Side Door plastic component Meshing using Hypermesh  

Side Door plastic component Meshing using Hypermesh

Objective :-

To perform Geometry cleanup and Meshing on Car side door panel which is a Plastic Component. Also apply thickness , assign property and check the normals.

Procedure :-

STEP 1 :- Component Study

1. Its a car's inner side door panel.

2. The given component is a plastic component. So it will be having varying thickness.

3. The main part of the component is of 2.8 thickness.

4. The rest part is consisting of many ribs and features.

5. Ribs are given to increase the strength of the component.

6. There is also a circular part where the speakers will be placed.

7. While going through the parent geometry we can see that there are many deformations formed while importing the geometry to hypermesh.

STEP 2:- Geometry Cleanup.

1. After importing the model we can Check for deformation.

2. The parent have deformations as shown below.

In some places you can see some gaps like these.

a) We can easily fix this by using Filler Surface.

b) Go to Quick Edit in Geometry.

c) Use Filler Surf tool click on the boundary of the gap. Then you can see the gap is filled and the boundary of the gap will be toggled.

In some regions we can see that instead of a regular pattern there will be irregular shapes.

a) This can be fixed by replacing the points at the end of the deformations.

b) Go to Quick edit.

c) Use option replace points , click on point and then click on the point to be replaced.

d) Then click on retain and click on the point to which the 1st selected point is to be replaced.

e) Like that replace the points suitably to get a good geometry.

While taking the Ribs we can see that all the ribs are having fillets at there edges. When taking the midsurface of these Ribs it will be a problem.

a) So for a better mid surface creation we will defeature the surface fillets in the Ribs.

b) For this we use the tool Defeature in geometry.

c) In Defeature use Surface Fillets option.

d) Use second option in that which is "Find Fillets in selected" under that choose surface.

e) Give Minumum and maximum radius, fillets in between this range will be deleted.

f) Click on Find.

g) This the Hypermesh will show us the surface fillets between that range.

h) From that we can choose the surface to be deleted under " fillets to remove"

i) Also under that we can see an option "ignore edge association" which will help use to deselect some edges which was automatically selected by hypermesh which we really needed.

j) Then click on remove so that we can remove the fillets and will get a good sharp edged ribs

But in some cases the defeturing cannot be used. Like even if we use the defeature , the defeatureing will not be proper. Like below

• In this case we can use a combination of tools.
• First measure the length of the remaining area to be defeatrued. Using Distance tool
• Then delete the whole fillet and the area which we want to defeature. Using Delete surface in Quick edit.
• Drag the boundary to the length which we have measured first. Using Geometry>Surface>Drag along vector.
• In that option choose lines and select the lines which we want to extend.
• Chose the vectors N1 and N2 to show direction of the drag.
• Give the distance and click on drag+
• After drag we can see some gaps on the ribs, these can be fixed using Filler Surface in the quick edit.

Here we can see that the parts are slipped away a littile bit.

a) We can solve this by deleting the slipped away surface and rebuilding a new surface connecting the too sides.

b) Tools used in this area is Delete Surface to delete the existing surface.

c) Ruled option or drag option to create new surface.

d) Trim with surface to trim the extra surfaces.

STEP 3:- Mid surface generation and its geometry cleanup of mid surface.

A. Auto mid-surface (Just for referance while making manual Mid-surface)

1. There is Auto Midsurface option but we cannot use that in here because it will delete some features that we needed. But we can first create one to know about the shape which our manual mid surface will be almost be looking like.

2.For Auto midsurface go to Geometry>Midsurface

3. Go to extraction options then choose skin offset for better offset

4. Then go back to auto extraction, Select the parent surface body which we want to create auto mid surface. Duplicate it. Then click on extract.

5. After sometime we get the auto midsurface

B. Manual mid surfaceing

1. This component is a plastic component so it will be having varying thickness.

2. So we need to check the thickness of each part seperately.

3. Checking thickness at the edges will be easy but checking thickness at area exept the sides is difficult so we can to one thing.

4 Create temp nodes (Shift+F2) on both sides of a place of the parent surfaces.

5. Then use distantce (f4), Two nodes option to measure, Thus we can measure the thickness of inside areas.

6. After getting thickness we can start manual mid surfaceing. For manual mid surfaceing we will use the Offset in Surace edit option.

7. Geometry>Surface Edit> Offset.

8.In offset option choose continuous offset

9.Then select the surface to be offseted

10.Make duplicate of that surface. Then click on offset.

11. While doing the manual mid-surface we cannot do the whole part in a single stretch. We need to do it part by part. but can almost do parts with same thickness at a single process.

12. We can easily make the mid surface of the mainbody but for ribs it is a bit difficult because of the different shapes on both sides in some ribs

Methods To Generate Midsurface for the Ribs

A. Using midsurface tool

1. Geometry > Midsurface

2. Change Auto midsurface to Final edit tools

3. Choose the two opposite sides of the ribs. In slide1 and slide2.

4. Choose Result in Middle Surface Component.

5.Click on extract.

Parent rib> Midsurface of the rib

B. Using middle line tool

1. First draw a middle line by using the edges of the parent rib.

2.Geometry > lines> Midlines.

3. Select one edge line on one line list and other edge line on other line list.

4. Click on create.

5. After Making the line we can project it to the below main midsurface.

6. To project the line to the midsurface by Tools> Project>To surface

7. Select the lines to project in Lines

8. Select the surface to which the lines should be projected in To surface

9. Select the direction in Along vector.

10. Click on Project.

11. Now we have 2 lines for a rib, above and below. Now we can make the mid surface of the rib by making a surface in between using the tool Ruled.

