Currently I'm trying to find the deformation of a complete design through a pressure field.
I made the design in Inventor and imported it in FEMAP as a STEP file (see attachment for design). After that I made boundary surfaces from the circular lines so they can be meshed.
I applied a pressure field on the blade in between using the Between coordinates data surface option.
The problem however, as shown in the 2nd attachment, is that only the blade in between deforms, while the rest of the design stays the same.
I want to be able to see the whole design deform because of the pressures on the blades in between. Does anyone know how I can do this?
I already tried;
- Stitch. Parts are not solid
- Nonmanifold Add. Unable to select round parts since they are no solids
- Convert surface. round parts are no selectable surfaces
Solved! Go to Solution.
The problem is clear for me, not displacements continuity exist between the blade and body, then you simply missed to calculate the intersection & merge nodes or define a GLUE edge-to-surface contact if you prefer working as independent bodies. The above is basic in Finite Element Method, don't let things to solve by the preprocessor, better take your action.
Here you can define a nonmanifold sheet body using command GEOMETRY > SURFACES > NONMANIFOLD-Add, this way FEMAP will create a only-one sheet body to mesh with sell elements assuring merging nodes at the intersected surfaces, assuring displacement continuity between bodies. Make sure surfaces are touching properly, not gap exist (extend midsurfaces till intersection), if not the nonmanifold process will fail.
Or better make sure to have a single solid body (if not use GEOMETRY > SOLID > ADD) and use command GEOMETRY > MIDSURFACE > AUTOMATIC, and use a proper TARGET THICKNESS value, this way FEMAP will create appropiate midsurfaces, extending where necessary, OK?.
I succesfully combined the surfaces using the NonManifold Add option, no free edges were visible between the blades and round plates.
Now, after succesfully adding materials and meshing all parts I created a data table to be able to interpolate the pressures on the blade.
This is where the problem occurs. Because I combined the surfaces earlier, FEMAP doesn't 'see' any more surface for the data table.
Do you know how I can fix this? So I can apply my data table to the blades and hopefully see the whole design deform!
Edit: When I combine the surfaces using Connect, Automatic the same scenario happens. FEMAP is unable to find any surface for my data table..
Things in FEMAP are very easy, you need to understand the philosophy:
Your FEMAP model is almost empty, only four surfaces exist. Post your STEP file better, or revise the version of the FEMAP file.
Next I apply Shell CQUAD4 elements property#1 to the blades and property#2 to the covers using an arbitrary thickness of 2 mm & aluminum material property, as well as mesh size, mesh the surfaces and here you are:
But please note meshes are not connected at all between blades & covers. Then we will use GLUE EDGE-TO-SURFACE to glue elements together during the solution with NX Nastran. Glue is a simple and effective method to join meshes which are dissimilar. It correctly transfers displacement and loads resulting in an accurate strain and stress condition at the interface. The grid points on glued edges and surfaces do not need to be coincident.
A simplistic description of edge-to-surface glue is that the software creates pseudo-faces along the edges in the source region. It then connects these pseudo-faces to the shell or solid faces in the target region with weld like connections. From the glue points on the source side pseudo-face, the software projects a normal in the outward normal direction. In addition, the software searches a small distance in the inward normal direction in order to glue edges and surfaces that may interfere due to meshing irregularities.
You need to define the SOURCE EDGE REGION using command CONNECT > CONNECTION REGION, making sure you select "Defined by = Curves" and "Output = Nodes", then select the edge curve of the blade as shows the following picture (repeat for the rest of edges):
Next lets create the TARGET SURFACE REGION: make sure you select "Defined by = Surfaces" and "Output = Elements", then select all the cover surface. Repeat for the bottom surface.:
Next step is to define the GLUE property using command CONNECT > CONNECTION PROPERTY, simply click in DEFAULTS and you are done!!:
And finally lets define the CONNECTOR PAIR using command CONNECT > CONNECTOR, make sure you select the proper TARGET & SOURCE region!!.
Repeat sistematically to fill all the edge-to-surface glue connectors, define loads & BCs and solve, the result could be more or less like the following picture (I have constrined the inner edge of the botton cover and apply a pressure = 1 MPa in the blades):
1. Thank you for your reply. when I create Boundary Surfaces from Curves, and try to Convert these into a surface I get an error as shown below.
2. When I use Surface > Ruled I get the design as below. Will this work?
3. And when I try to add the Shell elements I get an error saying it is not the correct element. Why can't I just use Plate elements?
4. How come your meshed design doesn't show any lines from the blades, but a clean mesh on the covers?..