[ErdemEskioglu]

Hello,

I am a new user in Pointwise and I have a question about block creation.
I am going to analyze my complete aircraft body which is placed in the rectangular control volume.
I have my geometry modelled in CATIA V5 exported as IGES, imported to pointwise and created unstructured domains on aircraft surfaces and control volume surfaces but I couldn't create a block.

I'm trying to create a block with a command Create>Assemble Special>Block.
I'm selecting the domains I've created starting from control volume domains then save the face with command Save Face. Then Fuselage domains which is okay too. My problem is wing surface domains. I'm selecting the wingtip domain,upper and lower surfaces domain of the wing and pointwise won't let me to create face. I'm only able to create face of wing when I create and select as domain of thewing-fuselage attachment area but I'm not sure If it's right selecting the attachment domain.
As you see in the picture I'm not able to create a face of the wing.
What should I do?

I'm uploading picture of the problem I hope you will understand the situation.

Kind Regards,
Erdem Eskioglu

[RcktMan77]

Hi Erdem,

If the entire aircraft body exists within your rectangular control volume, then you would want to create the unstructured block by selecting the domains associated with the aircraft body (fuselage, wing, tail, etc.) as one face and the outer control volume boundaries as the second face. If your control volume includes a symmetry plane, then you would select all of the aircraft body domains, the symmetry plane, and outer control volume domains and save those all as one face, since they should be simply connected. Typically, if your control volume is watertight, you should be able to simply select all of the domains and use the Assemble Blocks toolbar item to have Pointwise automatically assemble the block for you.

For your simulation, if you would like to have separate boundary conditions for the component surfaces of your aircraft in order to isolate surfaces for force and moment integration, then you can create unique boundary condition names for each component in the Set BCs panel found via the CAE menu. Here you might add a new boundary condition, name it wing-upper, and give it a viscous boundary condition type appropriate for your selected CAE solver. The specific CAE solver is set using the Select Solver... option also in the CAE menu.

I hope that helps answer your question. If you need additional clarification, then it might help if you can provide your Pointwise project file.

[ErdemEskioglu]

Hi Zach,

Firstly, thank you for your interest.
I have my entire body within the control volume there is no symmetry condition.
I am able to create a face of control volume by selecting connecting six faces of my rectangular volume. But I cannot create my aircraft body as one face. I'm able to create face seperately (e.g one face for fuselage then one face for vertical tail etc.) my geometry is watertight I think, I trimmed surfaces going into the fuselage and saved that way. I don't know what I'm doing wrong.
I can send you the my .pw file if you can give me your e-mail.

Thanks,

[RcktMan77]

Hi Erdem,

After looking at your Pointwise project file, I noticed that the domains which you have created on the fuselage and vertical tail don't include internal edges for the wings and empennage.

To correct this you would first select the domain--on the fuselage for example--and then from the Edit menu choose the "Add/Remove Edges..." option. Once the Add/Remove Edges panel opens you will want to select the edges which correspond to the root of your wing using the Display window. You should see the edges turn yellow with an arrow indicating a direction. You want the direction that this arrow points to be opposite the direction shown for the outer edge. If the edge's direction isn't already oriented in a direction opposite to the direction of the outer edge, you can flip the selected edge's direction using the "Flip Edge Orientation" button shown in the Add/Remove Edges panel. Then click the "Save Edge" button to add the interior edge to the domain, and click "OK" to exit the Add/Remove Edges panel.

You will want to repeat these steps for each domain where you have intersecting components on your aircraft which includes two more locations on the fuselage for the opposite wing and vertical tail, and then two domains on the vertical tail that intersect the horizontal tail.

Once you have edited all of these domains, then you should be able to select all of the domains using the List panel or Display window and click the Assemble Blocks toolbar shortcut. I've done all of this for you and saved the project file which you can download here as a reference for what the domains should look like once the internal edges have been included.

[ErdemEskioglu]

Hi Zach,

Thank you so much for your help. I cannot find Add/Remove edges menu but I figured it out and created new domains by special command. Now I'm able to create whole body as one face.
Now I am going to focus on boundary layer mesh creation and wake region mesh refinement. Can you suggest documents about these steps?

Best Regards,
Erdem Eskioglu

[RcktMan77]

Hi Erdem,

Pointwise provides a number of online resources demonstrating how to use the software in addition to the tutorials included with the installation. There are links on Pointwise's main website to Do-It-Yourself (DIY) training pages, webcasts, and more in-depth webinars which provide a number of video resources to demonstrate how to leverage the variety of features in Pointwise.

We also have an ongoing Tutorial Tuesday video series on our CFDMeshing YouTube channel where we premiere a new 2 to 3 minute video that demonstrates how to use a new feature of Pointwise every Tuesday. You might find this webinar on T-Rex useful for learning more about boundary layer meshing in Pointwise.

Hope that helps get you started!

