Meshing of Side Door Panel

OBJECTIVE:

• To extract the manual midsurface of the given component and perform geometry clean up.
• To mesh the same by following strict quality criteria while obtaining good mesh flow and low tria percentage.
• Assign thickness to all ribs.

PRE-REQUISITES:

• Finite element method(FEM) is a particular numerical method for solving partial differential equations in two or three space variables.
• To solve a problem, the FEM subdivides a large system into smaller, simpler parts that are called finite elements.
• This is achieved by a particular space discretization in the space dimensions, which is implemented by the construction of a mesh of the object.
• By meshing, we can reduce the number of degrees of freedom from infinite to finite.
• Mathematically, the element thickness specified by the user is assigned half on the element top and half on the bottom side.
• Hence, in order to represent the geometry appropriately, it is important to extract the midsurface and mesh on it.

PROCEDURE:

I) Initial Setup:

• Select Optistruct from the user interface menu.

• Click on Open -> Model -> Select the model.
• The following model is obtained:

• Change the geometry visualization bar to 'By Topo'.
• Upon inspection, we can see that the model is not symmetric and conclude that we have to perform clean up and mesh the surface as a whole.

II) Geometry clean up on the Parent:

• We can observe that the parent component has many defects and deformations.
• If we do not clean it up now, we will not be able to extract a good midsurface and face more problems in the future.
• The following problems we found:

a) Slanted platform on the surface:

i) The following surface was found:

ii) We have to delete the surface on top and bottom to proceed further.

iii) To delete click on Delete -> Surface -> Select the surfaces -> Delete entities.

[Note: Shortcut for Delete tool is F2]

iv) We can fill the surface by clicking on Geom-> Surface -> Ruled -> Select the Line lists -> Create.

v) To recreate the circle we need to create the center node first.

vi) To do so, click on Geom -> Nodes -> Arc center -> Lines -> Select the lines -> Create.

vii) Now we can create a circle by clicking on Geom -> Lines -> Circle center with radius -> Select center node -> Radius= 1.9 -> Select N1,N2 and N3 nodes -> Create.

viii) From the below picture we can see that the circle create is hovering above the surface.

ix) To project it to the surface, click on Tools -> Project -> To surface -> Lines -> Select the line -> Select the surface -> Along vector= Surface normal -> Project.

[Note: Shortcut for Project tool is F7]

x) To trim the line with surface click on, Geom -> Surface edit -> Trim with line -> With lines -> Select the surface -> Select the line -> normal to surface -> Trim.

[Note: Shortcut for Surface Edit tool is Shift +F9]

xi) Delete the surface to create holes by clicking on Delete -> Surface -> Select the surfaces -> Delete entities.

xii) To create the surface between the two circles click on Geom-> Surface -> Ruled -> Select the Line lists -> Create.

b) Rib Defeaturing:

i) To generate a good mesh we can defeature the ribs.

ii) To do so, click on Geom -> Defeature-> Surface Fillets -> Find fillets in selected surfaces -> Select the surfaces -> Min radius = 0.5, Max radius = 6 -> Find -> Remove.

iii) After defeaturing, the rib is shown below:

iv) But sometimes, the ribs do not get defeatured properly as shown below:

v) We need to manually create the surface in this case.

vi) We have to delete the unwanted surfaces first.

vii) To do so, click on Delete -> Surface -> Select the surfaces -> Delete entities.

viii) Draw a line from the end node by clicking on Geom -> Quick Edit -> Split -Surface-line -> Select node and line.

[Note: Shortcut for Quick Edit tool is F11]

ix) To extend the surface along the line click on Geom-> Surface -> Drag along line => Select the line lists that need to be extended -> Select the line along which surface must be extended -> Drag +.

x) Create the missing surface by clicking on Geom-> Surface -> Ruled -> Select the Line lists -> Create.

c) Additional step on the surface:

i) The following image shows an additional step on the surface:

ii) We have to delete all the surfaces using the delete tool.

iii) Create the lower and upper surfaces using Ruled option.

iv) The fixed surfaces look as shown below:

d) Plate Defeaturing:

i) The following image shows a plate that can be defeatured:

ii) We have to delete all the surfaces using the delete tool.

iii) Create the lower and upper surfaces using Ruled option.

iv) Toggle unnecessary lines by clicking on Geom -> Quick Edit -> Toggle edge.

• Now that we cleaned up the parent model we can extract the midsurface.

III) Midsurface Extraction:

• Since the component given is a sheet metal component, we can extract the midsurface and mesh the same.
• Midsurface is used to represent the entire 3-D model and create shell elements in it.
• This decreases the processing time and computational power needed to mesh.

[Note: Shell elements are 2-D representation of 3-D elements]

• There are two ways to extract a midsurface:

i) Auto midsurface

ii) Surface offset(Manual method)

• For this particular model, we will use the manual offset method as it provides good feature capturing.
• To use offset we need to find out the thickness of the model to calculate the offset value.
• Create nodes on either side of the parent model by clicking on Geom-> Nodes -> On Geometry -> Select the surfaces .

