[RuiVO]

Greetings,

How to change length scale of Pointwise from meters to millimeters?

I ask this because I have one T106 geometry in pointwise but its designed in meters. When I load this mesh in Fluent I can change the length scale easily. But when I run in OpenFoam the same is not so easy since OF is predefined to run in meters and my solutions aren't exactly the same since one of the blades has a 86 millimeters for axial chord and the other one in OpenFoam has 86 meters. The pressure distribution is similar but the total values of pressure are completely different. I guess with the correct adimensionalization I could get similar results, but I prefer to obtain actual similar results of the same order of magnitude.

Best regards

Rui

[jchawner]

Hi Rui:

Pointwise is dimensionless so you don't change units.

But to scale the mesh you just select everything and use Edit, Transform, Scale by the appropriate factors.

Hope this helps.

[RuiVO]

Hi jchawner,

Thank you for your answer. The was exactly what I did !

Best regards

Rui

[YNM_07]

Hi Guys,

I understand that pointwise works with a dimensionless length unit and you can scale the it down to achieve the appropriate sizing for export into your chosen solver. However, my issue is I have a geometry that includes a feature that is extremely small in relation to the largest dimension (1/1000th). When I scale by the appropriate factors I lose some accuracy in the feature, which happens to be a hemispherical protrusion, and it truncates the mentioned geometry.

Any suggestions on how to approach this? I will be importing the mesh into Fluent and although I see you can change the length scale in fluent, I would prefer to keep it in meters in order to avoid any possible errors throughout the analysis.

Any help would be much appreciated if you guys have any ideas!

Thanks in advance!

YNM_07

[Far]

I guess best option would to scale the mesh in Fluent (always).

[YNM_07]

Perfect, sorry that must have seemed like a silly question! I was unaware you could do that in Fluent, will give it a go.

Thanks again for your help!

Yannick

[rmatus]

Yannick:

Scaling the geometry in Pointwse should not truncate any parts. Are you sure the geometry is actually truncated and it is not a display artifact? You can check that by making sure Pointwise is set to use double-precision graphics. In Pointwise, go to Edit, Preferences and make sure Double Precision Graphics is checked on in the Graphics pane.

Could you post before and after images so I can see what is happening?

Thanks,
Rick

[YNM_07]

Yeah it could actually be a graphics problem. I initially thought it may be but didn't want to take any chances. I will give that a go sometime today a let you know how that goes. I can post some images as well.

Thanks for the response guys, really appreciate the help.

YNM_07

[tcarrigan]

Originally Posted by RuiVO

But when I run in OpenFoam the same is not so easy since OF is predefined to run in meters and my solutions aren't exactly the same since one of the blades has a 86 millimeters for axial chord and the other one in OpenFoam has 86 meters.

You can scale the grid in OpenFOAM by transforming the points. For example, to go from mm to m you would use the following command:

transformPoints -scale '(0.001 0.001 0.001)'

[jitendraseregar@gmail.com]

Originally Posted by jchawner

Hi Rui:

Pointwise is dimensionless so you don't change units.

But to scale the mesh you just select everything and use Edit, Transform, Scale by the appropriate factors.

Hope this helps.

If I have to change length scale in say meters so how much or what scaling factor should be used? any help would be much appreciated

[adi.ptb]

Hi,
according to above comments PointWise in dimensionless so all the length scales should be consistent right? For example if the geometry was created in mm and we import the geometry into PointWise and then lets say we use a value of 0.5 for the connector dimension. The 0.5 value that we specify is considered as mm in PointWise?

Thanks

[jchawner]

Yes, 0.5 would be 0.5 mm.

[adi.ptb]

Thank you so much for your reply john. I have another question about TRex that i hope you can help me with. 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 so much,

[jchawner]

You specify the initial spacing and a growth rate (for example, 1.2 = grows by 20%) of that spacing for each successive extrusion step. Extrusion continues until the cells become roughly isotropic for a smooth transition to the outer tet mesh.

Total layer height can be controlled to a certain degree but keep in mind that T-Rex stops extruding locally based on many criteria including cell quality and proximity to other extruding layers. Therefore, the height of the extruded region will vary across the geometry.

[adi.ptb]

Thanks john. I have specified some values for the TRex like collision buffer= 2, max angle = 160 degree, boundary decay =0.85, growth rate =1.27 and 20 layers. What you are saying is completely correct but I want an rough value for the overall height. so that I can roughly make that overall height to match my boundary layer thickness. How can I do that in PointWise? Should I measure the distance between two points to get that? and if that is true should I do it before export to the solver or after export? and how can I measure the distance between two points?

Thanks so much,

[jchawner]

I suppose you can set Max Layers, the maximum number of layers it will attempt to extrude. Then knowing the initial wall spacing and the growth rate you could compute the layer height where the max. number of layers is achieved.

On Windows, you can measure the distance between any two points using Alt + right mouse button. There are other key bindings for Linux and Mac that are in the User Manual.

[adi.ptb]

Hi john,

Is it correct that the extrusion progression is geometrical?

[jchawner]

I believe so, yes.

[RcktMan77]

Originally Posted by adi.ptb

Thanks john. I have specified some values for the TRex like collision buffer= 2, max angle = 160 degree, boundary decay =0.85, growth rate =1.27 and 20 layers. What you are saying is completely correct but I want an rough value for the overall height. so that I can roughly make that overall height to match my boundary layer thickness. How can I do that in PointWise? Should I measure the distance between two points to get that? and if that is true should I do it before export to the solver or after export? and how can I measure the distance between two points?

Thanks so much,

Adi,

You shouldn't artificially limit the number of layers that you grow using T-Rex. You want the extrusion to continue until the last cell height reaches an isotropy condition, so that the cell volumes between the last layer of anisotropic tetrahedra and the isotropic tetrahedra that fill in the interior are roughly the same. Otherwise you will have a large jump in cell volumes between the boundary layer resolved grid and the interior which most solvers find undesirable. Specify an arbitrarily large number for Max Layers. The extrusion should automatically stop upon reaching isotropy, and you should have a smooth transition in cell volumes between T-Rex cells and iso-tets.

Also specifying a Max Angle stop criteria of 160 degrees is pretty strict. You are likely going to get a better volume grid by relaxing this somewhat. Try 165 or 170 degrees instead.

Best Regards,



Zach

[ndtrong]

Originally Posted by tcarrigan

You can scale the grid in OpenFOAM by transforming the points. For example, to go from mm to m you would use the following command:

transformPoints -scale '(0.001 0.001 0.001)'

Thank you so much for your suggestion.