One very necessary part of the FEA process is cleaning up geometry so it can be meshed. Many times, we get CAD files that our pre-processor can’t read in properly or needs to be simplified to make a good mesh. In this blog, we will be going over some tricks to help go from a mess to a mesh! Terminology used here corresponds to Abaqus CAE. Stay tuned for a similar blog covering geometry cleanup within the 3DEXPERIENCE platform.
Mesh-Geometry Associativity
Abaqus CAE has associativity between the geometry and the mesh, meaning that the mesh is dependent on the geometry. The main benefit of this is that if the geometry changes, the part can be easily re-meshed; however, that also means having good geometry is very important. I’ve ordered these tricks in the approximate order in which I would try these if I were doing a full geometry cleanup from scratch.
Direct Nodal Connections
Connecting parts directly is a great way to reduce the number of connections needed in the model, if possible. In Abaqus CAE, this is done by merging part instances together. This combining of the part instances should be done early in the geometry cleanup process. In the below example, two tubes are assembled as separate parts. We can use the merge instances command to merge them into a single part.
The merge instances command can also be found in Instance > Merge/Cut.
Part Mirroring
If the part that needs to be cleaned up is symmetric, using the ‘Create Mirror’ tool can cut the amount of geometry cleanup that needs to be done in half. Therefore, I recommend doing this before any other cleanup operations if part mirroring is applicable. In the example below, a pallet is partitioned into a quarter model, then is simplified and mirrored back into a full model.
One thing to note when using part mirroring is that virtual topology operations will NOT be mirrored using this approach. The mirror command can also be found in Shape > Transform > Mirror.
Replace Faces
This tool is the bread and butter of all the geometry editing tools. It can be found in the part module or it can be accessed via Tools > Geometry Edit > Face > Replace. The real usefulness of this tool is removing fillets and small bumps in the model by checking the “extend neighboring faces” option.
If Something Is Really Stubborn
In the below example, we want to remove a fillet from this part. Normally this is an easy operation using replace faces, but wait! The faces on either side of this fillet are parallel and therefore, cannot be extended. Do not fear – we can use the create solid and create cut tools to help!
Create Solid: Creates solid features. Options to create solids include extrusions, revolutions, lofts, sweeps, and shell faces.
Create Cut: Removes material from a part. Options to create cuts include extrusions, revolutions, lofts, sweeps, and circular holes.
For our example, we’ll use the ‘Create solid: extrude’ feature to remove the fillet.
These are the main tools to use if you need to create a part from scratch as well. The solid and cut commands can also be found in the Shape menu while in the part module.
Working With Midsurface Models
Midsurfacing is a great way to simplify long and thin parts, allowing them to be modeled using shell elements instead of solids. To start, a midsurface region must be assigned – doing this changes the solid model to a reference representation (Tools > Midsurface > Assign).
From here, there are a few tools to use to help generate the midsurface:
Offset Faces (Tools > Geometry Edit > Face > Offset): Creates new faces at an offset distance from an original set of faces. This can be done manually using an offset distance, or a set of target faces can be used to compute the distance. This is the main tool used for midsurfacing.
Extend Faces (Tools > Geometry Edit > Face > Extend): Extends existing faces. This can be done manually using a set distance, or a set of target faces can be used to compute the distance. This is good for intersections between shell corners.
Blend Faces (Tools > Geometry Edit > Face > Blend): Closes the space between two sets of connected edges with new faces. This can be done through a shortest path, tangent path, or a specified path.
PARTITIONING IS YOUR FRIEND
Ever needed to make a load patch? Ever had to mesh around a hole? Partitioning is the way to do that! I recommend doing partitioning once you’ve finished all other geometry operations. Taking the time to make good partitions makes a world of difference in the mesh quality. The partitioning commands can be used in almost any module (Tools > Partition).