• To measure the distance between the two nodes click on Geom-> Distance -> Two Nodes.

• The thickness of the component is 2.8 therefore the offset value is half of it i.e, 1.4.
• To extract the midsurface, click on Geom -> Surface Edit -> Surface Offset -> Continous Offset -> Select The Entire surface -> Offset = 1.4 -> Colour normal(Blue) -> Offset.

[Note: When colour normal is clicked on, blue colour represents offsetting away from the user and orange colour represents offsetting towards the user]

• There are three ways to extract the midsurface of ribs:

a) Surface Offset

b) Final Edit Tools

c) Generate midline and create a surface between them

• Since few ribs have varying thicknesses, the surface offset option is not viable.
• To create rib midsurface, click on Geom -> Midsurface -> Final Edit Tools -> Surface Pair -> Select either sides of the rib -> Extract.

• From the below image we can see that the rib is not connected to the main midsurface.

• We can extend the rib to the midsurface by clicking on Geom -> Surface Edit -> Extend -> Extend over Edges-> By Distance =2 -> Select the lines needed to be extended-> Select the surface -> Extend.

• To trim the two surfaces with each other click on, Geom -> Surface edit -> Trim with Surface/Planes -> Self-intersecting surfaces.

• Draw a line from the end node by clicking on Geom -> Quick Edit -> Split -Surface-line -> Select node and line.

• Delete the unnecessary surface using the delete tool.

• We can also extend the rib to the midsurface by clicking on Geom -> Surface Edit -> Extend -> Extend over Edges-> To surfaces -> Select the lines needed to be extended-> Select the surface -> Extend.

• To create rib midsurface using midline click on Geom -> Lines -> Midline -> Select line lists.

• Project the midline to the midsurface by clicking on Tools -> Project -> To surface -> Lines -> Select the line -> Duplicate -> Select the surface -> Along vector= Surface normal -> Project.

• Create a surface using Ruled option.

• Extend the surface to the midsurface by clicking on Geom -> Surface Edit -> Extend -> Extend over Edges-> To surfaces -> Select the lines needed to be extended-> Select the surface -> Extend.

IV) Meshing:

• Before meshing we have to keep the following things in mind:

a)Always start meshing the complex component first.

b) Start meshing from the surface with the most features or the surface with free edges.

• To mesh a given surface click on 2-D -> Automesh -> Surface -> Select Surface -> Element size= 4 -> Mesh type= Mixed -> Check Align and Size box under Flow -> Mesh.

[Note: Shortcut for Mesh tool is F12]

V) Quality:

• Following quality criteria is of utmost importance in any Industry.
• The quality criteria needed to be followed for this component are listed below:

• Target Element Length = 4

  S.N	Quality Criteria	Definition	Value
  1	Aspect Ratio	The ratio of Maximum length to Minimum length	5
  2	Skewness	The angular measure of element quality with respect to the angles of ideal element types	45
  3	Warping	The angle between two planes on the same element	15
  4	Taper	Angular distortion of a quadrilateral shell element	0.5
  5	Min. Length	Edge of the element with the least length	2
  6	Max. Length	Edge of the element with the highest length	6
  7	Min angle Quad	The lowest angle between any two edges in a quad element	45
  8	Max angle Quad	The highest angle between any two edges in a quad element	135
  9	Min angle Tria	The lowest angle between any two edges in a Tria element	20
  10	Max angle Tria	The highest angle between any two edges in a Tria element	120
  10	Tria %	Number of trias present with respect to Number of quads	10

• To save the above criteria click on Preferences -> Criteria File Setting -> Enter the parameters -> OK

• The following rules must be followed when it comes to tria management:

• i) No trias should be formed on corners or edges(especially free edges).

  ii) No opposite trias should be formed.

  iii) Back to back must not be there.

  iv) Rotational quads must not be formed.

  v) Trias should not share a boundary with the feature line.

  vi) Elements must be properly connected.

• After meshing we can notice that a few elements have not passed the quality criteria.
• The failed criteria and methods used to clear them are discussed below:

a) Minimum Quad Angle:

i) The following image shows an element failing for Minimum Quad Angle:

ii) We can fix this by using smooth.

iii) To do so click on 2-D -> Quality Index -> Cleanup tools -> Select the failing element and the surrounding elements within the feature -> Smooth.

iv) After using smooth, the element has passed for Minimum Quad Angle as shown below:

b) Maximum Quad Angle:

i) The following image shows an element failing for Maximum Quad Angle:

ii) We can fix this by using smooth.

iii) To do so, click on 2-D -> Quality Index -> Cleanup tools -> Select the failing element and the surrounding elements within the feature -> Smooth.

iv) After using smooth, the element has passed for Maximum Quad Angle as shown below:

c) Maximum Size:

i) The following image shows an element failing for Maximum Size:

ii) We can fix this by using smooth.