12. Geometry> Surface > Ruled

13. In the 1st line list Select the first set of lines and in second box choose second set of lines.

14. Click on create.

C. Using Offset option

1. This option can be used where the ribs are of equal thickness.

2. Measure the thickness of the rib first.

3. Then go to Geometry> surface edit > Offset.

4. Select the surface to be offseted.

5. Right click on surfaces option and make duplicate.

6.Give half the thickness of the rib in offest box.

7.Click on vector normal to know the direction. If want to reverse click on reverse normal.

8.Click on offset.

Cleaning up of the mid surface

1. Small gaps and unnecessary hole can be filled using Filler surface tool in quick edit

2. Small deformations can be made good using Replace points in quick edit

3. Lines which will be failing for minimum length error can be eliminated using toggle edge in quick edit.

4. Proper connection shall be established between lines.

STEP 4:- Setting up Quality criteria

1. For setting up the criterias as given the project we need to go to Criteria editor.

2. For that go to Preferences> Criteria file settings

3. In that tick in the boxes near which all the criteria we wanted and give the values for each criteria.

4. Save the Criteria file so that we dont need to enter it each time.

5. Click on Apply

6. Click on Ok.

STEP 5:- Meshing

1. After setting up the Quality criteria we can start the meshing process.

2. 2D> Automesh.

3.After clicking on the surface box Select the surfaces needed to be meshed.

4.Give element size as 4 as in the question

5. Give the mesh type as Mixed.

6. Elements to surface component is choosen to add the mesh to the surface component

7. Keep connectivity is given to keep the mesh connectivity

8. Check the Align and size to get a good mesh flow.

9. Click on mesh.

10. We can change the surface to elements and select the elements we want to remesh and click on Mesh to remesh the elements

11. The mesh we get will have a huge number of trias, fixed trias and rotational quads. also the mesh flow wont be in a good pattern.

12. Inorder to make it a good mesh. We will reduce the number of trias ( removing the unwanted trias)

13. This can be achived be going to 2D> Quality Index> Cleanup tools.

14. We can remove trias and get good mesh flow by using the cleanup tools

• Main points to remember in Tria management:-

1. No trias in corner or edges.
2. No opposite trias.
3. No back to back trias.
4. No trias at hemmings or fillets or keep it miimal as lower as possible
5. No rotational quads.
6. No trias should share a boundary with feature line.
7. Connectivity between elements
8. Split and perform the mesh.
9. Use mixed type mesh for irregular surfaces and quad type only for rectangular and square surfaces.

• The main tools used while eleminating trias are in 2D>quality index>cleanup tools

• Place node :- Used to manually move a node
• Smooth :- used to smooth the elements to get better mesh flow
• swap edge:- to swap the sides of the element
• Node optimize:- place the node in an optimize position which try to reduce the errors
• Element optimize:- optimize the element sides to eliminate errors.
• Split/Collapse edges:- used to split the elements.
• Drag tria elements :- to move the trias in the mesh.
• Split quad elements:- to split quad elements
• combine tria elements :- used to combine tria elements

Other than this there are:-

smooth> Shift+f12:- used to smooth the mesh to get a good mesh flow

project> Shift + f7:- to align the lines with features

Translate> Shift+f4:- to move nodes to eliminate errors.

STEP 6:- Connections

1.If there is more parts and no connections between them we should establish connection between then.

2.Inorder to do that we should go to 2D> Connectors > Spot (we are useing spot connection, so selected spot)

3. In location select the nodes where you want to get the connection

4.In connect what select the components which all that we want to connect.

5.Choose elements because we are giving connections to elements.

6.In num layers give number of layers that we want to connect.

7.In tolerence give the distance between the components which we are going to connect.

8. Select the type of spot connection we want to give.

9. Click on Create.

STEP 7:- Checking the Normals and Free Edges

A. To check Normals

1. To check the Normals go to Tool > Normals

2. Choose elements

3. Select displayed 2d elements for selecting the whole elemets

4. Color display inorder for the color representation.

5. Click on Display.

6. Then we can see the whole model in Blues and reds. If the whole positive side is in one color and the negative side is in one color. Then it is ok.

7. If one side is having both colors then we need to change its normals.

8. By clicking on adjest almost all of it will be corrected.

9. But if not we need to change that by Changeing the Displayed 2D elements to Elements and select the elements which we want to change.

10. Then click on reverse. to change the normals.

B. To check Free Edges

1. For checking normal we need to go to Tool> Edges

2. Choose Elements> the select the whole elements.

3.Click on Find edges.

4. Now Hide other parts and Make edges mesh only visible.

5. Now check if there is red line on any area which is not a boundary.

STEP 8:- Assigning thickness

1. After the whole meshing is done we can assigin thickness to the mesh inorder to make the 2d mesh exact as the real product.

2. First step for assigining thickness is to move parts with same thickness to the same component.

3. To create a component . Right click on the Model view area> Create > component.

4. Now rename the component with Thickness value for easy workflow.

5. Move the parts to its assigned components based on the thickness.

6. Tools> Organise> Collectors.

7. Select elements and choose elements that we want to move.

8. In destination component choose the component to where we want to move these elements.

9. Click on move.

10. After making the whole components, we need to make the properties for each thickness.

11. To make property. Right click on Model view area > Create> Property.

12. Rename the property with the thickness value.

13. Also set the thickness of the property. By clicking on property we can see its details below.

14 In that we can see a T which represents the thickness give the thickness value . Click on enter.

15. To Apply the property to the Components. Right click on component

16. Select assign. Choose the property of the component from the pop up dialogue box

17. Click on Apply. Click on Ok.

18. To see the mesh in 3D. Choose the 2D detailed element representsation.

Result:-

Finished the Mid surfacing and Meshing of the side door plastic component with no fail of quality criteria and tria percentage is .75. Also checked the normal and free edge and applied the thickness to the components.