2D Dynamic mesh simulation of a scroll expander

ghorrocks · July 17, 2018, 03:26

You should do a sensitivity study to determine what residuals convergence your model requires. Try a range of tolerances and see what you require for the accuracy you are looking for.

Regarding residuals flatlining: see FAQ https://www.cfd-online.com/Wiki/Ansy...gence_criteria

Gert-Jan · July 17, 2018, 03:33

You should define these monitoring points in Pre. Go to Output Control/Monitoring points. Define several points in your geo by clicking on the screen and monitor pressure, velocity, tke, etc. When these show flat liners in your solver manager, your convergence is ok.
Don't focus too much on residuals. Imbalance of zero and flat monitoring points are much more important for deep convergence. For example, it could be that your residuals need to go to 1e-6 or 1e-7 before monitoring points become flat.

louisdub11 · July 17, 2018, 04:42

Thank you both for the answers.

When creating monitor points, I'm not able to have the axis as "1.0e-6"...

user points.PNG

Is there something I'm missing?

I set all the monitors to "full".

Capture.PNG

ghorrocks · July 17, 2018, 22:03

Your monitor point is showing pressure and velocity, not the residuals of the mass and momentum equations. They are different variables.

Gert-Jan · July 18, 2018, 01:38

Quote:

Originally Posted by louisdub11

Thank you both for the answers.

When creating monitor points, I'm not able to have the axis as "1.0e-6"...

Attachment 64596

Is there something I'm missing?

I set all the monitors to "full".

Attachment 64597

If you don't understand what the numbers in these plots represent, you should not run CFD-simulations at all.

Regs, Gert-Jan

Btw, I am Dutch. So, from an international point of view, I am quite direct. In other words, I am too honest to be polite.

louisdub11 · July 18, 2018, 02:22

Quote:

Originally Posted by ghorrocks

Your monitor point is showing pressure and velocity, not the residuals of the mass and momentum equations. They are different variables.

Ok, Thanks. I thought I should have residuals convergence for them as well

louisdub11 · July 18, 2018, 02:33

Quote:

Originally Posted by Gert-Jan

If you don't understand what the numbers in these plots represent, you should not run CFD-simulations at all.

Regs, Gert-Jan

Btw, I am Dutch. So, from an international point of view, I am quite direct. In other words, I am too honest to be polite.

I do understand them. I was just expecting residual values to see the convergence as in the mass and momentum equations.

I appreciate the help you provided me with, but if you don't want to teach me from your experience, then just say nothing. Being direct doesn't mean being rude

I am studying industrial engineering, and haven't had any CFD or FEM lessons at all (and very basic fluid mechanics 4 years ago). I chose to tackle a CFD problem for my master thesis, so I am sorry if in the urge of finishing it on time, I may ask sometimes silly questions

If for you everything seems to be obvious and you are the best, just stay humble

Thanks.

louisdub11 · July 19, 2018, 06:25

Now I have tried a simulation of 1h52, giving these results. I have flat lines on the monitor points, however I don't get flat lines on the residuals and turbulence plots.

Do I absolutely need to have flat lines everywhere or not?

Another question, when I put the reference pressure at 0 Pa in CFX Pre, I get the same results as when I put the reference pressure at 1 atm.

Maybe I don't put the reference at the right place? What could be the explanation?

Thanks

mass.PNG

tke.PNG

user.PNG

plot.PNG

ghorrocks · July 19, 2018, 07:02

Let me explain your charts a bit:

Momentum and Mass residuals: This is an estimate of the errors of the simulation. Smaller indicates tighter convergence. You have converged to 1e-10, convergence to this level of accuracy is rarely required. 1e-4 is usually coarse convergence, 1e-5 is normal, 1e-6 is tight. Also, when the residuals converge monotonically like this it is a sign the time step size can be increased. It will then converge faster in less iterations. You do 3500 iterations - CFX usually converges a simple steady state run in about 100 iterations. I think you can speed your run up a lot with a bigger time step.

Turbulence residuals: This shows the residual error on the turbulence equations. It is usual for convergence on these equations to not be as tight as mass and momentum. As the turbulence variables are usually not of primary importance (mass and momentum are the key ones) we usually accept a lower level of convergence for turbulence.

Monitor Points: You show a range of variables. They converge to a value and by about 1300 iterations there is no visible change to the values. Obviously if you examined the numbers in detail it is likely they are still converging. I recommend you look at this convergence and decide a level of accuracy you are happy to work with. This will then tell you the residuals tolerance you need to achieve that accuracy. Then future simulations can use that as a convergence tolerance and your simulations will be faster, and with a known level of error due to convergence.

