I would like to mesh a spherical surface with a nice, even mesh. The idea is to project a grid to the spherical surface.
I could do this in Inventor, I defined a 2D grid in a 2D sketch and after it was projected to the spherical surface in a +D sketch, so I have the grid points in a 3D sketch. I want to make a mesh with these points.
Is it possible to do this directly in Simulation?
How can I transfer the points of the 3D sketch to Simulation and use them as nodes?
Solved! Go to Solution.
If your geometry is really as simple as a sphere, you may be able to create it the fastest directly within Simulation. Please try the example "Ball in a Box with Body to Body Radiation Model" in the wiki Help to learn how to create geometry by hand.
You should be able to import your Inventor model directly. If you can split the surface of the sphere using your grid, the same surfaces will be created in Simulation. You might need to tweak the mesh size and other parameters so that generating the mesh created only one element per surface (if that's what you want) or N elements per surface.
Alternatively, you can add work points to all of the intersections on the sphere in Inventor. Then, there is an option to import the work points into Simulation. From the work points, you could then connect the dots to create your own mesh.
And now a question. Why do you want such a controlled mesh? Are you analyzing something unusual or really interesting?
16.9 years experience with Simulation Mechanical
Thanks for your reply, unfortunately I didn't have time to answer until now.
Please see the attached pictures, I try to explain the problem with those.
So let's say that the geometry is a concave surface with a thickness. It can't be treated like a thin wall object, I shouls use a 3d mesh. The geometry of the surface is not exactly spherical, just concave but it's rotationally symmetric.
I want to use a well controlled grid on tis surface.
My idea to generate this grid on the surface was the following:
Pict. 1. I do a grid with a point pattern in a 2D sketch.
Pict. 2. I start a 3D sketch and the grid is projected to the surface. Aim number 1 achieved, I have the nice nodes on the surface. But! These points are only sketch points, somehow I have to convert them into "workpoints" otherwise I can't import them to Multiphysics as nodes.
Pict. 3. I can put work point to every sketch point but only ONE BY ONE. I suppose I don't have to explain that this isn't a doable way.
So the main question is: Is there any opportunity to convert all of these points into workpoints? I tried to mark all of the points and put a workpoint to everyone with one click but it didn't work.
- Hi Ender,
I cannot think of any direct ways to create a 3D mesh with nodes in a pattern like you showed. There are some indirect ways to accomplish it. Whether they are viable will depend on the complexity of the model.
But before I go into the indirect methods, let me clarify my previous post (for the benefit of all readers). In the tutorial, a "line" was meshed and extruded, which creates a surface. If you create a mesh on a surface, extruding that mesh will create a 3D brick mesh. So for your concaved model, you could create a mesh of the cross-section and revolve it to get the solid mesh. Of course, the node pattern will be radial and tangential, not square as in your example.
If you really wanted the node pattern to have the arrangement that you showed (or any other pattern), here is one indirect way to do it.
1. Create a mesh of a thin, flat plate. Whether you use hand meshing techniques or import a solid model and mesh (using any of the options available) does not matter for this general technique, but your control may put some constraints on how you create the mesh.
2. Apply everything you need to complete the model (material properties, constraints, loads, etc).
3. Do a "Check Model" to get into the Results environment. This creates the nodes and elements used by the processor. The nodes are stored in a Foxpro-compatible database named NODES.DBF located in the ".ds_data\1\ds.mod" folder. (Substitute the actual design scenario number in place of the "1".)
4. Although not necessary, it may be helpful to exit from the software.
5. If you edit the NODES.DBF file, you can move the nodes to any location that you want! In your case, there are simple formulas based on the left/right, up/down, and thickness coordinate to calculate where the node should be on a spherical dome. Make the changes and save the file.
6. Open the model directly in the Results environment to confirm that your changes are correct. (Set the "File of Type" on the File > Open dialog to "Autodesk Simulation Results (*.fem)".)
7. One problem with this method is that the manual changes are not shown in the FEA Editor, and therefore you cannot run the analysis from within the software. (When the analysis is started from within the software, it always uses the model from the FEA Editor regardless of any manual changes you may have made.) You need to run the analysis from a command prompt. See the wiki help page "Schedule Analyses".
For editing the NODES.DBF, you might be able to do it directly in Excel or any programming language. Otherwise, you can convert the databases from the native Foxpro-format to text files, edit them, and convert them back to the native format. See the Help for the command "Tools > Options > Database Translation".
16.9 years experience with Simulation Mechanical
Thanks, it was a really helfpul answer! Sorry for the late answer! Now I can edit the nodes with a free dbf viewer.
I have another problem, it's more simple:
I have a result file with the XYZ coordiantes of the nodes, like this:
Node # 9 ( X = 508.198, Y = 110.16, Z = -4052.31 )
Displaced Position : X = 508.198, Y = 110.16, Z = -4052.31
Displacement = DX: 0.000241976, DY: -0.000159354, DZ: -0.00506048, Magnitude: 0.00506877
Current Result Value: 5.068766307e-003 mm
I would like to know the XYZ coordinatey more accurate, so in a form like this:
Node # 9 ( X = 508.198XXXXX, Y = 110.16YYYYYY, Z = -4052.31ZZZZZZ )
Is it possible to change this accuracy?
Im don't know how to do it in the results environment, but if what you want is the undisplaced node locations, then you can find a more precise value in the FEA Editor environment. Go to Tools>Options>Application Options>FEA Editor and change the Decimal value to somthing larger. In the FEA Editor, select the vertex that you want to know its location, right-click and inquire. Keep in mind that node number and vertex number are not the same.