iii) To do so click on 2-D -> Quality Index -> Cleanup tools -> Select the failing element and the surrounding elements within the feature -> Smooth.

iv) After using smooth, the element has passed for Maximum size as shown below:

d) Minimum Size:

i) The following image shows an element failing for Minimum Size:

ii) We can fix this by using element optimize.

iii) To do so click on 2-D -> Quality Index -> Cleanup tools -> Element Optimize -> Select the failing element and the surrounding elements within the feature.

iv) After using element optimize, the element has passed for minimum size as shown below:

e) Warpage:

i) The following image shows an element failing for Warpage:

ii) We can fix this by using the translate option.

iii) To do so, click on Tool -> Translate -> Select the Node(s) to be moved -> Select N1, N2 and N3 accordingly (based on the direction the node needs to be moved in) -> Magnitude =0.1 -> Translate +/ Translate - .

[Note: Shortcut for Translate tool is Shift +F4]

iv) From the below image we can see that the element passed for warpage by passing it on to the adjacent element.

v) We have to continue the aforementioned process until all the elements have cleared for warpage as shown below:

f) Taper:

i) The following image shows an element failing for Taper:

ii) We have to rotate the nodes in order to get a good mesh around the hole.

iii) To do so, Click on Tool -> Rotate -> Select the nodes needed to move -> Select N1, N2, N3 and B accordingly -> Angle =2 -> Rotate + / Rotate -.

iv) We can see that the element has passed for taper but there are other failing elements as well.

v) We have to remesh them by anchoring the nodes that were just rotated.

vi) To do so, click on 2-D -> Automesh -> Elements -> Select the Elements -> Element size= 4 -> Mesh type= Mixed -> Check Align and Size box under Flow -> Anchor the rotated nodes -> Mesh.

vii) The below image shows the best mesh for that region clearing all quality:

g) Skew:

i) The following image shows an element failing for Skew:

ii) Rather than using clean up tools, we can get a better result if we remesh the elements.

iii) The below image shows the best mesh for that region clearing all quality:

h) High Tria Concentration:

i) The following image shows a region with high tria concentration:

ii) We can obtain a better mesh by using the rebuild mesh tool.

iii) To do so, click on 2-D -> Rebuild mesh -> Select the Elements -> Rebuild.

iv) The below image shows the best mesh for that region having low tria concentration.

i) Bad Mesh Flow:

i) The following image shows a region with bad mesh flow:

ii) We can fix this by using the smooth tool.

iii) To do so, click on, Tool -> Smooth -> Select all the elements -> Iterations = 100 -> Smooth(Until value on status bar reaches 0).

[Note: Shortcut for Smooth tool is Shift +F12]

iii) The below image shows a better mesh flow:

• From the following image, we can see that all the elements are passing for all quality criterias:

• To check the tria percentage click on 2D -> Quality Index -> Page 3.

VI) Assigning Rib Thickness:

• After generating the mesh for the ribs, we need to assign thickness to it.
• To find out the thickness, click on Geom -> Midsurface -> Review Thickness -> Select the rib surface from the Parent Component.

• We need to create a Component and Property to assign the thickness.
• To do so right-click on Model Browser -> Create -> Component/Property -> Ok.

• In the card property bar enter thickness as 3.4.

• Click on Tools -> Organize -> Elements -> Select the elements on the respective Rib -> Select the Component created -> Move.

• Assign the property to the rib component by Right-Clicking on the Component -> Assign -> Select Property -> Apply -> OK.

• Assign thickness to all the ribs using the same procedure.

VI) Connection:

• Since the plate is just hovering over the main component we have to provide a connection between them.

• To do so, click on 1D -> Rigids -> Create -> Select two nodes -> Create.

VI) Equivalence:

• After meshing we need to check for free edges in the mesh.
• To do so, click on Tool -> Edges -> Elements -> All -> Tolerance= 0.5 -> Find free edges.

[Note: Shortcut for Edges tool is Shift +F3]

• From the below image we can see that there was a free edge in the model:

• By turning on the mesh we can see that a few nodes do not have connectivity between them.

• To clear them, click on Tool -> Edges -> Elements -> All -> Tolerance= 0.5 -> Preview Equivalence -> Equivalence.

• Repeat the process to find the free edges again with different tolerances.
• The below image shows the absence of any free edges within the model:

RESULTS:

• Performed geometry cleanup on the parent to get rid of deformations.
• Extracted the midsurface manually and performed cleanup on it as well.
• Obtained a good mesh flow with 0.93% tria percentage.
• Cleared all elements for quality.
• Assigned thickness to all ribs.

CONCLUSION:

• Understood the difference between auto-midsurface and manual midsurface and the reasoning behind choosing manual method for this particular model.
• Learnt different methods to recreate the surface in case of deformation.
• Learnt different tools required to clear all quality criterias.