Imbalances: This is second method of assessing convergence. It does it by summing all the variable fluxes and checking they balance. For some classes of simulations this is a better way of assessing convergence than residuals (eg CHT simulation). But for most simulations residuals are a better method of assessing convergence. Again, you can use these like the residuals to define a level of accuracy you are happy to have, and then using that as a convergence criteria for future simulations.

louisdub11 · July 19, 2018, 08:11

Quote:

Originally Posted by ghorrocks

Let me explain your charts a bit:

Momentum and Mass residuals: This is an estimate of the errors of the simulation. Smaller indicates tighter convergence. You have converged to 1e-10, convergence to this level of accuracy is rarely required. 1e-4 is usually coarse convergence, 1e-5 is normal, 1e-6 is tight. Also, when the residuals converge monotonically like this it is a sign the time step size can be increased. It will then converge faster in less iterations. You do 3500 iterations - CFX usually converges a simple steady state run in about 100 iterations. I think you can speed your run up a lot with a bigger time step.

Turbulence residuals: This shows the residual error on the turbulence equations. It is usual for convergence on these equations to not be as tight as mass and momentum. As the turbulence variables are usually not of primary importance (mass and momentum are the key ones) we usually accept a lower level of convergence for turbulence.

Monitor Points: You show a range of variables. They converge to a value and by about 1300 iterations there is no visible change to the values. Obviously if you examined the numbers in detail it is likely they are still converging. I recommend you look at this convergence and decide a level of accuracy you are happy to work with. This will then tell you the residuals tolerance you need to achieve that accuracy. Then future simulations can use that as a convergence tolerance and your simulations will be faster, and with a known level of error due to convergence.

Imbalances: This is second method of assessing convergence. It does it by summing all the variable fluxes and checking they balance. For some classes of simulations this is a better way of assessing convergence than residuals (eg CHT simulation). But for most simulations residuals are a better method of assessing convergence. Again, you can use these like the residuals to define a level of accuracy you are happy to have, and then using that as a convergence criteria for future simulations.

Thanks for the very clear explanations

I did a 150 time steps simulations with time steps of 0.5s.

This is the results I got, and it seems much better

mass.PNG

tke.PNG

user.PNG

plot.PNG

What about the pressure reference problem?

Edit: To be more accurate about the pressure, I have set the reference pressure at 0 Pa in the "domain models" in CFX Pre. When doing the post processing, I get a maximum of about 0.6 Pa and a minimum value of about -93 Pa. How can this radial pressure be negative compared to the reference of 0 Pa ?

photo.png

I checked the velocity analytically and it corresponds with the CFD result I have.

Thanks a lot !

ghorrocks · July 19, 2018, 18:26

You should set the reference pressure to a typical pressure in your model. This means the solver is using a pressure variable which should be close to zero. This minimises round-off error and makes convergence more reliable. This does not affect all simulations, but for complex and numerically unstable simulations it is essential. If it makes no difference in your case then your model is numerically stable - but you should set the reference pressure correctly anyway as it is good practice.

Negative absolute pressure: An incompressible flow has no mathematical lower limit to the pressure. It can go to a negative absolute pressure just fine. If this is not real and effects like cavitation then take place you need to include a cavitation model to account for this effect.

louisdub11 · July 23, 2018, 13:26

Hi, thanks Glenn for the previous answer

I am now trying to do the simulation of a journal bearing. In my case, I have a fixed eccentricity. I have tried with water and with oil and different rotational speeds, and it seems to always give me the same kind of result:

test1 k e_011.png

In the literature, I found several results describing the pressure distribution on the journal, like this:

gtp_137_08_082507_f002.png

Do you have an idea of what could be the problem (if there is any)?

ghorrocks · July 23, 2018, 18:13

I see many issues:

* I can see your results are quite blocky. This is clear sign your mesh is too coarse. You should do a mesh refinement study to determine a suitable mesh. While you are at it, do a time step (if transient) and convergence criteria study as well.

* One of those images you show is in the 3rd dimension. You appear to be doing a 2D simulation, so of course you won't get the pressure distribution in the 3rd dimension until you model it.

