Map Mid-Mesh Thickness Tool

The mid-mesh and solid can be specified by selecting entities in the HyperMesh session interactively, or optionally, external geometry or FE solver decks can also be selected as input.

FE and Geometry displayed
Traditional Element Visualization

Thickness Output:

1. Nodes – The thickness will be assigned on node cards. Option available only for Abaqus user profile.
2. Element – A single thickness will be assigned on element card. Option available only for RADIOSS, Abaqus, LS-DYNA, PAM-CRASH2G user profiles.
3. Nodal Thickness on Elements – Multiple thicknesses will be assigned on elements for each node. Option available for OptiStruct, LS-DYNA, Nastran user profiles.
4. Properties on Elements – Properties will be created for groups of elements, and a thickness will be assigned per property. Option available for OptiStruct, Nastran, Abaqus user profiles.
5. Properties on Components - Creates components and properties for groups of elements, assigns a thickness to each property, and then assigns the property to a component. Option available for LS-DYNA user profile.
6. Select Card Image - Assigns a thickness on INISHE entities, when you select one from the list: SHELL, EPESP_F, STRA_F, and STRS_F. Option available for RADIOSS user profile.
7. Thickness on Components - Assign thickness on PART (SHELL, TSHELL, and MEMBR). Option available for PAMCRASH-2G user profile.
8. Contact Thickness for Components - Assigns contact thickness to TCONT on PART (SHELL, TSHELL, and MEMBR). Option available for PAMCRASH2G user profile.

Minimum Thickness: (Optional)
Any calculated thickness below the specified value will be reset to the specified minimum value.

Maximum Thickness: (Optional)
Any calculated thickness above the specified value will be reset to the specified maximum value.

Assign offset to elements/sections:
If set, the offset value will be assigned on the element cards.

Note that the mesh deviates from the geometry; the mid-mesh node is equidistant from mesh corners, but not from the nodes on the geometry corners.
- 3D Element Visualization is active
- No Element Offset is active

Here, the offset has caused the mesh to match the geometry, though the initial mid-mesh node remains unchanged.
- 3D Element Visualization is active
- An Element Offset is active

Assign average thickness to element groups:
This option is available when the thickness output option is Elements. By setting this option, the thickness values on individual elements will be approximated to be an average value representing a group of elements.

Maximum Thickness Range Interval:
Controls the number of thickness properties or groups. Enabling this option ensures that no thickness group or property will have a thickness interval range greater than the specified value. In other words it is the maximum limit on the max thickness – min thickness in a thickness group or property.
Selecting Abs (absolute) groups thicknesses in the given intervals; selecting Rel (relative) calculates the absolute thickness interval value by multiplying the given value with the average thickness of the group (that is, the given value is the ratio of the interval value to the average thickness of the group).
Only available when thickness output is Properties on elements or when Assign average thickness to element groups is selected.

Fixed interval with start thickness
Controls thickness properties at constant intervals.
Enter a desired thickness value in the start thickness field, and a thickness interval value in the Interval field. All elements will be grouped into properties/components with fixed increments to the thickness specified by the interval value, beginning with the start thickness value.

Truncate thickness to range interval
Rounds the thickness values up or down to have the same number of decimal digits as the input value in the Maximum thickness range interval field.
Only available when Maximum Thickness Range Interval is selected.

Save log file:
The information logged during the computation can be directed the supplied file.

Clicking the Calculate Thickness button will begin the operation, the thickness will be computed and assigned on the mid-mesh.

Correction Method:
On elements or nodes where the thickness could not be computed correctly, there are different options to correct it:

• Interpolate from Neighbors: An appropriate thickness value is interpolated from the neighboring element/node thickness.
• Adjust to min/max values: If either minimum or maximum thickness is defined it is assigned on the corrected elements.

Scaling at corners:

This option is available only when the Correction method is set to Interpolate from Neighbors. When interpolating thickness values near t-junctions or corners, a scaling algorithm is applied:
Supplying a value less than 1 will result in linear decrease in the thickness values nearer to the junctions / corners.
A value of zero will result in an approximate mass-conserved thickness estimation.

Scaling at corners = 0
Thickness Contour Applied
Traditional Element Visualization

Scaling at corners = 0
Thickness Contour Applied
3D Element Representation

If this is equal to 1, the thickness is extrapolated / interpolated without any scaling.

Scaling at corners = 1
Thickness Contour Applied
Traditional Element Visualization

Scaling at corners = 1
Thickness Contour Applied
3D Element Representation

If this is greater than 1, the thickness will increase as you go closer to the junction.

Max Midmesh/Solid Angle (0.1,90)
Defines the cut-off angle in degrees.
Enter the maximum angle (0 to 90) that the mid-mesh makes with the solid, beyond which the estimated thickness will be ignored and corrected.
For example, the images below show the midmesh in blue, and the solid in black. In the first image the midmesh and the solid form a moderate angle. However in the second image the midmesh and the solid form a larger angle. It is possible that this area is a junction, located at the solid edge, or the solid may contain some noisy features, therefore you may want to ignore the calculated thickness and interpolate that value from surroundings.

Max thickness gradient (0, 10)
Measures the change in adjacent thickness values, and restricts the gradient.
Enter the maximum change in thickness allowed across two adjacent measurement locations, as a factor of the distance between the locations. Allowable factors range from 0 to 10.
For example, the image below shows a tiny projected boss in an otherwise planar area, which you may want to ignore. Defining the Max thickness gradient specifies the cut-off for the ratio of difference in thickness at two locations to the distance between the two locations. If the ratio is more than the given value, the measured thickness is discarded, and interpolated from its neighbors.

Max relative faceting error
Specify a maximum relative faceting error to use during faceting calculations.
When HyperMesh computes the proximity with a solid, it do not actually compute with the surface geometry. Instead, HyperMesh computes with the tessellated approximation (facets) of the geometry. In case of curved geometry, the facets may not exactly match the geometry, and hence the thickness is computed, causing faceting errors. Specifying the Max relative faceting error enables you to control the accuracy of the tessellation used, as a factor of the estimated thickness. The Max relative faceting error is the ratio of the maximum error of facets to the estimated thickness. If it exceeds this value, facets are further refined to better capture the geometry.

Max search distance
Specify the maximum distance which will be considered for searching solid proximity. This value is also used to restrict the maximum distance from which a good thickness value is considered for correcting an incorrect thickness estimate. You can also used this option to restrict the algorithm from assigning incorrect thicknesses for the mid-mesh that is out of the solid proximity.

Do not assign thickness to Mid-mesh outside solid
When this option is enabled, a thickness will not be assigned to the Mid-mesh outside of the solid.

In the View section, there are several options for visualization:

Element Coloring by thickness:
HyperMesh Element Color mode will be set to By Thickness resulting in contour plot of thickness.

Thickness Contour Applied
3D Element Visualization

3D Element Representation:
The mid-mesh elements will be visualized as 3d with the assigned thickness as depth.

3D Element Visualization

Highlight Corrected Elements:
The elements are highlighted whereby the thickness could not be calculated from solid, and the correction method has been deployed.

3D Element Visualization
Corrected Elements Highlighted