Manipulating Geometry and Meshing in FEMAP
This tutorial demonstrates how quickly FEMAP can modify geometry and create finite element models using the Meshing Toolbox, and Mid-surfacing and Non-Manifold Add tools
Tutorial Overview
This demonstration will show how quickly FEMAP can modify geometry and create a finite element model.
We will walk step-by-step through the process of importing and modifying geometry in order to create a finite element model from that geometry. To help us do that, we will be using the Mid-surfacing and Non-manifold Add Tools.
In this article:
- Importing CAD Geometry
- Geometry Manipulation
- Midsurfacing
- Correcting Free Edges
- Creating Meshing Surfaces
- Final Steps and Conclusion
Importing CAD Geometry
The first thing to do is import the CAD geometry. To do that, go to File > Import > Geometry and then select the geometry file you want to import.
File>Import>Geometry:
Scale factor is 39.97 to convert meters to inches
Set the geometry scale factor to 39.37 because the geometry is in meters and we want our graphic to come in inches.
Measure the first geometry imported into FEMAP to verify that the scale factor was set properly
The imported geometry comes into the active layer.
Isolate the geometry that will be using for meshing (in this case, the grey solid). To do so, create a new layer that the geometry will go into. (We named ours “Bracket Solid”)
Then place the solid into that layer (Modify>Layer>Solid):
Select “Show Selected Only” to isolate the geometry we’re looking for.
Geometry Manipulation
The next thing to do is prepare the geometry for mid-surfacing. As you can see, it has fillets, holes, and other things that we don’t want to model.
Removing Holes
First remove the small holes around the larger holes. They are not necessary to represent the structure.
Move to the loops command. To remove the holes, just select any curve on the circle.
Note how all small holes are removed!
Removing Fillets
Next remove the fillets. The fillets are going to cause issues with the mid-surfacing tool.
Go to Feature Removal > Surfaces.
To remove fillets properly, you have to select all the surfaces in a loop. Otherwise you could run into errors with the geometry modification.
Continue to select all the surfaces in one continuous loop. If you want to check the surfaces that you have selected, you can highlight it; showing clearly the surfaces you have selected.
Click OK and it will remove all those surfaces, leaving nice sharp corners. Repeat this step to remove all unnecessary fillets.
Now that all the fillets in the model are removed, we are ready to start mid-surfacing.
Midsurfacing
Create a new layer to put the surfaces into (we named ours Bracket Midsurfaces) and turn the layer on.
Next perform the mid-surfacing command by going to Geometry > Mid-surface > Automatic. Select all the surfaces on the bracket.
To determine the target thickness, you can measure the thickness of the bracket. Since most of the thicknesses on the bracket are similar, we just measured one area and selected a target thickness of 0.2 inches.
Select “Combine Midsurfaces” so that it will combine all the surfaces it creates into one solid, allowing us to avoid any coincidental curves.
Now that the surfaces have successfully been created, they can be viewed by turning off the Bracket Solid layer, leaving the 2D surfaces that were created.
Checking Free Edges
Check the free edges on these surfaces just to make sure that it performed correctly. To do that, go to the Meshing Toolbox. Turn on the “Toggle Entity Locator” and select Free Edges.
As you can see it created some free edges where we don’t want them.
Zoom in to see what the mid-surfacer did. As you can see, it created a sliver surface that we’re going to want to get rid of, and messed up the end of the foot. We’re going to get rid of those surfaces and recreate them.
Correcting Free Edges
First select and delete those surfaces.
Now recreate those surfaces by going to Geometry > Surface > Corners.
Select the corners of the surfaces you want to create.
Next add the circles back by projecting them onto the surface.
First project the curves from the solid onto the surface. To do that go to Geometry > Curve – From Surface > Project and select the surface. Then select the curves you want to project onto that surface.
We also want to do that to the bottom to create our property regions for the bottom surface. Redo the command Geometry > Curve – From Surface > Project. Now the circles on that surface can be deleted.
Now that the surfaces have been created, add them to the solid of the rest of the bracket.