* Journal bearings have a much thinner fluid thickness than what you have modelled. Also the effect needs a minimum speed before those effects are visible. Are you sure you have a journal bearing of the correct design and are operating it at the correct speed?

louisdub11 · July 24, 2018, 07:54

Quote:

Originally Posted by ghorrocks

I see many issues:

* I can see your results are quite blocky. This is clear sign your mesh is too coarse. You should do a mesh refinement study to determine a suitable mesh. While you are at it, do a time step (if transient) and convergence criteria study as well.

My mesh is quite fine, it is a problem of number of contours in CFD Post, I increased the number of contours and it gives me that result:

Capture.PNG

For the time steps and convergence, I did it as well and it seems that I have found a satisfactory result, considering all your previous explanations

* One of those images you show is in the 3rd dimension. You appear to be doing a 2D simulation, so of course you won't get the pressure distribution in the 3rd dimension until you model it.

Won't I be able to have the pressure distribution on the left image? Isn't it sufficient with the "2.5D mesh" in CFX?

* Journal bearings have a much thinner fluid thickness than what you have modelled. Also the effect needs a minimum speed before those effects are visible. Are you sure you have a journal bearing of the correct design and are operating it at the correct speed?

I will increase the eccentricity to have a thinner fluid thickness. At this time I have set a rotational speed of the shaft at 2000rpm, is it enough in your opinion?

Also, how can it be high pressure at the top and low pressure in the small gap? Would it be useful to add gravity effect on it?

Thanks a lot

EDIT: I have done everything from the start with a much thinner fluid film. I have added gravity effect, and instead of a simple smooth wall, I set the shaft as a rough wall. I have this result:

PROJET45_002.png

Does it seem better for you?

ghorrocks · July 24, 2018, 18:45

Why have you added gravity? Unless your fluid has a density difference gravity does nothing.

By thinner film I meant thinner film all around. I recommend you read journal bearing design textbooks so you can find what are typical design parameters for journal bearings. If you just guess shapes you are bound to not be realistic.

0xyqen · November 15, 2021, 12:28

Quote:

Originally Posted by louisdub11

Hello again,

As I couldn't have access to the customer portal for dynamic meshes, my objectives have changed: I need now to do the simulation of a journal bearing.

My first question is: when doing the mesh, should I generate a mesh for all the different parts, or should I generate a mesh only for the fluid region?

Thanks

I did the 2d modeling.
I am trying to do 3D modeling.
It gives negative volume error in 3D modeling, when I used mesh setting of 2d.

https://www.youtube.com/watch?v=ixoEB4-d5O8

ghorrocks · November 15, 2021, 16:54

FAQ: https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F

July 17, 2018, 03:26		#81
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,705 Rep Power: 143	You should do a sensitivity study to determine what residuals convergence your model requires. Try a range of tolerances and see what you require for the accuracy you are looking for. Regarding residuals flatlining: see FAQ https://www.cfd-online.com/Wiki/Ansy...gence_criteria __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

July 17, 2018, 22:03		#84
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,705 Rep Power: 143	Your monitor point is showing pressure and velocity, not the residuals of the mass and momentum equations. They are different variables. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

July 19, 2018, 07:02		#89
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,705 Rep Power: 143	Let me explain your charts a bit: Momentum and Mass residuals: This is an estimate of the errors of the simulation. Smaller indicates tighter convergence. You have converged to 1e-10, convergence to this level of accuracy is rarely required. 1e-4 is usually coarse convergence, 1e-5 is normal, 1e-6 is tight. Also, when the residuals converge monotonically like this it is a sign the time step size can be increased. It will then converge faster in less iterations. You do 3500 iterations - CFX usually converges a simple steady state run in about 100 iterations. I think you can speed your run up a lot with a bigger time step. Turbulence residuals: This shows the residual error on the turbulence equations. It is usual for convergence on these equations to not be as tight as mass and momentum. As the turbulence variables are usually not of primary importance (mass and momentum are the key ones) we usually accept a lower level of convergence for turbulence. Monitor Points: You show a range of variables. They converge to a value and by about 1300 iterations there is no visible change to the values. Obviously if you examined the numbers in detail it is likely they are still converging. I recommend you look at this convergence and decide a level of accuracy you are happy to work with. This will then tell you the residuals tolerance you need to achieve that accuracy. Then future simulations can use that as a convergence tolerance and your simulations will be faster, and with a known level of error due to convergence. Imbalances: This is second method of assessing convergence. It does it by summing all the variable fluxes and checking they balance. For some classes of simulations this is a better way of assessing convergence than residuals (eg CHT simulation). But for most simulations residuals are a better method of assessing convergence. Again, you can use these like the residuals to define a level of accuracy you are happy to have, and then using that as a convergence criteria for future simulations. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

