Menu

Discussion Forum

New Discussion
Filtra

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.

"Failed to find consistent initial values"

Posted 12 dic 2014, 12:43 GMT-5 Fluid & Heat Version 5.0 23 Replies

Gertjan van Zwieten
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

On a 2D unit square domain with an laminar flow model (incompressible, rho=1, mu=1e-2) and two sets of periodic flow conditions (i.e. both horizontal and vertical) I am trying to get a time dependent study going. However with any set of initial values other than u=v=p=0 I get an error "Failed to find consistent initial values. Last time step is not converged. - Feature: Time-Dependent Solver 1 (sol1/t1)". Failure cases include the stationary solution u=1, v=p=0. I would greatly appreciate it if anybody could clarify what is going wrong here because I am out of ideas. Thanks!
23 Replies Last Post 16 nov 2016, 05:16 GMT-5
Gertjan van Zwieten
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 13 dic 2014, 11:39 GMT-5
In fact *any* sort of working example with periodicity in flow direction would help me out tremendously. No matter what I try, I keep running into the "consistent initial values" brick wall that I completely fail to understand (and I have done similar things in other codes without problems). Anything that helps lead me around this issue is greatly appreciated.
Again, the most basic form of the problem is 2D incompressible flow on a fully periodic domain, failing with a uniform flow initial value.
Thanks.
In fact *any* sort of working example with periodicity in flow direction would help me out tremendously. No matter what I try, I keep running into the "consistent initial values" brick wall that I completely fail to understand (and I have done similar things in other codes without problems). Anything that helps lead me around this issue is greatly appreciated. Again, the most basic form of the problem is 2D incompressible flow on a fully periodic domain, failing with a uniform flow initial value. Thanks.
Gertjan van Zwieten
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 13 dic 2014, 15:57 GMT-5
Related. A unit square with no slip walls top and bottom and periodic flow condition left and right with no pressure jump, but with a volume force F = [1,0] (which should amount to the same thing) and selecting incompressible flow, neglected inertial terms (Stokes flow), density=1 and viscosity=1. Solving for a stationary solution should yield a Poiseuille profile. Instead it gives: "Failed to find a solution. Maximum number of Newton iterations reached." How come Newton iterations are even used on a linear problem?
Genuinely seeking to understand and find possible ways around these issues.
Related. A unit square with no slip walls top and bottom and periodic flow condition left and right with no pressure jump, but with a volume force F = [1,0] (which should amount to the same thing) and selecting incompressible flow, neglected inertial terms (Stokes flow), density=1 and viscosity=1. Solving for a stationary solution should yield a Poiseuille profile. Instead it gives: "Failed to find a solution. Maximum number of Newton iterations reached." How come Newton iterations are even used on a linear problem? Genuinely seeking to understand and find possible ways around these issues.
Gertjan van Zwieten
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 13 dic 2014, 19:22 GMT-5
Progress: my issues may be version related. I just tried a different computer with 4.3 installed and suddenly get solutions. Saving the model and loading in 4.4 brings back the error. I will investigate this further tomorrow.
Progress: my issues may be version related. I just tried a different computer with 4.3 installed and suddenly get solutions. Saving the model and loading in 4.4 brings back the error. I will investigate this further tomorrow.
Gertjan van Zwieten
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 14 dic 2014, 09:34 GMT-5
Dear forum
I can now confirm that the problem is version related, having tested on two independent machines, one windows 64 bit, the other linux 32 bit. All periodic flow problems I tried succeed for version 4.3a and fail for 4.3b and 4.4. Unfortunately I cannot test version 5 due to license constraints.
In absence of anything resembling a bug tracking system I will document my findings here hoping that somebody will pick it up. Meanwhile I will instruct my students to downgrade their systems.

