[jpesich]

Hello,

This is more of a numerical methods question and how to visualize it in STAR-CCM. My residuals have a tough time converging below 3 orders of magnitude. I have concluded it's the mesh that is holding up convergence.

Is there a way to visualize which cell has the largest residual and is holding up convergence for the whole solution?

Thanks!

[fluid23]

Indeed! There is an easy way and a hard way.

If you have access to the Steve-Portal, the easy way is obviously best. Log on and go to the macro hut and look for mesh quality analyzer (I think is the name). Install it and read the instructions. It will automatically analyze your mesh and results for mesh quiailty issues and high residuals then create scenes to help you visualize.

If not the hard way is, well... harder. Depending on what solver and turbulence models you are using you will see a number of items listed under Solvers in the model tree. One will say 'Coupled Implicit', 'Segregated Implicit', 'Coupled Explicit' or something like that. This is your main solver. If you highlight that in the tree, you will see an option in the propeties window that says temporary storage retained. Turn that on. Do the same thing in your turbulence solver and run 1 iteration.

Now if you go into your field functions you will notice that you now have options for all the residuals that appear on your residual plot. You can create thresholds for these to target the top 5% or 10% of each value by hitting query and then adjusting the max/min values. Then you simply need to create a scalar scene that has these thresholds. I always add a geometry displayer too to help me visualize where I am in the domain. Make sure to turn temp storage off before you run again.

A note on convergence. I too have struggled getting nice and pretty convergence plots on occasion. I have spoken with tech support about it and they told me that it can be a product of any number of things. As long as they don't go totally crazy (like gain an order of magnitude or more), your other values of interest converge (mass flow, force, whatever is important to you) converge and your high residual cells aren't near your areas of interest you should be fine.

I most commonly see this problem when I do hover analysis for rotorcraft. My continuity and energy residuals usualy don't drop more than 2 OoM's. However, the results are reliable and have been confirmed through flight testing.

[jpesich]

Thanks so much. This is awesome information!

[Catostrof]

Originally Posted by MBdonCFD

Indeed! There is an easy way and a hard way.

If you have access to the Steve-Portal, the easy way is obviously best. Log on and go to the macro hut and look for mesh quality analyzer (I think is the name). Install it and read the instructions. It will automatically analyze your mesh and results for mesh quiailty issues and high residuals then create scenes to help you visualize.

If not the hard way is, well... harder. Depending on what solver and turbulence models you are using you will see a number of items listed under Solvers in the model tree. One will say 'Coupled Implicit', 'Segregated Implicit', 'Coupled Explicit' or something like that. This is your main solver. If you highlight that in the tree, you will see an option in the propeties window that says temporary storage retained. Turn that on. Do the same thing in your turbulence solver and run 1 iteration.

Now if you go into your field functions you will notice that you now have options for all the residuals that appear on your residual plot. You can create thresholds for these to target the top 5% or 10% of each value by hitting query and then adjusting the max/min values. Then you simply need to create a scalar scene that has these thresholds. I always add a geometry displayer too to help me visualize where I am in the domain. Make sure to turn temp storage off before you run again.

A note on convergence. I too have struggled getting nice and pretty convergence plots on occasion. I have spoken with tech support about it and they told me that it can be a product of any number of things. As long as they don't go totally crazy (like gain an order of magnitude or more), your other values of interest converge (mass flow, force, whatever is important to you) converge and your high residual cells aren't near your areas of interest you should be fine.

I most commonly see this problem when I do hover analysis for rotorcraft. My continuity and energy residuals usualy don't drop more than 2 OoM's. However, the results are reliable and have been confirmed through flight testing.

This spares you so much time! Wish I found out about java macros earlier in the process, would have helped me a lot. Fantastic tool for increasing the working pace

[marmot]

Nice information above not sure what is all in the macro but just in case here is more info

I usually add the physical model, Cell Quality Remediation (this will smooth gradients for bad cells)

You can also visualize the bad cells, you have a field function called Cell Quality, I think 0 is bad, 1 is good. So if you make a plane section you can plot that or use a threshold to give everythign between 0-.01.

Also if you right click on region, remove invalid cells (you can also add the cell quality option to remove bad cells below a threshold)

Although after removing bad cells you should always check to make sure no islands of cells were created by, right click on region, Split non-contiguous, make sure on 1 region