Siddhant Agarwal & Shane Hereford

KTH Royal Institute of Technology

Stockholm, Sweden

Modern surface mounting technology (SMT) is built up of three processes, one of which is placement of components using a pick-and-place robot, as shown in Figure 1. The picking tool is a ceramic or metal straw which moves vertically down and picks up the component through application of a vacuum flow. The purpose of this computational fluid dynamics (CFD) project is to simulate the flow created by the vacuum pressure inside the picking tool. The component to be picked here is an SR0603 resistor. There are three main objectives of the study:

- Effect of the tool inner diameter on the suction force with a given vacuum pressure.
- Effect of distance between the tool and the component on the suction force for each diameter.
- Modeling the dynamical process when the component is sucked to the nozzle using overset meshes and a one degree of freedom model.

To perform the study, geometries were created for different diameters and distances between the suction tool and the resistor. Then the different geometries were meshed in the grid generation software, Pointwise. These meshes were then imported into CFD++, where the simulations were run to cover the three objectives of the study. The results would be verified using a mesh refinement study for the 0.4 mm diameter nozzle with a distance of 0.5 mm between the object and the component.

The flow inside the nozzle was expected to achieve transonic speeds around Mach 0.7. Therefore, the flow was solved using the compressible Navier-Stokes equations for a perfect gas - assuming air is one. The viscous terms were considered while solving the flow. However, the flow itself was treated as laminar. This is because only a very small region within the entire geometry had a Reynolds number of approximately 5000. In fact, a comparison between two simulations for the 0.2 mm diameter nozzle, one laminar and one with the standard K-ε turbulence model, showed virtually no difference in the force on the component.

It was also observed that the residuals for K-ε turbulence model did not converge properly because it was simply insufficient to model turbulence in this case - possibly due to adverse pressure gradients. Therefore, keeping the objectives of the project in mind, which required parametric studies with two variables - distance and diameter, this simplification was made to save significant computational time.

Furthermore, the 2-D case was treated as axisymmetric about the x-axis to save computational time, and because the flow was expected to be symmetric. This was indeed confirmed from a full 2-D simulation for the overset mesh later on as shown in Figure 2. Other nuances, such as surface roughness, could also not be considered.

A technical drawing of the suction nozzle was provided, and a 2-D axisymmetric geometry was created using SolidEdge. This geometry was then exported to Pointwise to be meshed. The final meshed geometry was then solved using CFD++. Figure 3 shows the geometry created in SolidEdge. Ten different simulations were run with varying nozzle diameter and nozzle distance from the target object. The force generated on the object was simulated for 0.1, 0.2, 0.3, 0.4, and 0.5 mm nozzle diameters all at a 0.5 mm distance from the target object. The lifting force on the object was also simulated at 0.1, 0.5, 1, 2, and 5 mm distances from the target object all with a nozzle diameter of 0.4 mm.

To perform a 1-DOF dynamic model using overset meshing, the geometry seen in Figure 3 was used. The nozzle diameter and distance from the target object simulated in the overset mesh was 0.4 mm and 0.5 mm, respectively.

Meshing was performed in Pointwise. Since CFD++ allows hybrid meshes, a mesh consisting of quadrilateral and triangle elements was constructed to avoid spending too much time on generating a completely structured mesh on a non-trivial geometry. A cell limitation of 100,000 cells was agreed upon to limit the simulation time and allow for the multitude of simulations required for this investigation.

Quad elements were used to resolve the boundary layer using a *Normal Extrusion* in Pointwise as shown in Figure 4. The boundary layer was resolved on the floor, object, and nozzle surfaces to a y+ of 1. Meaning, that for a flow velocity of about 240 m/s in the most critical regions, the initial cell height would have to be 1e-6 m.

The farfield was set to 10 times the length of the object in the y-direction and the total length of the nozzle head in the x-direction. The rest of the domain was then filled with triangles using the 2-D version of Delaunay algorithm.

To check the quality of the mesh, the aspect ratio and area ratio were considered. The aspect ratio of the boundary layer cells on the inside of the nozzle were held lower than the cells on the outside of the nozzle because it was presumed that most of the fluid activity would be concentrated in the smallest part of the nozzle head. The aspect ratio of the boundary layer cells on the outside of the nozzle were still held to below 100. The area ratio was kept to below six in the region surrounding the smallest part of the nozzle head, seen in Figure 5.

The simulations were performed in CFD++ because of its overset capabilities for transient simulations. For steady-state simulations, the mesh generated in Pointwise was imported into CFD++. The flow is solved using pre-conditioned compressible Navier-Stokes equations for a perfect gas. As per the CFD++ user manual, “the preconditioned equation system reduces the stiffness by moderating the eigenvalue spread caused by declining Mach number. It can accelerate convergence in low-speed flows and reduce the inherent level of artificial dissipation associated with the spatial discretization scheme.” [1] It was used for this case because the flow velocity is below Mach 0.3 in the majority of the flow as is seen in Figure 6.