STEPS TO REPRODUCE
- In model wizard select 2D, Laminar flow, Time dependent.
- Under Geometry add a 1x1 square.
- Under Laminar flow select incompressible, and set Fluid properties to rho=1, mu=1.
- Add a periodic flow condition on boundary 1 and 4, and another on 2 and 3.
- Set initial conditions u=1, v=0, p=0.
Leave the rest at default. Computation succeeds for Comsol 4.3a, but fails for 4.3b and 4.4 indicating "Failed to find consistent initial values".
Dear forum I can now confirm that the problem is version related, having tested on two independent machines, one windows 64 bit, the other linux 32 bit. All periodic flow problems I tried succeed for version 4.3a and fail for 4.3b and 4.4. Unfortunately I cannot test version 5 due to license constraints. In absence of anything resembling a bug tracking system I will document my findings here hoping that somebody will pick it up. Meanwhile I will instruct my students to downgrade their systems. STEPS TO REPRODUCE - In model wizard select 2D, Laminar flow, Time dependent. - Under Geometry add a 1x1 square. - Under Laminar flow select incompressible, and set Fluid properties to rho=1, mu=1. - Add a periodic flow condition on boundary 1 and 4, and another on 2 and 3. - Set initial conditions u=1, v=0, p=0. Leave the rest at default. Computation succeeds for Comsol 4.3a, but fails for 4.3b and 4.4 indicating "Failed to find consistent initial values".
Edwin Khoo
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 19 dic 2014, 17:53 GMT-5
Try setting the initial time step to something small. This can be found under Time-Dependent Solver > Initial Step and check the box and specify an initial time step.
Try setting the initial time step to something small. This can be found under Time-Dependent Solver > Initial Step and check the box and specify an initial time step.
Steve Conrad
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 19 dic 2014, 19:58 GMT-5
Post or send a copy of your model, and I will look at it. I have 4.4 and 5.0 installed.

--
Steven Conrad, MD PhD
LSU Health
Post or send a copy of your model, and I will look at it. I have 4.4 and 5.0 installed. -- Steven Conrad, MD PhD LSU Health
Nagi Elabbasi Facebook Reality Labs
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 22 dic 2014, 10:20 GMT-5
Dear Gertjam,

I believe the problem is that there is no unique value for the pressure. If you set a Pressure Point Constraint to zero at any point it works.

Nagi Elabbasi
Veryst Engineering
Dear Gertjam, I believe the problem is that there is no unique value for the pressure. If you set a Pressure Point Constraint to zero at any point it works. Nagi Elabbasi Veryst Engineering
Gertjan van Zwieten
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 23 dic 2014, 09:19 GMT-5

Try setting the initial time step to something small. This can be found under Time-Dependent Solver > Initial Step and check the box and specify an initial time step.


Hi Edwin, thanks for the advice. Unfortunately the error did not go away with an initial step as low as 1e-10. Could you perhaps explain the rationale behind this suggestion?
[QUOTE] Try setting the initial time step to something small. This can be found under Time-Dependent Solver > Initial Step and check the box and specify an initial time step. [/QUOTE] Hi Edwin, thanks for the advice. Unfortunately the error did not go away with an initial step as low as 1e-10. Could you perhaps explain the rationale behind this suggestion?
Gertjan van Zwieten
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 23 dic 2014, 09:23 GMT-5

Post or send a copy of your model, and I will look at it. I have 4.4 and 5.0 installed.


Hi Steve, thanks for the offer. Please find attached a model file corresponding to "steps to reproduce".
[QUOTE] Post or send a copy of your model, and I will look at it. I have 4.4 and 5.0 installed. [/QUOTE] Hi Steve, thanks for the offer. Please find attached a model file corresponding to "steps to reproduce".
Gertjan van Zwieten
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 23 dic 2014, 09:28 GMT-5

I believe the problem is that there is no unique value for the pressure. If you set a Pressure Point Constraint to zero at any point it works.


Hi Nagi, the pressure singularity should be an issue for stationary problems only; for time dependent problems the pressure is constrained at t=0 by the initial condition.
[QUOTE] I believe the problem is that there is no unique value for the pressure. If you set a Pressure Point Constraint to zero at any point it works. [/QUOTE] Hi Nagi, the pressure singularity should be an issue for stationary problems only; for time dependent problems the pressure is constrained at t=0 by the initial condition.
Nagi Elabbasi Facebook Reality Labs
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 23 dic 2014, 10:14 GMT-5
Hi Gertjan,

Not if you have an incompressible fluid formulation. A uniform increase in pressure at any time is still a solution even in the time dependent problem.