[ErdemEskioglu]

Hi Zach,

Thank you for your support. I will watch the videos.

Thanks,
Erdem

[jitendraseregar@gmail.com]

what is the units of SU2 export type file from pointwise? I mean the grid file is in m or cm ........? or non-dimesional

[RcktMan77]

Pointwise will export the mesh using the dimensional units you choose to work in. For example, if I opt to work with inches, then I would scale my geometry definition to match the model's size as it would be represented in inches. Then I can proceed to mesh the geometry, and the distances, spacings, etc. that Pointwise reports and exports will correspond to inches; and thus, inches becomes the units of my grid. You can do the same for whichever units you prefer, or work in a dimensionless environment altogether.

[jitendraseregar@gmail.com]

Originally Posted by RcktMan77

Pointwise will export the mesh using the dimensional units you choose to work in. For example, if I opt to work with inches, then I would scale my geometry definition to match the model's size as it would be represented in inches. Then I can proceed to mesh the geometry, and the distances, spacings, etc. that Pointwise reports and exports will correspond to inches; and thus, inches becomes the units of my grid. You can do the same for whichever units you prefer, or work in a dimensionless environment altogether.

Suppose if I want grid size in mm. So how much scaling is to be done. Can you help?

[RcktMan77]

Well, you first need to know what dimensions were used when creating the geometry definition (CAD) file that you imported into Pointwise. Once you determine which dimensions were used, then it is straightforward to select the appropriate scaling factors to scale the analysis model from the units it was created into something in millimeters. You can determine the extent of the geometry by selecting Properties from the File menu after importing your CAD into Pointwise. From the table in the Properties panel you can ascertain the size of your model, and what units it was created in.

If you are not importing a CAD file, and you're either creating the geometry within Pointwise, or you're not using a geometry definition at all to create your mesh, then Pointwise is dimensionless. This means that 1 grid unit can be whatever dimension you wish it to be; thus, an edge spacing of one on a connector can be an inch, a centimeter, a millimeter, or whichever dimension you prefer.

[adi.ptb]

Hello PointWise Users,

I have a problem that I need to simulate but first I have to generate a high quality mesh for it and a mesh with full control. The problem is a lobed mixer. It consists of an annular duct formed from concentric pipes, where the trailing edge of the outer pipe is shaped into 12 lobes that are uniformly spaced in an axisymmetric manner around the centerline. The trailing edge of the inner pipe closes to form a conical plug. I have attached the pictures of the geometry. The computational domain is circumferentially sized to include only a quarter of the flowfield, with periodic conditions imposed on the two circumferential ends of the domain. I think I have provided enough information about the geometry and computational domain and it’s time to talk about a kind of mesh that I must generate for the computational domain.
The mesh should be as follow, the surfaces of the lobes and the conical plug must have structured hexa cells except for the nose of the conical plug. Also some inflation layers around the lobes and tri cells for the volume mesh. I was asked to mesh this domain in ANSYS ICEM CFD but after a week struggling with ICEM without any progress I searched for other solutions. Actually, creating so many blocks for the lobes and plugs are very tedious in ICEM. It gets really messy. It’s been 3 days since I have found this great mesh generator (PointWise) and I’m thinking about shifting to it. I worked with its tutorials and it’s really flexible and highly automated which can save a great deal of time for complex geometries like what I have In hand.
So after working with PointWise a little bit I gave the problem a try and I was able to generate the kind of surface mesh that I need which I was not able to generate in ICEM and this is a great progress. I just need to generate the volume mesh to get it done. After generating the surface mesh for all the domains I selected all of the domains and assembled an unstructured block for them. PointWise shows that it is working but it seems that nothing happens and no block is generated. I also used create, assemble special to select the outer boundaries of the domain and then select the interior domains to create a block but there is no option to save the faces (it’s off). I don’t have enough experience in PointWise to figure out what the problem is so I ask for your help. I have attached some pictures and a link to the file.

Thanks in advance

https://www.dropbox.com/s/a9wvrpnlxvmxf4j/LobedMixer2WedgeSurfaceMesh.pw?dl=0

[RcktMan77]

Hi adi,

One problem is that the domains that you have created along your symmetry boundaries for your outer control volume overlap other domains that lie along these same axisymmetric planes. You need to either re-create these domains taking into account your existing domains where there is overlap, or you need to use the Add/Remove Edges... command found under the Edit menu (as previously mentioned in this thread) to add internal edges for these domains which correspond the boundaries of the surface mesh for your geometry.

Another problem is that you seem to have included separate control volumes inside of your geometry. This is fine for FEA simulations, but if you're simply running CFD simulations, then there should be a single control volume that surrounds the wetted surface.

I've made these changes already, so hopefully you can visually see the differences. There are still a number of issues with mesh spacing, particularly near the surface of your geometry that you will need to modify, but this should address your original problem. You can download the file here.

