Let's begin in the Part Design workbench. The conrod is a symmetric part, so it can be modelled as a half and mirrored by the XY plane. Please sketch the bottom part on the XY plane.
Pad the Sketch, then select a face as the below picture.
Sketch the middle part. Use the external constraints to place it precisely.
Pad the sketch as in the below image. You probably should select the reverse direction.
In the similar way select a plane and start sketching the top part of the conrod.
You have to create holes for a crankshaft and a piston pin. You can to this sketching circles on selected faces and using the pocket feature.
Use the Through all option.
In the same way remove material from the middle of the conrod. But this time the pocket feature should be driven by the Dimension option.
The latest FreeCAD introduces the draft feature. The draft is useful for cast and forged parts. Select all side faces with [Ctrl] key. Then activate the draft feature.
In the task view you can see two important text fields: Neutral plane and Pull direction. Activate the Neutral plane field and select the back (parallel to XY) face.
For the Pull direction you should select an edge. The edge should be normal to neutral plane, and in our case parallel to Z axis. At the end increase the Draft angle.
The below image shows the draft feature effects.
In the next step create a draft feature for the pocket in the middle part.
The neutral plane:
And the pull direction edge:
You should also check the Reverse pull direction checkbox.
Optionally round (fillet) some edges. Round works also for edges tangent to the selected edge. Plan a filleting sequence carefully.
There are missing holes for bolts. Select the bottom face for sketching.
If there is not enough material for holes, you can return to the first pad and resize the sketch.
Create a second hole using the Part Design mirror feature. The mirror plane is YZ.
Now you need some Part workbench tools. Use the Part mirror to create mirrored (to the XY plane) solid. I explained Part and Part Design differences in an older post.
Fuse both solids using the boolean union tool.
The final shape looks pretty nice, doesn't it?
FEM analysisZ88 Aurora is a multiplatform, freeware finite element method tools. You can download Z88 for Windows, OS X or Linux from this page. Only 64-bit Linux distributions are supported.
First of all you need an simplified model. Small fillets are very problematic for FEA meshers. I disabled the final solid and created a new fusion repeating last two steps (Part mirror and then fusion) for latest pre-filleted feature (Draft001).
Select a solid and export it as a STEP file.
In the Z88 you should use the Linear mechanical analysis. Start a new project creating a new directory.
Import the STEP file.
The 3 shape can be rotated using RMB. You have 3 visibility presets: Shaded, Surface Mesh, Mesh and Picking.
Most of FEM tools is divided to three parts:
- pre-processor - create a mesh, add constraints,
- solver - calculate displacements and stresses,
- post-processor - display results.
Tetrahedron No. 17Next I clicked Add to add a rule and Create to create a mesh. Then click Mesh info to test if the mesh is computable.
- Linear shape functions
- Quality of displacements bad
- Stresses in the Gauss points inaccurate
- Stresses in corner nodes very inaccurate
- Computing effort: medium
- Size of element stiffness matrix: 12 12
Tetrahedron No. 16
- Quadratic Isoparametric Serendipity element
- Quality of displacements very good
- Stresses in the Gauss points very good
- Stresses in corner nodes good
- Computing effort: very high
- Size of element stiffness matrix: 30 30
In the next step you have to check surfaces for constraints. Select a node with [Ctrl] and the click Surface and Add set. You can change name for the created set. The Angle parameter can change selected area (check the Z88 manual for more information).
Create a second set for the pin hole.
Upper nodes are unnecessary, you can deselect them with [Shift] and rectangle selection.
Next add constraints. For the bearing set X, Y and Z displacements to 0. Then add a new constraint.
For the pin set projected surface load to -28000 along Y direction. The difference between projected surface load and surface load explains on of the Z88 tutorials.
Note: exported STEP is in [mm]. Internal material Z88 library uses [mm] and [N]. So, surface load is in [N] and stresses will be in [MPa] ([N]/[mm^2]).
Open the Material database tab and define a material.
Finally, you can run one of the 4 solvers. Check Z88 manual for more information. I used SICCG.
After successful calculation open the post-processor and check result.
You can use a clipping plane to see internal points.
FreeCAD 1 file.
FreeCAD 2 file.
Used in the tutorial:FreeCAD 0.13.1806 (Git)
Z88 Aurora 2