Preprocessing (Meshing) car side door panel using Hypermesh by Altair.
Door panels serve as an interface between the interior of the car and the inner workings of the door. They are expected to meet a variety of design specifications regarding safety, aesthetics, and functionality and coverup complex electrical and mechanical components for operating locks, windows, and other features.
Usually Side door panel have: Carrier pocket, bezel, speker grill etc.
There are numerous plastic mterial used in a car and are categorised as:
-Internal parts : door panel, dashboard, glove box, etc
- external parts: Bumpers, mudguards, mirror covers
- in engine compartment: air supply system, oil ducts etc
- other: fuel tanks.
A projection can be defined as anything that adds material onto a part's nominal wall. The reinforcing ribs, snapfit latch, bosses are all projections off of that nominal wall. The design guidelines are the same for all of these shapes. Reinforcing ribs are the most frequently specified when injection molding parts.
Just as bridge beams and columns are supported at their vertex with gussets to add strength to the structure, the same concept applies to plastic injection molding.
Reinforcing Ribs
A standing wall, or a rib, can have many functions, but its primary use is to provide the maximum stiffness at the minimum cost. Thick walls provide more stiffness than thin walls, but thick walls require more plastic material and a longer molding cycle.
Extracting midsurface:
Dealing with midsurface extraction of plastic components can be complex but by analysing model we can choose from multiple options to extract midsurface.
Three automid algorithm hypermesh can perform are:
Offset
offset + plains
offset+ plain+ sewwp
skin offset
manual : Surface edit > offset ; Surface pair.
Here we'll be doing manual offset by measuring thicknes at various parts and then adjusting the mid surface by extending and intersecting.
Procedure:
Step1: Import the .igs geometry file from import solver deck. Change from step to.igs (refer figure 1)
Figure 1 .
Step 2: (Inspect the model ) Switch to BY 2D TOPO from GEOMETRY COLOR MODE, that is in Visualization Tab. As shown below in (refer figure 2)
Figure 2 .
Step 3:For ease for topology repair, we can go to Visualization tool at visualize tab. check and uncheck the visibility of free,shared suppresed edges, t junctions and that makes easy to detect the geometry. as shown below. (refer figure 3)
Step 4: Geometry clean up is the basic step before meshing as it improves the mesh quality. In this Model we have few geometry cleanup to do as shown below
- Figure shows red & yellow lines ( free edges and t junctions which should be green as shared edge)
Go to Geom > quick edit (shortcut : f11). Select Toggle edge and right mouse click on yellow line ( as it will untoggle the whole line ) and again left
mouse click on red line it will toggle it into shred edge ( green line).
Figure 3 .
- Figure show the gap between surfaces. which should not be there.
Go to Geom> edge edit and selecet Replace in tolerance give random value 10 and in moved edge select upper red line in retained edge select lower edge and select replace.
Figure 4 .
- Figure shows duplicate surface as when selected we can see overlapping surface
Go to delete panel ( shortcut : f2) from options select surface and select the over lapping surface and delete the surface. now there will be gap in surface which can be filled by ruled
to crete surface go to Geom> surface and select ruled option and select lines to create surface.
Figure 5 .
- Figure shows the ribs with fillet less than 2 mm which is our minimum element length quality which can fail. so we need to defeture the ribs.
Most of the ribs will be defetured by defeature tool
Go to Geom> defeture and select Surface fillets select find fillets in select surface select the rib surfaces. give minimum and maximum radius between which hypermesh will find the fillet failing for minimu length quality. give minimum as 1 and maximum as 2. hypermesh will highlight the fillets between these values and select remove.
Figure 6 .
For the fillets which do not get get defeatured, go to Surface edit ( shortcut: Shift+ f9) select Trim with lines from first option select surfaces of rib and drag a cut line as shown below
Figure 7 .
Then measure the distance as shown and then go to defature surface fillets and defeature fillets only the end portion doesn't get defeatured.
Figure 8.
Then go to Geom > Surface select the drag anlon vector give the masured distance select the edge lines and give vector direction N1 and N2 and select drag+
At last we can fill the gap by ruled tool in surface panel only.
Figure 9 .
Step 5: Toggle the unwanted lines which can cause minimum element failure when meshing. to togglr go to Geom > quick edit (shortcut : f11). Create cuts in surface to make rectangular surface where ever possible to get a good mesh flow.
Step 6: Moving to Second major step i.e. Midsurfacing.
If not turned on turn on the display fied points options from pannel which makes easy to measure distance from point to point.
check the distance at random points of surfaces. go to Geom > Distance ( shortcut F4) and select two points option.
