[weigl]

I am working with T-Rex meshing on a 2D aerofoil. But it seems everything I put in front of my professor, he keeps saying "its not a good mesh"

what I wanted to know is what exactly makes a good unstructured mesh?

edit: when ever i import my mesh into FLUENT it gives me negative volume and back handedness issues

Domain Extents:
x-coordinate: min (m) = -2.900000e+01, max (m) = 3.100000e+01
y-coordinate: min (m) = -3.000000e+01, max (m) = 3.000000e+01
Volume statistics:
WARNING: 18355 cells with non-positive volume detected.
minimum volume (m3): -1.353355e+01
maximum volume (m3): -1.094973e-08
total volume (m3): -3.599919e+03
Face area statistics:
minimum face area (m2): 4.464826e-06
maximum face area (m2): 6.046664e+00
Checking mesh..........
WARNING: left-handed faces detected on zone 3: 0 right-handed, 27263 left-handed.
WARNING: left-handed faces detected on zone 4: 0 right-handed, 38 left-handed.
WARNING: left-handed faces detected on zone 5: 0 right-handed, 198 left-handed.
WARNING: left-handed faces detected on zone 6: 0 right-handed, 99 left-handed.
WARNING: left-handed faces detected on zone 7: 0 right-handed, 204 left-handed..
WARNING: 55065 face(s) on zone 2 with wrong node order (on 1000000)..............
Done.

WARNING: Mesh check failed.

But it shows fine in pointwise

[dgarlisch]

If there are multiple domains in your grid, be sure the domain normals are all are oriented in the same relative direction. By convention, 2D Fluent grids are built in the XY plane with the domain normals pointing in the +Z direction. Use Edit, Orient... to adjust.

As far as "what makes a good grid?" That is the million dollar question! It seems like your professor should give you some "good mesh" criteria to use.

I general you want to the max included cell angles to be < 175. And you want a nice transition from smaller cells to larger cells.

Use the Examine tools menu in Pointwise to evaluate these criteria.

If you post your PW file or an image we can provide more specific help.

Please read this.

[weigl]

Originally Posted by dgarlisch

If there are multiple domains in your grid, be sure the domain normals are all are oriented in the same relative direction. By convention, 2D Fluent grids are built in the XY plane with the domain normals pointing in the +Z direction. Use Edit, Orient... to adjust.

As far as "what makes a good grid?" That is the million dollar question! It seems like your professor should give you some "good mesh" criteria to use.

I general you want to the max included cell angles to be < 175. And you want a nice transition from smaller cells to larger cells.

Use the Examine tools menu in Pointwise to evaluate these criteria.

If you post your PW file or an image we can provide more specific help.

Please read this.

this is what my current mesh looks like: http://www83.zippyshare.com/v/LjauoBu4/file.html

I understand that you have to check the aspect ratios, wall distances and orthogonality etc of the mesh profile. What I dont get is how I know whats best for a certain system. Are there any predefined set of values for a particular condition?

i am trying to validate my results against transonic viscous flow values to see if an unstructured mesh works well on it.

I have been able to validate results with structured mesh, but the whole unstructured mesh I can't seem to get down.

[dgarlisch]

I will have to leave those kinds of details up to more experienced grid builders. However, I did find a few things...

In Grid, T-Rex..., you need to check the Push Attributes box. This will force the T-Rex layers growing off of the wake connector to "push" their spacing onto the Match domains.

The T-Rex Growth Rate is currently set to 2.0. That seems way too high! Normally, we use values around 1.2.

I am not sure if the wall delta-S spacing is correct. It is my understanding that you should use a value based on the target Y+ value. You can use the (free) Pointwise Y+ calculator.

On the T-Rex, Attributes tab, you can also play with the Boundary Decay value (0 to 1.0) to propagate the cell sizes further out from the airfoil. Values closer to 1.0 propagate cells further into the far field.

Finally, you said this was transonic. If I recall my aero properly, that means you may have shock fronts. You probably need to add a baffle connector to the dom in the region of the expected front to properly resolve the shock. To add a baffle, create a connector at the proper location near the airfoil. The connector should not touch the airfoil and its end point should be just outside the trex layer region. Add the connector to the domain using Edit, Add/Remove Edges... menu.

I have attached a picture of my result.

[weigl]

Originally Posted by dgarlisch

I will have to leave those kinds of details up to more experienced grid builders. However, I did find a few things...

In Grid, T-Rex..., you need to check the Push Attributes box. This will force the T-Rex layers growing off of the wake connector to "push" their spacing onto the Match domains.

The T-Rex Growth Rate is currently set to 2.0. That seems way too high! Normally, we use values around 1.2.

I am not sure if the wall delta-S spacing is correct. It is my understanding that you should use a value based on the target Y+ value. You can use the (free) Pointwise Y+ calculator.

