Feature Curve Definition and Boundary Splitting

screech1987 · November 30, 2010, 12:36

Hi,

Currently I have having problem defining my geometry and unstructured Poly mesh in two separate cases.

Firstly, I am meshing a 3D swept wing (.dbs file) with a set limit of around 200000 cells. I am experiencing problems with refinement in a small region at the wing tip with a 'saw tooth' effect. To solve this I am trying to define a feature curve to which the mesh will adhear to erradicate this. For accuracy this curve should follow the CAD geometry, but all the methods I have tried seem to want to follow the existing mesh in the .dbs file.

Second problem, is when I load in geometry for a flat plate case, Star merges several boundaries which make up the plate and adjacent freestream flow. This is even with 'Load all edges' ticked on the loading of the geometry (.stl, .Iges, parasolid). This leaves me with one large flat boundary which should be split into a wall and a flow section. But all the methods I have tried to split the boundary have failed.

Any ideas?

Cheers
Martin

abdul099 · January 6, 2011, 17:29

For the first problem, you can try to play around with the parameters for feature curve creation. When it doesn't work, you can either create an empty feature curve and mark the edges by hand or just edit the old one.

For the second problem, did you choose "One Boundary per part surface" when importing the geometry? If you've done so, it should create several boundaries which can be combined (way more comfortable than splitting boundaries).
When you have choosen "One Boundary per part", it will do what it should do, create only one single boundary for the whole part and you have to split it up.
If that wasn't the problem, I'm still struggling to understand the problem. What is "a wall and a flow section"? Maybe a picture would be helpful...
In general, you can split boundaries by many ways, depending on your model - there's no general rule how to split boundaries for a "3D swept wing (.dbs file) with a set limit of around 200000 cells" case.

screech1987 · January 7, 2011, 09:45

Robin,

Yeah I tried everything, but must be due to being a .dbs file where the CAD doesn't really exist. Had to resort to just adding to the existing feature curves on the imported 'mesh' of the .dbs, but this does lead to quite a zig-zaggy path. But it provided acceptable results.

No that was not the problem, basically what i meant about a 'wall and a flow section' was there is a plate of length 1.7m, which forms the bottom of the computational domain, however for inlet values and flow development, the domain was extended 0.15m upstream of the plate. Thus the bottom of the computational domain is made up of a freestream boundary and a wall boundary adjacent to each other.

However on a high level, do you know:

A) How to add feature curves to existing geometry within star, which are defined by CAD/ specific co-ordinates?

B) how do I split a boundary (which is all in lets say y=0), into separate boundaries at specific co-ordinate locations. (through the use of feature curves if needs be)?

Thanks Again for your advice.

abdul099 · January 7, 2011, 21:34

Hi screech,

For your B), the easiest way is to build your cad model with seperate surfaces. You can split boundaries in ccm+ "by patch", which is nothing else than cut single (or multiple) surfaces from the cad model out of a boundary and put them into a new one.

If that isn't possible, you can try to build a new body in the ccm+ cad modeler which cuts the boundary you want to split. Afterwards you can intersect the boundaries which will create a feature curve where one boundary intersects the other one and you can split the boundary by feature curve.

Another possibility when you want to split a planar boundary is to generate a block region which touches the boundary everywhere where you want to have it split up in a seperate boundary. Then go to the surface repair -> Merge / Imprint, choose "Mulit region imprint" -> "find pairs" and imprint them. Leave the surface repair and delete the generated interfaces and the block region. And here you go, you will have a splitted boundary, and if necessary, you can mark it with a feature curve (mark by boundary perimeter).

And when all of this is not possible and it's only to define the inlet boundary and you have already a volume mesh, you can also generate a field function which switches a value from 0 to 1 at a particular position and cut by this field function. (It will not look nice with a poly mesh, better to do this with a trimmed mesh, especially in combination with the trimmer mesh alignement)

For A), I would recommend either to generate the patches in CAD (you can mark patch perimeters with feature curves) or the second suggestion with the new body and intersecting or imprinting the boundaries.
You can also generate a feature curve by hand by clicking on vertices, but you are limited to a surface representation. So with that, you can only generate a feature curve where a edge of your surface triangulation (either imported or remeshed) is present.

