Scaling down of Geometry

AS_Aero · April 5, 2018, 05:03

Hi All

I am trying to do a Vertical axis wind turbine simulation and my entire geometry is of 2m length/height and if I want to simulate that, its going to be a huge simulation although I want to see the effects around the wind turbine and within the turbine as well. And another important thing I want to study is the wind turbine power for a particular RPM and wind velocity.

So now my question is can I scale up my entire geometry by 2cm or 20cm and study the effects ? This will be more easy for me to do the computation but my doubt is will it affect the results or can I do the scaling for the results also ?

Second thing is doing a 2D simulation or taking a small portion of the geometry and do the computation ?

Which method is better ?

Gert-Jan · April 5, 2018, 05:41

In my opinion the strong point of CFD is that you don't have to scale up or down. So from a CFD point of view I think it is a rather strange approach.

Certainly you can do that, and then scale the power using affinity rules. Either for upscaling and downscaling. But I think you cannot save a lot of elements on small scale. Geometry details will remain the same, not?

Alternatively buy HPC packs, a facter and larger computer........

ghorrocks · April 5, 2018, 06:34

I agree with Gert-Jan. Don't scale, simulate it real size.

As you probably know, when you scale you keep the important non-dimensional numbers (like Reynolds Number, Rayliegh Number etc) the same by changing the geometry and using some other factor, maybe fluid speed or material properties; such that the non-dimensional numbers are unchanged. But for any model of reasonable complexity you will find several non-dimensional numbers are important and it is not possible to keep them all the same. So you have to choose which one you keep the same and which one you vary. In other words, scaling introduces a source of error as some non dimensional numbers must be changed.

2D simulation: See the FAQ: https://www.cfd-online.com/Wiki/Ansy..._simulation.3F If your flow can be modelled as 2d then you should model it 2d as it will make modelling far easier. But be aware that just because the geometry is 2d does not mean the flow is 2d.

AS_Aero · April 5, 2018, 07:16

Dear Glenn and Gert

Thanks a lot for your valuable answers. The thing why I thought of scaling is since I want to simulate the effect of the wind turbine by placing it on a tall building which is again 3m tall and then the far field also I need to extend so on the whole my air domain will be around 10m length and 5m tall so its really a huge domain atleast for meshing and i might need that many cores to use for one computation. So if I convert all this meter by cm 10cm*5cm then the amount of mesh required will be drastically reduced and still i can study the effects.

Second thing regarding the 2D simulation, I have more than 5 blades and hence to study the blade interaction and the interaction of the turbine itself with the case and structures I am not sure if 2D will help, but if I want to see how the Power produced by the turbine and the Cp values wornt this 2D be enough ? And this was also suggested by the Ansys customer support. But I dint understand by '' flow can be modeled as 2D '' and I have an inlet face , so in 2D it will be a line.

Then I also have a doubt about the interface region ! In 3D I will have interface along the length of the turbine blade and on both sides of the turbine, but in 2D I will have only one interface which is around the blades, and in CFX we cant do 2D but a single cell thickness. so should I still give interface on both sides or it doesnt matter ?

AtoHM · April 5, 2018, 07:39

I dont know why you think "the amount of mesh" will be reduced by scaling? Assume you have a mesh cell of 1m³ at the boundary of your domain and a cell close to the blade with, IDK, 0.005 m³. If you scale everything, the total number of elements will be the same, only your absolute element size will be reduced. The number of cells will only reduce if you scale different regions differently, leading to a coarser mesh.

ghorrocks · April 5, 2018, 07:42

For the 2D question: Please post an image of what you are modelling so we can understand your geometry. For the scaling question refer to Michael's answer

Gert-Jan · April 5, 2018, 07:57

Quote:

Originally Posted by AtoHM

I dont know why you think "the amount of mesh" will be reduced by scaling? Assume you have a mesh cell of 1m³ at the boundary of your domain and a cell close to the blade with, IDK, 0.005 m³. If you scale everything, the total number of elements will be the same, only your absolute element size will be reduced. The number of cells will only reduce if you scale different regions differently, leading to a coarser mesh.

I think he wants to scale the geometry first and then remesh. ;-)
But as I already mentioned, the geometric details will remain the same. So the elements savings will be limited, other then some larger elements far away.