A good rule of thumb when partitioning is to try to make as many rectangular shapes as possible. See the below example for the way I like to partition around holes – the washer zones give a perfect surface for preloaded bolts (see level 3 in this previous blog post) and the cross design allows all the surrounding areas to be map meshed.
Virtual Topology
Once you’re in the mesh module in Abaqus, virtual topology can be used to determine which features to mesh and which ones to ignore. This is not the same as editing the geometry – if the part is exported, all the virtual topology will be ignored. The main emphasis of virtual topology is to relax the need for the mesh to conform to every edge and vertex in a part and allows you to obtain a simpler model with less detail. There are five main modules in the virtual topology toolset:
Combine Faces: Allows you to combine faces, treating them as a single face and ignoring any boundary edges and vertices between them.
Combine Edges: Allows you to combine edges, treating them as a single edge and ignoring any vertices between them.
Ignore Entities: Allows you to remove selected edges and vertices from the assembly.
Automatically Create: Allows you to set parameters that Abaqus will use to create the virtual topology.
Restore Entities: Allows you to reactivate entities that were previously ignored.
All of the virtual topology tools can be found in the mesh module. The virtual topology toolset can also be accessed by going to Tools > Virtual Topology.
Some downsides to using virtual topology is that instances containing it can no longer be merged or cut from each other. Some part features, such as the create mirror feature, also will ignore virtual topology. However, it is a very powerful feature that can clean up geometry that can’t be cleaned up using the geometry editing tools discussed earlier in this blog.
Take a look at two different meshes of this video game controller – one with virtual topology, and one without. As you can see, the mesh with virtual topology still follows the shape of the geometry but does not force nodes to be on every edge, creating a better overall mesh.
Some Other Useful Tools
Repair Small Faces (Tools > Geometry Edit > Face > Repair Small): Removes small faces and repairs the adjoining edges and faces to create a closed geometry.
Repair Small Edges (Tools > Geometry Edit > Edge > Repair Small): Removes small edges and repairs the adjoining edges and faces to create a closed geometry.
Merge Edges (Tools > Geometry Edit > Edge > Merge): Merges edges into a single edge, removing redundant vertices and edges. This works very similarly to the combine edges function in virtual topology.
Remove Redundant Entities (Tools > Geometry Edit > Edge > Repair Redundant Entities): Removes redundant vertices and edges from a selected region. This works very similarly to the ignore entities function in virtual topology.
If All Else Fails: The Nuclear Option
If no other geometry cleanup strategy works, you can always delete the problem faces, clean up the edge geometry, and then use the cover edges tool to make a newer, simpler face. Doing this will create shell geometry, so you will have to use the solid-from-shell tool to convert the part back to a solid.
Remove Face (Tools > Geometry Edit > Face > Remove): Removes faces in the part.
Cover Edges (Tools > Geometry Edit > Face > Cover Edges): Creates a face using a selected group of edges. The selected edges must form a closed loop.
Convert to Precise (Tools > Geometry Edit > Part > Convert to Precise): Abaqus CAE tries to change neighboring entities so that their geometry matches exactly. Imprecise parts use a looser tolerance to create a closed volume than the precision used by Abaqus CAE.
Create Solid from Shell (Shape > Solid > From Shell): Creates a solid feature from a three-dimensional shell part by selecting the faces that will form a closed part.
In the workflow below, I use this method to clean up a particularly difficult part.
For this particular example, the replace faces operation created the solid body automatically, meaning I didn’t have to use the create solid from shell tool. However, I would always double check to make sure. After all, every geometry cleanup is a slightly different problem!
Query (Tools > Query): Gives options to obtain information about the model. By going to the geometry diagnostics in the query window, you can check various information about the geometry, including whether it is a solid or shell.
Final Thoughts
Abaqus CAE has many tools available to help simplify geometry, turning a mess into a mesh! Of course, everything we’ve shown here in this blog is not exhaustive.
Feel free to let us know your favorite geometry cleanup tool (or have us help clean up your own geometry) by getting in touch with us today!