Hope this helps - if not, don't hesitate to ask again.

Regards

screech1987 · January 8, 2011, 06:11

The method idea for splitting boundaries works great!

For your answer to A), could you explain in a little more detail about the patch generation? (and does this work for un-planar surfaces or regions of high curvature?)

Thanks again, and sorry for the dumb questions haha

Martin

abdul099 · January 18, 2011, 15:23

Hi Martin,

there are no dumb questions, only dumb answers

Patch generation is meant to take place in an external CAD program, like Catia, NX, ProE... A patch is nothing else than a single surface of your body.
For Catia V5, I know, you can split a surface by defining a line on the surface or generating an intersecting surface.

When you import the geometry in a native CAD format or in parasolid (I thing, IGES doesn't work, but I'm not sure), ccm+ should keep the patches build in the cad program.
Then you can split boundaries "by patch". It works for arbitrary shaped surfaces due it's only dependend on the definition of the surfaces in the cad.

Don't know about splitting surfaces in the cad modeller now, but when I find something out, I will share it with you (and the other guys in this forum).

Cheers

aero17 · November 12, 2017, 14:18

I recently downloaded the mesh from the NASA site of a ZPG flat plate so that I could duplicate the results using various turbulence models in Star. To duplicate the NASA boundary conditions, I needed to make part of the floor symmetry BC and part of the floor a wall BC. I was able to split be angle and choose 0 degrees to separate the meshed floor into multiple patches. That was fairly easy except for having to combine many multiple patches back together. But using shift you can choose multiple patches from the model tree.

November 30, 2010, 12:36	Feature Curve Definition and Boundary Splitting	#1
screech1987 New Member Martin Join Date: Nov 2010 Posts: 23 Rep Power: 16	Hi, Currently I have having problem defining my geometry and unstructured Poly mesh in two separate cases. Firstly, I am meshing a 3D swept wing (.dbs file) with a set limit of around 200000 cells. I am experiencing problems with refinement in a small region at the wing tip with a 'saw tooth' effect. To solve this I am trying to define a feature curve to which the mesh will adhear to erradicate this. For accuracy this curve should follow the CAD geometry, but all the methods I have tried seem to want to follow the existing mesh in the .dbs file. Second problem, is when I load in geometry for a flat plate case, Star merges several boundaries which make up the plate and adjacent freestream flow. This is even with 'Load all edges' ticked on the loading of the geometry (.stl, .Iges, parasolid). This leaves me with one large flat boundary which should be split into a wall and a flow section. But all the methods I have tried to split the boundary have failed. Any ideas? Cheers Martin

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Wind turbine simulation	Saturn	CFX	60	July 17, 2024 06:45
RPM in Wind Turbine	Pankaj	CFX	9	November 23, 2009 05:05
CFX doesn't continue calculation...	mactech001	CFX	6	November 15, 2009 22:25
Concentric tube heat exchanger (Air-Water)	Young	CFX	5	October 7, 2008 00:17
New topic on same subject - Flow around race car	Tudor Miron	CFX	15	April 2, 2004 07:18

January 6, 2011, 17:29		#2
abdul099 Senior Member Join Date: Oct 2009 Location: Germany Posts: 636 Rep Power: 22	For the first problem, you can try to play around with the parameters for feature curve creation. When it doesn't work, you can either create an empty feature curve and mark the edges by hand or just edit the old one. For the second problem, did you choose "One Boundary per part surface" when importing the geometry? If you've done so, it should create several boundaries which can be combined (way more comfortable than splitting boundaries). When you have choosen "One Boundary per part", it will do what it should do, create only one single boundary for the whole part and you have to split it up. If that wasn't the problem, I'm still struggling to understand the problem. What is "a wall and a flow section"? Maybe a picture would be helpful... In general, you can split boundaries by many ways, depending on your model - there's no general rule how to split boundaries for a "3D swept wing (.dbs file) with a set limit of around 200000 cells" case.