AS_Aero · April 5, 2018, 08:20

Yes it makes sense, even if I scale the entire geometry it might not really help me. Sorry it was my stupid thought that I will get reduced cells. But its not.

AS_Aero · April 10, 2018, 05:16

Sorry for the late reply . .. The CAD is almost similar to the video link in the Youtube :
https://www.youtube.com/watch?v=DUl74SGWC48

Here this guy is creating an interface on both sides of the rotor disc where the blades are attached, but the customer service technical support said we dont need that ! Can someone tell me if its necessary or not ! And my geometry is around 2m length and it also has some casing around the turbines which i consider as a part of stationary parts.

Gert-Jan · April 10, 2018, 06:31

The windmill in the movie requires 3 interfaces.
If your geometry requires 2 or 3 is impossible to say since we don't know your geometry. As a first guess I would say you need three as well. That would sound most logical. Only if your bottom disc is on the same height as a surrounding wall (where the windmill is standing on), then you don't need to have it.

Or does the support mean you can group the top and the bottom side into a single interface. Then in Pre you only have to define 2 interfaces. But in the run, you will still have three interface surfaces. That would not make any difference.

AS_Aero · April 10, 2018, 07:08

Mine is completly same just that there is a casing outside the windmill, and the length is much more. That means I have these discs as support for blade every 500cm. So my entire geometry is 2m length so 4 times like this. And have disc on both ends also.
But the ansys support told me you dont need any interface on the sides as the disc itself is rotating and it will act like a wall.
Also when I am creating the geometry I normally create a cylinder outside the wind mill rotor and then boolien - subtract the wind mill from that , so I get the fluid volume to be meshed. Same as what you see in the video. But am not sure why the guys at support told me that I dont need interface on the sides as the discs are rotating as well and i just need the interface along the length of the turbine blades.
Am new to this turbomachinery and hence I am not sure how it works.
Then comes the question if I can do a symmetry and do the computations. But when I do the symmetry I have to split the geometry exactly at the middle, that means I have to cut at the center of the disc, then again there wornt be any interface on one side as its already a wall. (sorry If I am complicating by explaining) !!

Gert-Jan · April 10, 2018, 07:18

Provide a screenshot of your full 3D-setup in CFX-Pre.
Meaning, not the setup of you symmetrical case.

AS_Aero · April 13, 2018, 07:19

Hi
Sorry for the delay in uploading the image
The following link has the image !!
https://ibb.co/btmUnS
https://ibb.co/gcVpnS

Now the question is can I do a symmetry at the centerplane and do the simulation ? The complete geometry is of 2.1m length and the blade alone is 2m.
Regarding the interface is it enough if I have an interface only along the length of the turbine blades ?

Here I cant do 2D simulation or can I ? As I have a plate/disc at the center which is used to support the blade !! And I have the casing which covers the rotor /blades and their influence will be huge on the rotation of the blades right ?

Gert-Jan · April 13, 2018, 07:37

Given your geometry, I assume that you create a large cilinder as interface around the turbine and extent it up on to the internal wall of housing. At least, I would do it that way. In that case you don't need an interface at the bottom and top part of the cilinder, since these surfaces are part of the housing. But remember that you define them as Counter Rotating Wall in Pre. So that they effectively stand still.

Certainly you can simulate it using a symmetry plane in the middle. Why not? As long as your wind is normal to the turbine. The center plate will be cut in half. No props.

Certainly you can also do a 2D simulation. Why not? By comparing with other cases, you can deduce what the effect is of the plates and the housing. And it facilitates simulations for redesign the blades. So it gives you extra information. But you have to understand what you are doing. Meaning that you have to be careful extrapolating these results to full scale and different wind directions.

So, stay suspicious. Always!

AS_Aero · April 13, 2018, 09:14

Perfect !! I normally created the interface as per the video shown in youtube
https://www.youtube.com/watch?v=DUl74SGWC48
But the tech support guys told me I dont need any interface on the sides only along the length of the blade is enough, and the interface extends upto the outer surface of the disc on the rotor blade side and then the question comes there wornt be any meshsurface where the disc is there so how can i give it as interface.

Regarding the symmetry.. when I do the symmetry, how about the interface on the side of the symmetry ?