To do that, use the non-manifold add command. Geometry > Surface > Non-manifold add.
Select the surfaces. When you perform this command it will display the free edges, showing that we no longer have the unwanted free edges.
Creating Meshing Surfaces
Breaking Up the Surfaces
Now we’re ready to start breaking these surfaces into meshing surfaces. Go to the Geometry Editing tab under the Meshing Toolbox. We will start at the feet.
Meshing around a hole can prove challenging. One of the geometry meshing tools that makes this easy is the Pad command.
Using the “select”, select a curve on any circle and it will create a pad around that circle that will create a math-mesh, creating a nice circle. Repeat the pad command on all of the feet.
Continue breaking up the surfaces into meshing surfaces by using to the point-to-edge command. This is good for creating more rectangular surfaces, which are good for meshing. It can then be broken up further by using the point-to-point command.
Determining where you want to break up surfaces will come from experience and trail-and-error.
Meshing
Now that the surfaces have been broken up, we’re ready to start meshing. The bottom has a variable thickness so we will create multiple property regions with varying thicknesses.
First create the material and property regions. Create a new material and load one in from the FEMAP presets. (We chose aluminum 7050)
Next create 3 properties. First property with a thickness of 0.2 inches, second property with a thickness of .375 inches, and the third property region with a thickness of .225 inches.
To begin meshing, go to the meshing toolbox and select the mesh surface command. From here we can select the property we want to start meshing with (the 0.2 inches property).
Set the mesh size to 0.2 inches. Select Mapped Mesh and choose the Auto Mapped Approach. Use the select tool to select the surfaces to mesh.
If the mesh does not show up, it is likely because it switched over to a wrong layer. To fix this go to Modify > Layer > Mesh, selecting the mesh on that surface and picking the mid-surfacing layer.
To avoid this later, activate the desired layer by double clicking on its title - any new entities created will be assigned to the active layer.
When meshing the bottom, the outside ring has the thicker property so switch to the second property (Bracket t=0.375″).
On the inside, we don’t want to size any of those, so we turn mesh sizing off and change property over to the last option (Bracket t=0.225″).
Final Steps
As you can see, all the mesh looks the same, so how can you tell where your property regions are? We can select coloring elements with property colors as opposed to element coloring (use F6 View Options).
Then, to change the property colors, go to Modify > Color > Property > Select All > Random
Once the colors have been randomized, turning off the filled edges, nodes, and surfaces allows you to see the property regions that were created.
Lastly check the free edges to make sure there are no unwanted free edges. And we can see, there are no unwanted free edges.
And just like that we have our finished mesh of the bracket!
Conclusion
As you have seen from this demonstration, FEMAP can quickly create meshes of your objects, and also provides the tools you need to deal with any troublesome geometry.
Related Articles
Manipulating Geometry and Meshing in Femap
What is in this webinar? This webinar will give an introduction to the capabilities that Femap has in creating finite element models. We will walk through a step by step process of importing geometry into Femap and creating a finite element model of ...Meshing Toolbox in FEMAP
Quickly and interactively edit geometry and create quality mesh using the Femap Meshing Toolbox The Meshing Toolbox is a centralized collection of FEMAP's geometry clean-up and meshing functionalities in a single pane. Below you will find an overview ...The Meshing Toolbox
10 Tools to Quickly Create and Refine Accurate Finite Element Models This deep-dive into the meshing toolbox will showcase tools that will help you edit geometry and create accurate meshes from the associated geometry. This webinar will explore all ...An Analyst’s Guide to Resolving Common Geometry Problems
What is in this webinar? In this webinar, we will walk through some helpful tips, tricks and strategies that can help mitigate some common geometry problems faced by an analyst. Topics will include: Refining a thin-walled solid wing box structure ...Part 4 - Meshing and Analysis Preparation
Introduction Welcome to the introduction to FEMAP video series. In the previous video we set up the material and element properties on the machined arm components and defined loads and boundary conditions. In this video we will continue the ...