Nagi Elabbasi
Veryst Engineering
Hi Gertjan, Not if you have an incompressible fluid formulation. A uniform increase in pressure at any time is still a solution even in the time dependent problem. Nagi Elabbasi Veryst Engineering
Gertjan van Zwieten
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 10 years ago 23 dic 2014, 10:45 GMT-5

Not if you have an incompressible fluid formulation. A uniform increase in pressure at any time is still a solution even in the time dependent problem.


Well that's embarrassing. I humbly stand corrected, and thank you very much for pointing this out. The reason I got away with the setup earlier was the use of a Krylov solver, but indeed the systems were always singular. Mystery solved. Thanks to all who offered to help out!
[QUOTE] Not if you have an incompressible fluid formulation. A uniform increase in pressure at any time is still a solution even in the time dependent problem. [/QUOTE] Well that's embarrassing. I humbly stand corrected, and thank you very much for pointing this out. The reason I got away with the setup earlier was the use of a Krylov solver, but indeed the systems were always singular. Mystery solved. Thanks to all who offered to help out!
Andrea Cugno
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 9 years ago 10 mag 2016, 10:20 GMT-4
"The reason I got away with the setup earlier was the use of a Krylov solver, but indeed the systems were always singular."

Hello,
I got a quite similar problem. Could you explain better how do you solve it?
How did you change the setting in the solver?

Thanks!
"The reason I got away with the setup earlier was the use of a Krylov solver, but indeed the systems were always singular." Hello, I got a quite similar problem. Could you explain better how do you solve it? How did you change the setting in the solver? Thanks!
Jeff Hiller COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 9 years ago 11 mag 2016, 08:07 GMT-4
Hello Andrea,
Nagi's post of 12/22/14 gives the solution: you don't change any setting on the solver, but rather you constrain the pressure at some point to eliminate the singularity.
Jeff
Hello Andrea, Nagi's post of 12/22/14 gives the solution: you don't change any setting on the solver, but rather you constrain the pressure at some point to eliminate the singularity. Jeff
Andrea Cugno
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 9 years ago 11 mag 2016, 09:46 GMT-4
Thank you for your quick answer...

How to do that?
perhaps by mean a pointwise constraint?

Thanks!

Andrea
Thank you for your quick answer... How to do that? perhaps by mean a pointwise constraint? Thanks! Andrea
Jeff Hiller COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 9 years ago 11 mag 2016, 10:31 GMT-4
Again, it's all in Nagi's post of 12/22/14: you use a Pressure Point Constraint.
Jeff
Again, it's all in Nagi's post of 12/22/14: you use a Pressure Point Constraint. Jeff
Andrea Cugno
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 9 years ago 11 mag 2016, 10:55 GMT-4
I said that I'm doing something similar not the same thing...

I'm solving the problem with the PDE coefficient form toolbox, so I don't think that there is a possibility to set a pressure constraint...

Again, do I have to do that with a pointwise constraint or something? How ca I do with PDE Coefficient for tool?

Thanks.
I said that I'm doing something similar not the same thing... I'm solving the problem with the PDE coefficient form toolbox, so I don't think that there is a possibility to set a pressure constraint... Again, do I have to do that with a pointwise constraint or something? How ca I do with PDE Coefficient for tool? Thanks.
Jeff Hiller COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 9 years ago 11 mag 2016, 11:43 GMT-4
I had indeed presumed that by "quite similar" you meant you were encountering the same error message while working with the laminar incompressible flow physics interface due to a lack of a reference pressure in your model. Otherwise, it's hard to say, it depends not only on what equations you are trying to set up but also how you are going about it. It could be as simple as setting a Dirichlet BC, or the solution may be different.
Jeff
I had indeed presumed that by "quite similar" you meant you were encountering the same error message while working with the laminar incompressible flow physics interface due to a lack of a reference pressure in your model. Otherwise, it's hard to say, it depends not only on what equations you are trying to set up but also how you are going about it. It could be as simple as setting a Dirichlet BC, or the solution may be different. Jeff
Andrea Cugno
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 9 years ago 11 mag 2016, 12:12 GMT-4
Thanks for replying...

Let me explain better, maybe I have been a bit hermetic.