Then how big does this interface should be ? Is there any rule of thumb that my interface domain should be x times away from the rotor blade tip ?

Gert-Jan · April 13, 2018, 10:37

You should put the cilindircal interface half way the gap between rotor and housing.

I don't understand why you ask what to do with the interface on the side of the symmetry. Like the guy from support mentioned, there should only 1 cylindrical interface, round 360°. Now you cut this in half since you cut your whole geometry in half. So what happens is that the interface ends at the symmetry plane in a perpendicular way (90°). The same as at the other end of the interface where it ends on the internal wall of the housing.

Not?

AS_Aero · April 16, 2018, 03:38

The thing is first what I do is, I create the rotor domain separately and the stator part seperately and then I split it on the geometry exactly at the middle so as symmetry...So now I will have only one half of both stator and rotor part. But the interface will be there along the rotor diameter. I think I am confusing you. I will do it and send you the file, then you can have a look maybe if you have some time.

AS_Aero · April 16, 2018, 09:27

Hi
So as I said, I have attached the geometry file of the simulation, kindly have a look on the files if you have some time and if you have the ansys workbench platform, thats more easy as you can see the named surfaces of my geometry as well. The link to download is as follows !!

https://wetransfer.com/downloads/840...6132159/34b2af

Thanks in advance !!

Gert-Jan · April 16, 2018, 10:28

I don't have design modeler anymore. I replaced it is with spaceclaim.

Nevertheless, I could open your symmetrical geometry. I created a cross section and in principle it is ok.

But as I (read previous threads) and your support contact suggested, it is easier to use only 1 interface of 360°. For this you have to remove the circluar interface and extend your rotating domain up onto the inside wall of your housing. Then, this inside wall will be rotating since it ends up in your rotating domain. But if, in Pre, you set it as a CRW (counter rotating wall), it effectively stands still in your simulation. See my figure attached.

So, you end up with a single cilindrical interface of 360° (marked blue). This will save you some elements since you don't need to a lot of refinement in the small gap where the circular interface was located.

I marked the faces yellow that should be symmetrical. These are both in rotating and in stationary domain.

AS_Aero · April 17, 2018, 03:08

Dear Gert

Thanks a lot for your information. Yes this is what I was also thinking, but I was sceptic about the CRW, will I have to select that face alone in the Stator/casing part and name it as a wall with CRW option ? And I should give the negative rotation velocity or negative RPM ?

April 5, 2018, 05:03	Scaling down of Geometry	#1
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Hi All I am trying to do a Vertical axis wind turbine simulation and my entire geometry is of 2m length/height and if I want to simulate that, its going to be a huge simulation although I want to see the effects around the wind turbine and within the turbine as well. And another important thing I want to study is the wind turbine power for a particular RPM and wind velocity. So now my question is can I scale up my entire geometry by 2cm or 20cm and study the effects ? This will be more easy for me to do the computation but my doubt is will it affect the results or can I do the scaling for the results also ? Second thing is doing a 2D simulation or taking a small portion of the geometry and do the computation ? Which method is better ?

April 5, 2018, 06:34		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	I agree with Gert-Jan. Don't scale, simulate it real size. As you probably know, when you scale you keep the important non-dimensional numbers (like Reynolds Number, Rayliegh Number etc) the same by changing the geometry and using some other factor, maybe fluid speed or material properties; such that the non-dimensional numbers are unchanged. But for any model of reasonable complexity you will find several non-dimensional numbers are important and it is not possible to keep them all the same. So you have to choose which one you keep the same and which one you vary. In other words, scaling introduces a source of error as some non dimensional numbers must be changed. 2D simulation: See the FAQ: https://www.cfd-online.com/Wiki/Ansy..._simulation.3F If your flow can be modelled as 2d then you should model it 2d as it will make modelling far easier. But be aware that just because the geometry is 2d does not mean the flow is 2d. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