July 19, 2018, 18:26		#91
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,705 Rep Power: 143	You should set the reference pressure to a typical pressure in your model. This means the solver is using a pressure variable which should be close to zero. This minimises round-off error and makes convergence more reliable. This does not affect all simulations, but for complex and numerically unstable simulations it is essential. If it makes no difference in your case then your model is numerically stable - but you should set the reference pressure correctly anyway as it is good practice. Negative absolute pressure: An incompressible flow has no mathematical lower limit to the pressure. It can go to a negative absolute pressure just fine. If this is not real and effects like cavitation then take place you need to include a cavitation model to account for this effect. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

July 23, 2018, 18:13		#93
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,705 Rep Power: 143	I see many issues: * I can see your results are quite blocky. This is clear sign your mesh is too coarse. You should do a mesh refinement study to determine a suitable mesh. While you are at it, do a time step (if transient) and convergence criteria study as well. * One of those images you show is in the 3rd dimension. You appear to be doing a 2D simulation, so of course you won't get the pressure distribution in the 3rd dimension until you model it. * Journal bearings have a much thinner fluid thickness than what you have modelled. Also the effect needs a minimum speed before those effects are visible. Are you sure you have a journal bearing of the correct design and are operating it at the correct speed? __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

July 17, 2018, 03:33		#82
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,827 Rep Power: 27	You should define these monitoring points in Pre. Go to Output Control/Monitoring points. Define several points in your geo by clicking on the screen and monitor pressure, velocity, tke, etc. When these show flat liners in your solver manager, your convergence is ok. Don't focus too much on residuals. Imbalance of zero and flat monitoring points are much more important for deep convergence. For example, it could be that your residuals need to go to 1e-6 or 1e-7 before monitoring points become flat.

July 17, 2018, 04:42		#83
louisdub11 Member Louis Dubail Join Date: May 2018 Location: Brussels, Belgium Posts: 52 Rep Power: 7	Thank you both for the answers. When creating monitor points, I'm not able to have the axis as "1.0e-6"... user points.PNG Is there something I'm missing? I set all the monitors to "full". Capture.PNG

July 19, 2018, 06:25		#88
louisdub11 Member Louis Dubail Join Date: May 2018 Location: Brussels, Belgium Posts: 52 Rep Power: 7	Now I have tried a simulation of 1h52, giving these results. I have flat lines on the monitor points, however I don't get flat lines on the residuals and turbulence plots. Do I absolutely need to have flat lines everywhere or not? Another question, when I put the reference pressure at 0 Pa in CFX Pre, I get the same results as when I put the reference pressure at 1 atm. Maybe I don't put the reference at the right place? What could be the explanation? Thanks mass.PNG tke.PNG user.PNG plot.PNG

July 23, 2018, 13:26		#92
louisdub11 Member Louis Dubail Join Date: May 2018 Location: Brussels, Belgium Posts: 52 Rep Power: 7	Hi, thanks Glenn for the previous answer I am now trying to do the simulation of a journal bearing. In my case, I have a fixed eccentricity. I have tried with water and with oil and different rotational speeds, and it seems to always give me the same kind of result: test1 k e_011.png In the literature, I found several results describing the pressure distribution on the journal, like this: gtp_137_08_082507_f002.png Do you have an idea of what could be the problem (if there is any)?

July 24, 2018, 18:45		#95
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,705 Rep Power: 143	Why have you added gravity? Unless your fluid has a density difference gravity does nothing. By thinner film I meant thinner film all around. I recommend you read journal bearing design textbooks so you can find what are typical design parameters for journal bearings. If you just guess shapes you are bound to not be realistic. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

November 15, 2021, 16:54		#97
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,705 Rep Power: 143	FAQ: https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
decomposePar problem: Cell 0contains face labels out of range	vaina74	OpenFOAM Pre-Processing	37	July 20, 2020 05:38
[mesh manipulation] Importing Multiple Meshes	thomasnwalshiii	OpenFOAM Meshing & Mesh Conversion	18	December 19, 2015 18:57
radial turbine blade simulation with dynamic mesh 6dof(fluent)	mamyjooooon	FLUENT	0	April 7, 2011 14:28
[snappyHexMesh] snappyHexMesh won't work - zeros everywhere!	sc298	OpenFOAM Meshing & Mesh Conversion	2	March 27, 2011 21:11
Icemcfd 11: Loss of mesh from surface mesh option?	Joe	CFX	2	March 26, 2007 18:10