I'm trying to solve a coupled problem in which the two set of equation are:
-The navier stokes equation in which the forcing terms is coupled with another field that has another own (2nd) equation. Finally there is the incompressibility constraint (div(v)=0)
The geometry is a circle domain with dirichlet boundary condition on v and Neumann boundary condition for the other field.

I followed the following procedures:

1I Wrote the equation in the PDE coefficient form in which also the hydrostatic pressure is a dependent variable. The equation for it in the coefficient form will be everything equal to zero a part of the forcing term equal to the divergence of v.
I tried to solve the problem with the initial condition (compatible with the boundary condition) exactly equal to the solution that I had in the time independent solver.

2.Write the equation in the coefficient form in which the hydrostatic pressure is taken into account as a Lagrangian multiplier with a weak constraint on the divergence of v and repeat the same strategy with the initial condition.

In both case the code find a correct let me say "static" solution but has a problem at the initial time step
("Failed to find consistent initial values") with the time dependent solver.

3. Same strategy but pointwise constraint, the code doesn't find a solution in a reasonable time.

I can't attach the code...

Thank you in advance.
Andrea
Thanks for replying... Let me explain better, maybe I have been a bit hermetic. I'm trying to solve a coupled problem in which the two set of equation are: -The navier stokes equation in which the forcing terms is coupled with another field that has another own (2nd) equation. Finally there is the incompressibility constraint (div(v)=0) The geometry is a circle domain with dirichlet boundary condition on v and Neumann boundary condition for the other field. I followed the following procedures: 1I Wrote the equation in the PDE coefficient form in which also the hydrostatic pressure is a dependent variable. The equation for it in the coefficient form will be everything equal to zero a part of the forcing term equal to the divergence of v. I tried to solve the problem with the initial condition (compatible with the boundary condition) exactly equal to the solution that I had in the time independent solver. 2.Write the equation in the coefficient form in which the hydrostatic pressure is taken into account as a Lagrangian multiplier with a weak constraint on the divergence of v and repeat the same strategy with the initial condition. In both case the code find a correct let me say "static" solution but has a problem at the initial time step ("Failed to find consistent initial values") with the time dependent solver. 3. Same strategy but pointwise constraint, the code doesn't find a solution in a reasonable time. I can't attach the code... Thank you in advance. Andrea
Jeff Hiller COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 9 years ago 12 mag 2016, 09:33 GMT-4
Alas, without knowing what equations you are solving and precisely how you are implementing them in COMSOL, users of this Forum cannot offer much useful help - at best you'll get wild guesses that may send you in the wrong direction.
Note that you can clear all solutions from your .mph files (By using the button on the Study ribbon) to make them small enough to post here.
Best,
Jeff
Alas, without knowing what equations you are solving and precisely how you are implementing them in COMSOL, users of this Forum cannot offer much useful help - at best you'll get wild guesses that may send you in the wrong direction. Note that you can clear all solutions from your .mph files (By using the button on the Study ribbon) to make them small enough to post here. Best, Jeff
Amitesh Kumar
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 8 years ago 2 set 2016, 14:49 GMT-4

I am facing a same issue .

"Failed to find consistent initial values.
Segregated group 1

System matrix is zero.
Last time step is not converged."


I am trying to apply a series of voltage values on certain time steps .But i am stuck at this error.



Alas, without knowing what equations you are solving and precisely how you are implementing them in COMSOL, users of this Forum cannot offer much useful help - at best you'll get wild guesses that may send you in the wrong direction.
Note that you can clear all solutions from your .mph files (By using the button on the Study ribbon) to make them small enough to post here.
Best,
Jeff


I am facing a same issue . "Failed to find consistent initial values. Segregated group 1 System matrix is zero. Last time step is not converged." I am trying to apply a series of voltage values on certain time steps .But i am stuck at this error. [QUOTE] Alas, without knowing what equations you are solving and precisely how you are implementing them in COMSOL, users of this Forum cannot offer much useful help - at best you'll get wild guesses that may send you in the wrong direction. Note that you can clear all solutions from your .mph files (By using the button on the Study ribbon) to make them small enough to post here. Best, Jeff [/QUOTE]
Bill
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 8 years ago 15 nov 2016, 04:32 GMT-5

Thanks for replying...

