XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''"> Checking the Finite Element Model
There is rarely such a thing as a perfect finite element model, beyond trivial cases such as single-element test problems. Every finite element model is an approximation to a model's behavior. One of the reasons for this is that elements can vary in accuracy depending upon how they are used. In addition, it is important to verify the correctness of your finite element model, and test for problems such as duplicate elements or unconnected (un- equivalenced) groups of elements.
Patran provides numerous verification capabilities to check the quality of your finite element model. It is a good idea to run finite element verification tests on a regular basis, both to check the potential accuracy of your model, and to get an idea of the overall quality of your finite element mesh. Several of the tests provided are described in the following subsections.
To verify a finite element model:
1. Select the Verify action on the Finite Elements application form.
2. Select the corresponding Object and Method for checking an aspect of your finite element mesh.
Element Shape Tests
• Aspect measures the maximum dimension ratio of opposing edges, faces or principal directions in surface or solid elements. For example, in a Quad element, the aspect ratio represents the ratio of length to width. Normally, finite elements provide more accurate answers when the aspect ratio is closest to 1.
• Warp measures the degree to which a Quad element's corner points are out of plane from the centroidal plane of the element.
• Skew measures angular deviation from a rectangular shape in surface elements.
• Taper measures geometric deviation from a rectangular shape in Quad elements.
• Edge Angle measures the maximum deviation angle between adjacent faces of a solid element.
• Face Warp, Face Skew, Face Taper measures warp, skew, and taper, as described above, for faces of a solid element.
• Twist measures the maximum twist between opposing solid element faces in Wedge and Hex elements.
Other Element Tests
• Boundaries test for free element edges with no adjacent connected element. This is an important test to check for unequivalenced portions of your model.
• Duplicates detect multiple elements connected to the same nodes.
• For shell elements, Normals check for consistent normals between adjacent elements.
• Jacobian Ratio, Jacobian Zero tests based on the maximum variation and minimum value of the Jacobian determinants of each element, respectively.
• IDs color code the elements based on their ID numbers. This is a useful test for visual verification of element number ranges and order of modeling.
Other checks include midside node offsets for higher order elements, superelement boundaries, and a contour line plot based on nodal ID values.
For many of these verification tests, you can set a tolerance value to specify the value or percentage that elements cannot exceed. Then in most cases, a color-coded element display is produced showing the results of the verification test. Elements failing your tolerance are displayed in the highest spectrum color (generally red). Other elements are color-coded to spectral values to show how close they are to
your tolerance.
The proper settings for this tolerance value become a matter of experience with particular element types. For example, a linear triangle element may be very sensitive to distortion, while a quadratic-order triangle element may give good results with even a fairly high degree of distortion. While using a conservative value may help you improve the quality of your finite element mesh, it may also lead to more human engineering time in modifying this mesh for better verification results.
Options When Tests Fail
When elements fail your verification tests, your options include the following:
Remesh the Model
Replacing the existing mesh with a better one is frequently a good way to conserve time, particularly when these new meshes do not substantially alter the analysis run time. In a case where some elements have excessive aspect ratios, for example, re-meshing with a higher mesh density in the long direction may quickly resolve this problem.
Particularly in cases where you have created a finite element mesh from a geometry model, it is easy and straightforward to re-create the meshes for individual regions.
To remesh a model:
1. Delete the original mesh by selecting Delete/Mesh on the Finite Elements application form.
2. Re-create the mesh by selecting from the Create/Mesh family of options described above.
Repair Individual Elements
For some verification tests involving Quad elements, Patran provides automated features to repair elements that are out of tolerance. For example, when Quad elements fail the aspect ratio check, there is an option to automatically divide them into smaller elements at their corner points.
Alternatively, you can directly perform operations to create and modify your finite element model. For a brief description on creating your own nodes and elements for a finite element model, see
Direct Finite Element Modeling. Other options here include selecting the Modify action on the Finite Elements application form, which supports operations such as smoothing the mesh, editing element and node data, or splitting existing elements into smaller ones.
Check your Tolerance
Patran does not force changes to be made to your model based on the results of verification tests. These results are intended as guidelines for you, to help you make better analysis modeling decisions. Therefore, you may decide to increase your tolerance value when you are using higher-order elements, or when elements that have failed your verification tests are located in less-critical areas of your model.
In general, finite element verification tests should become a routine part of your process of finite element modeling. The complexity of many finite element meshes, combined with the limits of visualizing these models graphically, means that you cannot always see problems in your model. For example, duplicate elements often look identical to single elements, and a badly distorted element may not be visible within a dense, complex mesh of a critical region.
By using Patran's automated verification capabilities and applying your own engineering judgment to the results, you add an extra measure of reliability to your analysis work.