April 5, 2018, 07:42		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	For the 2D question: Please post an image of what you are modelling so we can understand your geometry. For the scaling question refer to Michael's answer __________________ 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
[DesignModeler] Fill tool - grouping the faces of a complicated geometry?	HeikkiT	ANSYS Meshing & Geometry	8	July 20, 2016 07:37
Export geometry file from ansys mechanical	browns6	Structural Mechanics	0	August 27, 2013 16:19
CFX POST Geometry Scaling	monkey1	CFX	2	July 11, 2013 04:01
Problem Importing Geometry ProE to CFX	fatb0y	CFX	3	January 14, 2012 19:42
2D geometry to 3D geometry	Sgonzalezg	ANSYS Meshing & Geometry	11	April 8, 2011 11:02

April 5, 2018, 05:41		#2
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,827 Rep Power: 27	In my opinion the strong point of CFD is that you don't have to scale up or down. So from a CFD point of view I think it is a rather strange approach. Certainly you can do that, and then scale the power using affinity rules. Either for upscaling and downscaling. But I think you cannot save a lot of elements on small scale. Geometry details will remain the same, not? Alternatively buy HPC packs, a facter and larger computer........

April 5, 2018, 07:16		#4
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Dear Glenn and Gert Thanks a lot for your valuable answers. The thing why I thought of scaling is since I want to simulate the effect of the wind turbine by placing it on a tall building which is again 3m tall and then the far field also I need to extend so on the whole my air domain will be around 10m length and 5m tall so its really a huge domain atleast for meshing and i might need that many cores to use for one computation. So if I convert all this meter by cm 10cm*5cm then the amount of mesh required will be drastically reduced and still i can study the effects. Second thing regarding the 2D simulation, I have more than 5 blades and hence to study the blade interaction and the interaction of the turbine itself with the case and structures I am not sure if 2D will help, but if I want to see how the Power produced by the turbine and the Cp values wornt this 2D be enough ? And this was also suggested by the Ansys customer support. But I dint understand by '' flow can be modeled as 2D '' and I have an inlet face , so in 2D it will be a line. Then I also have a doubt about the interface region ! In 3D I will have interface along the length of the turbine blade and on both sides of the turbine, but in 2D I will have only one interface which is around the blades, and in CFX we cant do 2D but a single cell thickness. so should I still give interface on both sides or it doesnt matter ?

April 5, 2018, 07:39		#5
AtoHM Senior Member M Join Date: Dec 2017 Posts: 642 Rep Power: 12	I dont know why you think "the amount of mesh" will be reduced by scaling? Assume you have a mesh cell of 1m³ at the boundary of your domain and a cell close to the blade with, IDK, 0.005 m³. If you scale everything, the total number of elements will be the same, only your absolute element size will be reduced. The number of cells will only reduce if you scale different regions differently, leading to a coarser mesh.

April 5, 2018, 08:20		#8
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Yes it makes sense, even if I scale the entire geometry it might not really help me. Sorry it was my stupid thought that I will get reduced cells. But its not.

April 10, 2018, 05:16		#9
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Sorry for the late reply . .. The CAD is almost similar to the video link in the Youtube : https://www.youtube.com/watch?v=DUl74SGWC48 Here this guy is creating an interface on both sides of the rotor disc where the blades are attached, but the customer service technical support said we dont need that ! Can someone tell me if its necessary or not ! And my geometry is around 2m length and it also has some casing around the turbines which i consider as a part of stationary parts.

April 10, 2018, 06:31		#10
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,827 Rep Power: 27	The windmill in the movie requires 3 interfaces. If your geometry requires 2 or 3 is impossible to say since we don't know your geometry. As a first guess I would say you need three as well. That would sound most logical. Only if your bottom disc is on the same height as a surrounding wall (where the windmill is standing on), then you don't need to have it. Or does the support mean you can group the top and the bottom side into a single interface. Then in Pre you only have to define 2 interfaces. But in the run, you will still have three interface surfaces. That would not make any difference.

April 10, 2018, 07:08		#11
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Mine is completly same just that there is a casing outside the windmill, and the length is much more. That means I have these discs as support for blade every 500cm. So my entire geometry is 2m length so 4 times like this. And have disc on both ends also. But the ansys support told me you dont need any interface on the sides as the disc itself is rotating and it will act like a wall. Also when I am creating the geometry I normally create a cylinder outside the wind mill rotor and then boolien - subtract the wind mill from that , so I get the fluid volume to be meshed. Same as what you see in the video. But am not sure why the guys at support told me that I dont need interface on the sides as the discs are rotating as well and i just need the interface along the length of the turbine blades. Am new to this turbomachinery and hence I am not sure how it works. Then comes the question if I can do a symmetry and do the computations. But when I do the symmetry I have to split the geometry exactly at the middle, that means I have to cut at the center of the disc, then again there wornt be any interface on one side as its already a wall. (sorry If I am complicating by explaining) !!