CFD++ uses linear or non-linear forms of the Riemann solver based on the flow speed to provide upwind flux information to the transport schemes used in CFD++ [1]. The default setting using minimum dissipation on only left-hand side, instead of left-hand side and right-hand side, is used since the flow was not expected to have severe transients like strong shocks and expansions. A dissipation rate of 0.25 was set based on the *Help Set Numerics* feature of CFD++, which allows the user to choose a flow type - transonic in this case - and automatically adjust settings for Riemann solver, time discretization, and spatial discretization.

The fluid used is air at standard temperature and pressure (STP): 273.15 K and 101325 Pa, respectively. CFD++'s default settings were left as they were. The domain was initialized using STP conditions and zero velocities in x and y direction. The boundary conditions were set as shown in Figure 7. At the outlet a pressure boundary condition of 71325 Pa is used, symmetry is along the x-axis, and the nozzle and the resistor (marked with a dashed grey box in Figure 7) are set as adiabatic no-slip walls, with the option for solve to wall enabled.

An implicit time integration scheme was used for this project compared to an explicit one for higher stability. The CFL number is ramped up from 1 to 75 from global time step 1 to 100. These settings are automatically updated once transonic flow was set in *Help Set Numerics*. CFD++'s “new Multigrid” method was used for accelerating convergence. It uses a W-Cycle and agglomeration technique that can group 4-6 cells at a time [1].

The simulations were run in axi-symmetric 2-D mode with symmetry axis x placed at y = 0. CFD++ uses a multi-dimensional Total Variation Diminishing (TVD) polynomial interpolation through limited reconstructions over cells and nodes. Nodal polynomials were used because the meshes are of hybrid nature. Furthermore, out-of-face viscous polynomials, consisting of “those contributions to the derivatives in the viscous fluxes which cannot be written purely in terms of the immediate face neighbors”, were enabled [1]. The spatial discretization scheme used was second order accurate.

Before running the simulations with varying nozzle geometries, a mesh study was conducted on the nozzle with a diameter of 0.4 mm and a distance from the target object of 0.5 mm. One coarser mesh and two finer meshes were created and simulated in order to determine whether or not the mesh density was adequate. The base mesh was generated in accordance with the methodology outlined in the Meshing section above. The coarse mesh was generated by reducing the number of points on the geometry surfaces by a factor two. The finer mesh was generated by increasing the number of points on the geometry surfaces by a factor of two, and the finest mesh was generated by making the triangle mesh domains much denser in the critical regions. These meshes resulted in the cell counts presented in Table 1.

Mesh Density | Residual Level | Lifting Force [mN] | Number of Cells |
---|---|---|---|

Coarse | 1e-4 | 0.0759 | 11,472 |

Base | 1e-6 | 0.0878 | 24,167 |

Finer | 1e-4 | 0.0878 | 53,023 |

Finest | 1e-2 | 0.0878 (unsteady) | 82,135 |

The results of the mesh study found that the base mesh created first was adequate. The simulations for the coarse, base, and finer mesh had well converging lifting forces. The lifting force in the finest mesh simulation did not converge well. However, the force found in the coarse simulation was not the same as the other three finer simulations which all converged to the same force experienced by the component. This indicates that the mesh cannot be coarser. Also, the residuals level for the finer mesh did not drop as much as the base mesh. Taking all of these factors into account, the base mesh was used for the rest of the simulations with varying nozzle geometry.

Investigating the effect of inner nozzle diameter on the suction force involved simulating five different inner nozzle diameters, all at the same distance to the target object. The results of these simulations can be seen in Table 2.

Nozzle Diameter [mm] | Lifting Force [mN] | Residuals Level | Max Mach Number |
---|---|---|---|

0.1 | 0.000281 | 1e-5 | 0.790 |

0.2 | 0.00483 | 1e-3 | 0.808 |

0.3 | 0.0270 | 1e-5 | 0.789 |

0.4 | 0.0898 | 1e-6 | 0.806 |

0.5 | 0.213 | 1e-3 | 0.772 |

Surprisingly, varying the inner nozzle diameter had little effect on the maximum flow velocity within the nozzle. It did, however, effect the force exerted on the target object. Increasing the nozzle diameter by 0.1 mm resulted, on average, in a 10 times higher lifting force. The difference between the lifting force generated by a 0.1 mm nozzle and a 0.5 mm nozzle has a factor of 1000.

Investigating the effect of object distance from the nozzle on lifting force generated involved running simulations at five different nozzle to object distances. The geometry used for all of these simulations was the 0.4 mm nozzle. The results from these simulations can be seen in Table 3.

