steps, or by sharpening tolerances.
Regards,
Henrik