Let me explain better, maybe I have been a bit hermetic.

I'm trying to solve a coupled problem in which the two set of equation are:
-The navier stokes equation in which the forcing terms is coupled with another field that has another own (2nd) equation. Finally there is the incompressibility constraint (div(v)=0)
The geometry is a circle domain with dirichlet boundary condition on v and Neumann boundary condition for the other field.

I followed the following procedures:

1I Wrote the equation in the PDE coefficient form in which also the hydrostatic pressure is a dependent variable. The equation for it in the coefficient form will be everything equal to zero a part of the forcing term equal to the divergence of v.
I tried to solve the problem with the initial condition (compatible with the boundary condition) exactly equal to the solution that I had in the time independent solver.

2.Write the equation in the coefficient form in which the hydrostatic pressure is taken into account as a Lagrangian multiplier with a weak constraint on the divergence of v and repeat the same strategy with the initial condition.

In both case the code find a correct let me say "static" solution but has a problem at the initial time step
("Failed to find consistent initial values") with the time dependent solver.

3. Same strategy but pointwise constraint, the code doesn't find a solution in a reasonable time.

I can't attach the code...

Thank you in advance.
Andrea

Hi Andrea,
I have met a similar notification telling that "Failed to find consistent initial values" with PDE equations;
Have you solved it ? and could you please give me a hint?
Thank you in advance.
Best Regards,
Bill
[QUOTE] Thanks for replying... Let me explain better, maybe I have been a bit hermetic. I'm trying to solve a coupled problem in which the two set of equation are: -The navier stokes equation in which the forcing terms is coupled with another field that has another own (2nd) equation. Finally there is the incompressibility constraint (div(v)=0) The geometry is a circle domain with dirichlet boundary condition on v and Neumann boundary condition for the other field. I followed the following procedures: 1I Wrote the equation in the PDE coefficient form in which also the hydrostatic pressure is a dependent variable. The equation for it in the coefficient form will be everything equal to zero a part of the forcing term equal to the divergence of v. I tried to solve the problem with the initial condition (compatible with the boundary condition) exactly equal to the solution that I had in the time independent solver. 2.Write the equation in the coefficient form in which the hydrostatic pressure is taken into account as a Lagrangian multiplier with a weak constraint on the divergence of v and repeat the same strategy with the initial condition. In both case the code find a correct let me say "static" solution but has a problem at the initial time step ("Failed to find consistent initial values") with the time dependent solver. 3. Same strategy but pointwise constraint, the code doesn't find a solution in a reasonable time. I can't attach the code... Thank you in advance. Andrea [/QUOTE] Hi Andrea, I have met a similar notification telling that "Failed to find consistent initial values" with PDE equations; Have you solved it ? and could you please give me a hint? Thank you in advance. Best Regards, Bill
Bill
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 8 years ago 16 nov 2016, 05:16 GMT-5


Not if you have an incompressible fluid formulation. A uniform increase in pressure at any time is still a solution even in the time dependent problem.


Well that's embarrassing. I humbly stand corrected, and thank you very much for pointing this out. The reason I got away with the setup earlier was the use of a Krylov solver, but indeed the systems were always singular. Mystery solved. Thanks to all who offered to help out!


Dear Gertjan,
I added a pressure point constraint in your model, there is no error occuring, but without any solutions.
Any suggestions would be appreciated.
Thank you in advance.
Best Regards,
Bill
[QUOTE] [QUOTE] Not if you have an incompressible fluid formulation. A uniform increase in pressure at any time is still a solution even in the time dependent problem. [/QUOTE] Well that's embarrassing. I humbly stand corrected, and thank you very much for pointing this out. The reason I got away with the setup earlier was the use of a Krylov solver, but indeed the systems were always singular. Mystery solved. Thanks to all who offered to help out! [/QUOTE] Dear Gertjan, I added a pressure point constraint in your model, there is no error occuring, but without any solutions. Any suggestions would be appreciated. Thank you in advance. Best Regards, Bill

Note that while COMSOL employees may participate in the discussion forum, COMSOL® software users who are on-subscription should submit their questions via the Support Center for a more comprehensive response from the Technical Support team.

Suggested Content