April 10, 2018, 07:18		#12
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,827 Rep Power: 27	Provide a screenshot of your full 3D-setup in CFX-Pre. Meaning, not the setup of you symmetrical case.

April 13, 2018, 07:19		#13
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Hi Sorry for the delay in uploading the image The following link has the image !! https://ibb.co/btmUnS https://ibb.co/gcVpnS Now the question is can I do a symmetry at the centerplane and do the simulation ? The complete geometry is of 2.1m length and the blade alone is 2m. Regarding the interface is it enough if I have an interface only along the length of the turbine blades ? Here I cant do 2D simulation or can I ? As I have a plate/disc at the center which is used to support the blade !! And I have the casing which covers the rotor /blades and their influence will be huge on the rotation of the blades right ?

April 13, 2018, 07:37		#14
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,827 Rep Power: 27	Given your geometry, I assume that you create a large cilinder as interface around the turbine and extent it up on to the internal wall of housing. At least, I would do it that way. In that case you don't need an interface at the bottom and top part of the cilinder, since these surfaces are part of the housing. But remember that you define them as Counter Rotating Wall in Pre. So that they effectively stand still. Certainly you can simulate it using a symmetry plane in the middle. Why not? As long as your wind is normal to the turbine. The center plate will be cut in half. No props. Certainly you can also do a 2D simulation. Why not? By comparing with other cases, you can deduce what the effect is of the plates and the housing. And it facilitates simulations for redesign the blades. So it gives you extra information. But you have to understand what you are doing. Meaning that you have to be careful extrapolating these results to full scale and different wind directions. So, stay suspicious. Always!

April 13, 2018, 09:14		#15
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Perfect !! I normally created the interface as per the video shown in youtube https://www.youtube.com/watch?v=DUl74SGWC48 But the tech support guys told me I dont need any interface on the sides only along the length of the blade is enough, and the interface extends upto the outer surface of the disc on the rotor blade side and then the question comes there wornt be any meshsurface where the disc is there so how can i give it as interface. Regarding the symmetry.. when I do the symmetry, how about the interface on the side of the symmetry ? Then how big does this interface should be ? Is there any rule of thumb that my interface domain should be x times away from the rotor blade tip ?

April 13, 2018, 10:37		#16
Gert-Jan Senior Member Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,827 Rep Power: 27	You should put the cilindircal interface half way the gap between rotor and housing. I don't understand why you ask what to do with the interface on the side of the symmetry. Like the guy from support mentioned, there should only 1 cylindrical interface, round 360°. Now you cut this in half since you cut your whole geometry in half. So what happens is that the interface ends at the symmetry plane in a perpendicular way (90°). The same as at the other end of the interface where it ends on the internal wall of the housing. Not?

April 16, 2018, 03:38		#17
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	The thing is first what I do is, I create the rotor domain separately and the stator part seperately and then I split it on the geometry exactly at the middle so as symmetry...So now I will have only one half of both stator and rotor part. But the interface will be there along the rotor diameter. I think I am confusing you. I will do it and send you the file, then you can have a look maybe if you have some time.

April 16, 2018, 09:27		#18
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Hi So as I said, I have attached the geometry file of the simulation, kindly have a look on the files if you have some time and if you have the ansys workbench platform, thats more easy as you can see the named surfaces of my geometry as well. The link to download is as follows !! https://wetransfer.com/downloads/840...6132159/34b2af Thanks in advance !!

April 17, 2018, 03:08		#20
AS_Aero Senior Member Join Date: Mar 2013 Location: Germany Posts: 357 Rep Power: 14	Dear Gert Thanks a lot for your information. Yes this is what I was also thinking, but I was sceptic about the CRW, will I have to select that face alone in the Stator/casing part and name it as a wall with CRW option ? And I should give the negative rotation velocity or negative RPM ?