Distance to Object [mm] | Lifting Force [mN] | Residuals Level | Max Mach Number |
---|---|---|---|

0.1 | 4.03 | 1e-3 | 0.883 |

0.5 | 0.0898 | 1e-6 | 0.806 |

1.0 | 0.00915 | 1e-2 | 0.806 |

2.0 | 0.000361 | 1e-1 | 0.805 |

5.0 | 0.0 | 1e-4 | 0.790 |

The nozzle to object distance heavily affects the lifting force generated, while the maximum fluid velocity remains constant, except at a distance of 0.1 mm. This is likely due to the fact that this small distance creates a channel that begins to accelerate the fluid before it enters the nozzle head. At a distance of 0.1 mm the force is multiple millinewtons. Doubling this distance to 0.5 mm reduces the force by a factor of 100. Further doubling the distance to 1 mm and 2 mm reduces the lifting force by about a factor of 10 each time. At a distance of 5 mm the lifting force is zero.

Finally, as per the third objective of this project, the dynamic suction of the component was simulated using a 1-DOF model. The component was free to move along the x-axis as shown in the overset mesh imported in CFD++ in Figure 8. The axi-symmetric model was used because the forces in y and z directions and moments experienced by the component are not considered in interest of time. Another simplification was made to the case by removing the floor from underneath the object because the object was supported in air by extremely thin supports for the purpose of this simulation. As would be seen later, this was done to avoid a lengthy sequence of rather non-trivial cuts.

The mesh was a concatenation of two separate meshes: one with the component and a structured grid extruded out of it and the other one being the background mesh with everything but the component. Care was taken to ensure that the cells extruding out of the component and those in the background mesh in the same area as the component were of roughly the same size to avoid any possible complications during grid cutting procedure.

In CFD++, the hole-cutting for the overset meshes is defined dynamically at each time step using a set of cutter and live boundaries. For this case, the live and the cutter boundaries are shown in Figure 9. The live boundaries essentially march until they encounter the cutter boundaries. Cells not bound by the live boundaries are then orphanized at each step.

The overset simulation was set up in a similar manner to the one for the steady-state case with a few differences:

- Live and cutter boundaries were assigned for performing hole cutting at each time step.
- The simulation strategy was set to transient and a time step of 1e-6 seconds was used.
- The component was assigned a mass of 1e-6 kg and set free to move along the x-axis.

Running the overset simulation was costly in terms of computational time. A small time step of 1e-6 seconds was used as a compromise even though a time step of 1e-8 seconds would have been needed to make the inner residuals drop by at least one order of magnitude. Figure 10 shows the inner grid residuals for the time step of 1e-6 seconds. The global residuals shown in Figure 11 drop by at least three orders of magnitude before beginning to rise again as the simulation approaches 2000th iteration.

The instability of the solution as the simulation approaches 2000th iteration is also evident from the plot of the force experienced by the component shown in Figure 12. With more time/computational resources at hand, one could experiment with a lower time step and a modified grid to improve the stability of the solution as the component gets closer to the nozzle.

The pressure contours at time equal to 0 seconds and time equal to 0.0022 seconds (which is as far as the authors of this report got in simulation) are shown in Figure 13. Similarly, Mach contours at the beginning and end of simulation are shown in Figure 14.

Changing the nozzle diameter by just 0.1 mm has a heavy effect on the lifting force generated on a target object. The force increases by about one order of magnitude when the diameter is increased by 0.1 mm, while the maximum flow velocity and flow profile do not change. This indicates that larger diameter nozzles should be used to pick up and place larger electronic components, as long the diameter is still small enough to not suck the entire component through the nozzle.

It was also found that between 0.1 mm and 0.5 mm from a target object, the nozzle lifting force reduces by two orders of magnitude. The force further reduces by one order of magnitude as the distance is doubled after 0.5 mm. This indicates that for the most secure picking up of electronic components, the suction nozzle should be less than 0.5 mm from the object.

The dynamic simulation utilizing an overset mesh showed that the force generated by the nozzle at the given vacuum pressure was sufficient for picking up the object. The resulting force confirmed the findings from the parametric simulation. The dynamic simulation yielded a lifting force of 0.135 millinewtons.

[1] CFD++ User Manual, /METACOMP/mlib/mcfd.15.1/html/index3.html [2] Vatistas, G. H., Lin, S., and Kwok, C. K., “Reverse Flow Radius in Vortex Chambers,” AIAA Journal, Vol. 24, No. 11, 1986, pp. 1872, 1873. doi: 10.2514/3.13046

If you would like to generate your meshes using Pointwise request a free evaluation today.

In addition to the offer cited above, by submitting this form, you are giving Pointwise, Inc., 213 S. Jennings Avenue, Fort Worth, Texas, 76110, U.S.A. (www.pointwise.com) permission to add you to our mailing list. You will receive *This Week at Pointwise* and other emails about Pointwise activities and other CFD events like webinars, user group meetings, training courses, etc. You may revoke your permission at any time by emailing unsubscribe@pointwise.com with your request.