January 7, 2011, 09:45		#3
screech1987 New Member Martin Join Date: Nov 2010 Posts: 23 Rep Power: 16	Robin, Yeah I tried everything, but must be due to being a .dbs file where the CAD doesn't really exist. Had to resort to just adding to the existing feature curves on the imported 'mesh' of the .dbs, but this does lead to quite a zig-zaggy path. But it provided acceptable results. No that was not the problem, basically what i meant about a 'wall and a flow section' was there is a plate of length 1.7m, which forms the bottom of the computational domain, however for inlet values and flow development, the domain was extended 0.15m upstream of the plate. Thus the bottom of the computational domain is made up of a freestream boundary and a wall boundary adjacent to each other. However on a high level, do you know: A) How to add feature curves to existing geometry within star, which are defined by CAD/ specific co-ordinates? B) how do I split a boundary (which is all in lets say y=0), into separate boundaries at specific co-ordinate locations. (through the use of feature curves if needs be)? Thanks Again for your advice.

January 7, 2011, 21:34		#4
abdul099 Senior Member Join Date: Oct 2009 Location: Germany Posts: 636 Rep Power: 22	Hi screech, For your B), the easiest way is to build your cad model with seperate surfaces. You can split boundaries in ccm+ "by patch", which is nothing else than cut single (or multiple) surfaces from the cad model out of a boundary and put them into a new one. If that isn't possible, you can try to build a new body in the ccm+ cad modeler which cuts the boundary you want to split. Afterwards you can intersect the boundaries which will create a feature curve where one boundary intersects the other one and you can split the boundary by feature curve. Another possibility when you want to split a planar boundary is to generate a block region which touches the boundary everywhere where you want to have it split up in a seperate boundary. Then go to the surface repair -> Merge / Imprint, choose "Mulit region imprint" -> "find pairs" and imprint them. Leave the surface repair and delete the generated interfaces and the block region. And here you go, you will have a splitted boundary, and if necessary, you can mark it with a feature curve (mark by boundary perimeter). And when all of this is not possible and it's only to define the inlet boundary and you have already a volume mesh, you can also generate a field function which switches a value from 0 to 1 at a particular position and cut by this field function. (It will not look nice with a poly mesh, better to do this with a trimmed mesh, especially in combination with the trimmer mesh alignement) For A), I would recommend either to generate the patches in CAD (you can mark patch perimeters with feature curves) or the second suggestion with the new body and intersecting or imprinting the boundaries. You can also generate a feature curve by hand by clicking on vertices, but you are limited to a surface representation. So with that, you can only generate a feature curve where a edge of your surface triangulation (either imported or remeshed) is present. Hope this helps - if not, don't hesitate to ask again. Regards

January 8, 2011, 06:11		#5
screech1987 New Member Martin Join Date: Nov 2010 Posts: 23 Rep Power: 16	The method idea for splitting boundaries works great! For your answer to A), could you explain in a little more detail about the patch generation? (and does this work for un-planar surfaces or regions of high curvature?) Thanks again, and sorry for the dumb questions haha Martin

January 18, 2011, 15:23		#6
abdul099 Senior Member Join Date: Oct 2009 Location: Germany Posts: 636 Rep Power: 22	Hi Martin, there are no dumb questions, only dumb answers Patch generation is meant to take place in an external CAD program, like Catia, NX, ProE... A patch is nothing else than a single surface of your body. For Catia V5, I know, you can split a surface by defining a line on the surface or generating an intersecting surface. When you import the geometry in a native CAD format or in parasolid (I thing, IGES doesn't work, but I'm not sure), ccm+ should keep the patches build in the cad program. Then you can split boundaries "by patch". It works for arbitrary shaped surfaces due it's only dependend on the definition of the surfaces in the cad. Don't know about splitting surfaces in the cad modeller now, but when I find something out, I will share it with you (and the other guys in this forum). Cheers

November 12, 2017, 14:18		#7
aero17 New Member Barry Join Date: Nov 2017 Posts: 1 Rep Power: 0	I recently downloaded the mesh from the NASA site of a ZPG flat plate so that I could duplicate the results using various turbulence models in Star. To duplicate the NASA boundary conditions, I needed to make part of the floor symmetry BC and part of the floor a wall BC. I was able to split be angle and choose 0 degrees to separate the meshed floor into multiple patches. That was fairly easy except for having to combine many multiple patches back together. But using shift you can choose multiple patches from the model tree.