Now creating midsurface by surface offset option. one is shown below
- Make a new component name it MIdsurface and make it current
- go to Geom > Surface edit (shortcut : shift+f9). select offset option
- Select continuous offeset and give offset value 1.4 as the thickness is 2.8
- Select the surfaces to be offset. from extended entity option select duplicate> current comp and
- Check colour normal if red ( meaning from inwords to outwards) chane it by reverse normal to blue ( meaning from outwards to inwords).
- Select offset. Simillarly do for other parts except ribs.
Figure 10 .
Step 7: Since have a varying thickenss , hence offset won't give good result therefore I extracted midsurface by two ways:
(a) Go to Geom> Misdurface> change from Auto midsurface to final edit tools and select surface pair tool.
select side 1 surface and sie 2 surface and extract.
(b) Go to Geom > Lines and select midline tool
- from linelist one select one line from select line list second option select the other line and select Create.
Figure 11.
- Now Project this midline to the base midsurface from Tool > project and select to surface tool.
- Select lines to be projected.
- Select surface from to surface.
- Keep in surface normal in along vector option.
-Trim the surfaces by the lines we created and projected
- go to Geom> Surface edit ( shortcut: Shift + f9) and select trim with lines tool.
- from second option with lines select surface selece free line and keep normal to surface and trim.
- After triming both the surface go to Geom> Surfaces select ruled tool and create surface using the trimed lines.
Step 8: After extracing midsurface for every surface there might be gap or no connectivity. so to connect the adjacent surfaces use Extend option.
- Go to Geom> Surface edit ( shortcut: Shift + f9) and select Extend tool.
- Keep Extend over edges and by distance give random value as 1.
- Select lines to extend over and extend .
- Do it for both the surfaces.
- Trim the intersecting surfaces go to Geom> Surface edit ( shortcut: Shift + f9) select Trim with Surfs/plane.
- From third option self intersecting surfs select the surfaces and Trim.
- Check for connectivity after trimming and delete the unwanted surfaces.
Figure 12 .
TIP : To cross check the Connectivity of ribs to the base surface or wall we can mask the wall surface opposite to rib and hence the empty surfaces or gaps will denotr the connection as shown below.
But for area where the rib is almost very close to wall we can assume it as connected.
Figure 13 .
Once the Midsurface is created with proper shared edges check again for geometry .
- Toggle the lines that may fail for minimum length.
- Remove the unwanted points on the surface that can lead to element fail.
Midsurface check by colour contrast
Turn on the parent & midsurface, change and give them contrasting colour.
This will help indicate the for any missing midsurface or improper midsurface.
Here in this one can easily identify the orange midline and the orange points of midsurface on the blue parent surface.
Figure 14 .
Step 9: Moving to third major step i.e. Meshing.
So first assig the quality criteria vaslues for the desired mesh.
Go to prefrences > quality criteria from top tab.
Given quality criteria are
Target Element Length = 4mm
| S.N | Quality Criteria | Value |
| 1 | Aspect Ratio | 5 |
| 2 | Skewness | 45 |
| 3 | Warping | 15 |
| 4 | Taper | 0.5 |
| 5 | Min. Length | 2mm |
| 6 | Max. Length | 6mm |
| 7 | Min angle Quad | 45 |
| 8 | Max angle Quad | 135 |
| 9 | Min angle Tria | 20 |
| 10 | Max angle Tria | 120 |
| 11 | Tria % | 10 |
TIP : To check for any unwanted points and lines left that can cause element fail for minimum length. we can give a mesh to whole component in one shot and turn on the quality for minimum length only rest can be resolved.
Once mesh is created go to quality index and select save failed.
- Go to Mask option (shortcut: f5) from options select elements.
- From extended entity selection menu select Retrieve
- Select mask and select reverse all.
Figure 15 .
Or you can manually check for elements failing.
Go to Geoms>Temp nodes select the elements and select add or cilck middle mouse button for confirmation.
Figure 16 .
After giving tempnodes for failing elements delete the elements and correct the geometry where temp nodes are given.
Step 10: Start meshing from a complex area or the area which is diverging
Figure 17 .
Mesh part by part by part. go to mesh panel from 2D> Automesh
- Select Size and bias option
- Keep target element size as 4
- Do mesh with Elems to surf comp : will keep mesh on component irrespective of current component.
- first order: keeps the mesh in first order
- Keep connectivity: keeps the mesh connected to adjacent meshed surface.
- flow: align size: keeps th mesh in proper alignment and elememnt size within range
- map: size skew: keeps the elements size average throughtand avoids skew elements.
- link opposite edges with aspect ratio Auto: keeos equal number of nodes at opposite ends of surface to give a good mesh.