On the T-Rex, Attributes tab, you can also play with the Boundary Decay value (0 to 1.0) to propagate the cell sizes further out from the airfoil. Values closer to 1.0 propagate cells further into the far field.

Finally, you said this was transonic. If I recall my aero properly, that means you may have shock fronts. You probably need to add a baffle connector to the dom in the region of the expected front to properly resolve the shock. To add a baffle, create a connector at the proper location near the airfoil. The connector should not touch the airfoil and its end point should be just outside the trex layer region. Add the connector to the domain using Edit, Add/Remove Edges... menu.

I have attached a picture of my result.

Thank you for your reply.

The mesh is looking better.

As for orientation, when i try to orient it i get something like the picture i have attached below. why is that one arrow not pointing in the positive z?

[RcktMan77]

Is there a particular reason you're using an unstructured mesh for such a simple geometry? Pointwise has a hyperbolic extrusion feature which would create a boundary conforming mesh very easily which should provide some benefits to the accuracy of your solution since the cell edges are flow-aligned. I've created an example for you using your NACA0012 geometry which you can download using this link. The initial spacing was set to that which you were using, and it is oriented appropriately for use with FLUENT.

To learn more about using hyperbolic extrusions in Pointwise for your specific example, see this video.

[weigl]

Originally Posted by RcktMan77

Is there a particular reason you're using an unstructured mesh for such a simple geometry? Pointwise has a hyperbolic extrusion feature which would create a boundary conforming mesh very easily which should provide some benefits to the accuracy of your solution since the cell edges are flow-aligned. I've created an example for you using your NACA0012 geometry which you can download using this link. The initial spacing was set to that which you were using, and it is oriented appropriately for use with FLUENT.

To learn more about using hyperbolic extrusions in Pointwise for your specific example, see this video.

Because my professor wants me to use an unstructured mesh for my thesis. he's not really very keen on a structured mesh. he wants to add transonic viscous effects which he believes a structured mesh will do no justice to

[dgarlisch]

Originally Posted by weigl

Thank you for your reply.

The mesh is looking better.

As for orientation, when i try to orient it i get something like the picture i have attached below. why is that one arrow not pointing in the positive z?

I loaded up the original mesh you posted above. All the arrows were pointing in the same direction. I am using Pointwise V17.3R4. Which version are you using?

Could you upload the grid file that is doing this? If you zip the PW file, and it is less than 195.3KB, you can attach it to this forum directly.

[weigl]

Originally Posted by dgarlisch

I loaded up the original mesh you posted above. All the arrows were pointing in the same direction. I am using Pointwise V17.3R4. Which version are you using?

Could you upload the grid file that is doing this? If you zip the PW file, and it is less than 195.3KB, you can attach it to this forum directly.

here is the .pw file: http://www65.zippyshare.com/v/uw1pAAk1/file.html

i have set the orientation back to normal. but when i orient the domain it shows the way it did in the image. I am using 17.2R1

[dgarlisch]

That appears to be a bug! I will log it with our support team.

It appears this bug is already fixed in the next release of Pointwise V17.3R5. It will be available in a week or two.

As a workaround:

1. Change the orientation as you want it.
2. Accept the messed up domain.
3. Initialize the domain to rebuild the grid in the new orientation.

Also, if your professor will allow it, I strongly suggest that you update your Pointwise installation. There have been many bug fixes and enhancements since V17.2R1!

[weigl]

Originally Posted by dgarlisch

That appears to be a bug! I will log it with our support team.

It appears this bug is already fixed in the next release of Pointwise V17.3R5. It will be available in a week or two.

As a workaround:

1. Change the orientation as you want it.
2. Accept the messed up domain.
3. Initialize the domain to rebuild the grid in the new orientation.

Also, if your professor will allow it, I strongly suggest that you update your Pointwise installation. There have been many bug fixes and enhancements since V17.2R1!

Ah ok. I was breaking my head over it. I guess i will use fluent to fix my problems until then. I will ask the university if they can upgrade it.

[adi.ptb]

Hi,
I have a simple question about TRex. I understand that TRex is anisotropic tetrahedral extrusion. I want to know how the progression is handled from one layer to the next one and how to calculate the total height of the layers. Is there any mathematical expression based one the initial height, number of layers and the growth rate to calculate the total height?

Thanks in advance,

[RcktMan77]

The extrusion advances geometrically. You provide an initial cell height and a growth rate. The cell height for each successive layer is multiplied by this growth rate. The geometric series looks like:

initDs * growthRate^(layerNum - 1)

[adi.ptb]

Thanks zack. This is exactly what I needed to hear. I suspected that the progression might be geometrical but I wasn't sure. Thank you so much for making it clear to me.

[adi.ptb]

Hi Zack,


Thanks