[adi.ptb]

Dear Zach,
Thank you very much for your help. I really appreciate it. You saved me.
I looked at the modifications that you made and I have some questions to ask you. First of all I must mention that I did a boolean operation in SolidWorks to subtract the conical plug from the rest of the volume but when I imported the geometry into the PointWise there was so many free edges. Back to your modifications, I tried to replicate what you did. I deleted the domains associated with the conical plug on the symmetry planes and the back of the plug and also their connectors. Then I selected the domains on the symmetry planes and edit, Add/Remove Edges and then picked the loop of connectors that form a domain on the symmetry planes and then save the edge and ok. Then selected all of the domains and assemble blocks. Is this correct?

Thanks

[RcktMan77]

Hi Adi,

With regards to the free edges you are seeing, some of them are valid--basically all of the geometry curves on the symmetry planes are valid free edges. You can typically assemble a single watertight model of your geometry within Pointwise prior to meshing. This basically involves selecting the collection of related database surface entities and either using the Create -> Assemble -> Models... command, or using the corresponding Assemble Models toolbar shortcut. We typically begin with the full model to ensure that there are no free edges before splitting the model along symmetry planes. If the full model geometry is available as a single part in Solidworks, then you should be able to save off that component as a separate *.sldprt file, and read that directly into Pointwise.

With regards to re-creating the domains and assembling blocks, this is pretty much what I did. In the Add/Remove Edges panel I had to select the Restart Domain button prior to defining the closed loop of connectors for its edge.

[adi.ptb]

Hi Zach,

Thanks for your explanations. I'm still unable to replicate what you did. I followed your suggestion and deleted all of the domains on the symmetry planes including the domains of the volume and the plug and also a domain on the back of the plug and a thin domain at the back of the lobe. After that I deleted the connectors of the conical plug along the symmetry planes and its connectors on the back. Then I created new domains on the symmetry planes using the existing connectors. I didn't use Add/Remove Edges. After that I went to Create,Assemble special,Blocks and use automatic method to create a block since selecting all of the domains and hitting the assemble blocks button didn't generate any block. After that I initialized the block and after about half an hour PointWise produced two messages.
Error: Could not Import the tets!
Warning: One or more entities could not be initialized
I wanted to ask you if this has anything to do with the seperate control volumes inside the geometry as you mentioned and would you mind explain a bit about how you resolve this issue.

Thanks so much

[adi.ptb]

Hi Zach,

I was able to resolve the issue.

[RcktMan77]

Hi adi,

Sorry, it's been a busy morning, but I'm glad to hear you have managed to figure things out.

Best Regards,



Zach

[adi.ptb]

Hi Zach,

Sorry to bother you again. I have a problem that I hope you can help me with. I tried to create some inflation layers to resolve the boundary layers around the lobes and the plug. So I selected the desired structured domains on the lobes and plug and extruded them to create inflation layers. After creating inflation layers I ended up with 10 new structured blocks. When I tried to assemble an unstructured block for the volume (The block that you created) I couldn’t assemble it because there was only one closed face in the volume. For resolving this issue I used this approach. First I created an unstructured block for the entire volume and then assigned a layer to this block and turned it off. After that I created structured blocks for the inflation layers. Now I have new domains (inflation domains) that I don’t know what is the proper boundary condition for them. I left them unspecified and exported the mesh to OpenFoam and then checked the mesh in OpenFoam and there was problems. I have attached a figure from checking the mesh in OF. I want to ask you if I have created the inflation layers correctly in the first place. My other question is about hyperbolic extrusion that we use for generating the inflation layers. I used the y plus calculator in the PointWise website and specified a step size for the extrusion with certain number of steps. How can I find out about the total height of the inflation layer with specified step size and number?

Thanks a lot

[RcktMan77]

Hi adi,

It sounds from your description (and OpenFOAM's error message confirms this) that the unstructured block that you created for the outer volume overlaps the blocks you created via hyperbolic extrusion. These blocks should be point matched unless you're attempting to create an overset mesh. Given that you're using OpenFOAM and it doesn't yet fully support overset meshes, then I'm inclined to think this isn't what you want.

You should start with your surface mesh, select the domains that you wish to extrude, perform the extrusion, and then from the domains created at the extent of your extrusion use connectors to create the topology for your farfield. These domains now become your new surface mesh face so-to-speak when defining your outer unstructured block.

With regards to determining the extent of the hyperbolic extrusion, it grows geometrically. You provide an initial spacing, a growth rate, and a number of layers to grow. You can simply calculate this: initDs*growthRate^(numSteps-1)

Alternatively, you can use option+right-click on any point or node in Pointwise's Display window (e.g. on a point or node at the extent of the extrusion) and then again on another point (e.g. a point on the surface), and Pointwise will display the distance between those two points in the Messages window.

Hope that helps!

Best Regards,



Zach