Figure 18 .
Tip: Start from on part and then to adjacent surface. do not jump from one area and to area far from it.
Tip: Mesh rib and then surface so as to avoid disconnectivity of nodes of surface and nodes at rib. as shown
Figure 19.
If by chance this situation occurs and you have meshed rib the to relove this issue or to bring connectivity.
Go to 2D> Mesh edit
- Select Imprint option.
- Select node from source destination and select nodes to connect from rib.
- Select the elements from destination option and select 2 layers or rows of lements around the rib.
- In layers give value 2 as we have selected 2 layers of elements. and select create.
Figure 20.
Meshing at Holes
Step 12: To get a good mesh at holes we need to make the nodes at holw even and then rotate. make the nodes even while meshing.
- Create a node at center of circle by Geom>Nodes>Arc center
- From option Select lines and select circle and select create. (refer figure 8)
Figure 21 .
Step 13: Now rotate and make the side of hole parallet to nearest edge. to rotate go to Tool>Rotate and selects nodest to rotate.
- Select N1, N2, N3 and base point as centre point.
- Put value 5 degree in angle and click rotate+/ rotate-. (refer figure 9)
Figure 22.
Step 14: Now go to auto mesh (Shortcut: Shift + f12). (refer figure 10)
- Select elements , from elements option select by Geom and select surface with rotated circle nodes.
- Select anchor nodes and select the nodes on circle. Basically anchor nodes freezes the selected nodes and rest nodes are remeshed.
Hence making it a good mesh flow around hole without trias touching to it.
Figure 23.
Tip: Resolve the quality issues while meshing the surface itself and do not leave failed elements to resolve after finishing mesh.
Rules to have a good mesh:
- Maximum feature capturing is recommended.
- Reduce number of trias as much as possible
- Avoid surface with more tria concentration
- No trias touching the edges
- No opposite trias
- No trias in Fillet and hemmings
- No rotational Quads
- No back to back touching trias
- No tria touching another tria.
CHECKS:
=Trias in mesh
Once after the mesh is done Check for mesh violating trai rules. to get better view of tria in the visulization tab select by Config
It will show the trias and quads in contrasting colours which make easy to look out for trias.
Resolve the opposite trias, drag trias touching the edge wherever possible, drag apart tow or more touching trias. ( always give smooth after draging tria)
Figure 24.
=Free edge check by to junction and free edge
To check free edge go to Tools>edges (shortcut : shift + f3) and select elements and select free.
Select find edges. ( Rename the component created for free edges ^edges to free ) Aslo taking t-connections (yellow lines) to get a proper view.
- Again select elements and change free to T-connections select find edges
- Then hide the surface and mesh. lookfor any single red line in between meshed elements.
Figure 25.
Now if there are any such free edges, from same Edge panel select elements give tolerance as 1 and select preview equivalence.
- The free edge nodes within tolerance range will appear as green dots. Select equivalance and the nodes will be pasted.
- Even after equivalencing the nodes does not get pasted then do manual pasting or replacing nodes.
- Go to Geom> node edit (shortcut f3) select replace node and with as another node. Hypermesh will replace one node with other and hence no free edge will be left.
Assigning thickness:
Step 15:
- Measure the thickness of this rib.It is divided into 3 segments and since it is varying thickness rib we will ssign 3 diffrent thickness to three diffrent segments. Thickness measured are 2.77, 2.69 , 2.46 & 2.04
Figure 26.
- Taking average as 2.7mm, 2.5mm & 2.2mm. Create new component and rename it as Rib2.7 mm, create another component and rename it as Rib2.5mm ; create another component and rename it as Rib2.2 mm
- Create property with its name as Rib2pt7 mm and in it give value of thickness as 2.7mm
simillarly for other two components.
- Make Rib2pt7mm as current component and right click on it, menue will pop choose Assign. Another menu will pop up select from property list Rib2pt7 mm. and Apply. similarly do for rest of two component.
Figure 27 (a) . Figure 27 (b).
- Go to Tool> organise, from options select the elements and select elements from 1st segment of rib and select move.
Similarly do for every component.
Figure 28.
- From visualization tab chage form 2D Traditional Element Representation to 2D Detailed Element Representation.
Figure 29.
Step 16: At last check for element normals. Go to Tool> normals. Setlect elements and select display. if all the elements on one side do not have same orientation (colour) then adjust them. Select Adjust. it automatically adjusts the normals. if it dosent there is a chance of duplicate elements.
Figure 30.
Conclusion: Side door panel is meshed with optimum meshflow and 1% tria. with assigned thickness nd zero elements failing for quality.
Final image:
