**4.2 Stock of material for finishing operations (stock material)**

Normally some stock of material (also called thickness) is left for the finishing operation. The value of this stock of material is set in the CAM by the user, and it is an offset of the geometry to be machined. For steels machining an average of values that are employed are between 0.5 mm and 1 mm of stock that should be removed in the finishing operation. One value given to the thickness of the leftover of metal could represent a significant effort in finishing and this could prejudice the quality of the surface and also prejudice two situations: a) geometric errors caused by deflection of the tool; b) elevated surface roughness. Low stock can also prejudice the quality of the surface therefore tool can come across difficulties when carrying out properly, the material being cut. This causes passing and crushing material that should be cut. Once again each case ought to be methodically evaluated.

When milling complex shapes besides this theoretical stock, a volume of material cannot be removed from the roughing, due to topological limitations between the surface complexity and cutting tool geometry.

An extra volume of stock can be found on the degrees of material formed after roughing as illustrated in Figure 6(a). This extra volume depends of the depth of cut, the curvature of the surface and the geometry of the tool. Cutting tools with an extreme radius or spherical tools minimize but do not eliminate this condition.

To optimize roughing, tools with greater diameters are employed. In regions of corners, many times the cutting tool is limited to reach and to carry out the milling. Then again an extra volume of material is left by the roughing (Figure 6).

Fig. 6. Thickness to finishing

Block of raw material

(a) Row material cubic (b) Row material near net shape

**4.2 Stock of material for finishing operations (stock material)** 

Once again each case ought to be methodically evaluated.

extra volume of material is left by the roughing (Figure 6).

minimize but do not eliminate this condition.

The roughing employs movements in 2 ½ axis. The tool is positioned at a determined height in Z. After movements are executed in 2 axes for the removal of material at this level. When the removal of material at this level is finalized the tool is then positioned at a new level of Z (defined by the depth of cut), the material is removed at this plan. The process is repeated until the roughing is complete. End-mill with corner radius is the cutting tool frequently

Normally some stock of material (also called thickness) is left for the finishing operation. The value of this stock of material is set in the CAM by the user, and it is an offset of the geometry to be machined. For steels machining an average of values that are employed are between 0.5 mm and 1 mm of stock that should be removed in the finishing operation. One value given to the thickness of the leftover of metal could represent a significant effort in finishing and this could prejudice the quality of the surface and also prejudice two situations: a) geometric errors caused by deflection of the tool; b) elevated surface roughness. Low stock can also prejudice the quality of the surface therefore tool can come across difficulties when carrying out properly, the material being cut. This causes passing and crushing material that should be cut.

When milling complex shapes besides this theoretical stock, a volume of material cannot be removed from the roughing, due to topological limitations between the surface complexity

An extra volume of stock can be found on the degrees of material formed after roughing as illustrated in Figure 6(a). This extra volume depends of the depth of cut, the curvature of the surface and the geometry of the tool. Cutting tools with an extreme radius or spherical tools

To optimize roughing, tools with greater diameters are employed. In regions of corners, many times the cutting tool is limited to reach and to carry out the milling. Then again an

Fig. 5. Blank material options

used for this operation.

and cutting tool geometry.

Frequently the differences of the volume of material beyond the theoretical stock is not cautiously evaluated, which has repercussions with possible problems in the milling. It is common that the machinists of the CNC machines reduce the speed during the milling process manually in some regions of the piece. To minimize this problem of semi-finishing operations have the objective to remove this excess of material and maintaining the stock as close as possible to the theory value (offset of geometry).

#### **4.3 The tool-surface contact in free form milling**

Finishing operation of machining can be considered the most important along the manufacturing free form shapes, once that implicates directly on the final product, in terms of surface integrity and geometric errors. A ball-end cutting tool is the most suitable to finish free form shapes by milling due to this geometry which permits to reach different curvature shapes. However, this tool implicates in specifics characteristics in milling free form shapes, once that the contact tool/surface alternates constantly and affects directly the milling process, in terms of cutting speed, cutting force, surface quality and so on (see also SOUZA et al, 2010).

First, the cutting speed usually cannot be calculated by nominal tool diameter. It has to be taken into account the effective diameter according to the axial cutting depth together to shape curvature. For a planar surface milled by a ball-end tool (Figure 7), the maximum effective diameter can be calculated by equation 2. But it has to be taken into account the radius of curvature of a free form geometry alternates constantly (Figure 7b). Therefore, the effective tool diameter following this oscillation and thus, the cutting speed as well. This is one of the drawbacks because the machining process became unstable.

$$R\_{cf} = \sqrt{R^2 - (R - ap)^2} \tag{2}$$

Where:

*Ref* = Effective radius [mm] *ap* =axial depth of cutting [mm] *R* = Tool radius [mm]

Advanced Free Form Manufacturing by Computer Aided Systems – Cax 563

High frequency spindles, in combination with high feed rates are a more precise characterization for HSC (High Speed Cutting), especially for die and mould manufacturing. Literature mention HSC operations using feed rates as high as 20.000 mm/min. However, the feed rate varies severely along the path. These feed rate oscillations depend on two limitations: mechanical (inertia) and electronic (CNC control). In the first case, the machine does not achieve acceleration and deceleration as fast as required by a specific programmed feed rate. In the second, CNC limits the feed rate to a maximum value according to its processing capacity, considering a tool path is described by small linear segments. Feed rate oscillation happens even in the most updated CNC machines and it drastically affects machining time and surface quality. The ordinary CAM software estimates the machining time considering that the feed rate is kept constant as set in the NC program; the software does not consider the CNC and machine's limitations. Therefore, the machining time

A free form tool path is described by an small straight line interpolation. The respective CNC program generated by a CAM software create an huge NC programs and it represents a great amount of information for the CNC machine to process in short periods of time. As a result, the CNC machine may have to reduce its feed rate to manage such large amounts of information. Therefore, the linear segment length is directly related to the feed rate during milling and, as a consequence, to the machining time. Better description about the topic can

A typical CNC control of a machine tool has two major responsibilities: i) the servo control loop and ii) the interpolator, responsible for coordinating the machine tool axis motions. The NC program, as well as others error compensation programs and routines, is located in a higher level of the control hierarchy. Supervisory tasks such as final part measurements and

From the machine point of view, acceleration, deceleration and kinematics characteristics could be the feed limits in a machining process. According to ELBESTAWI (1997), the main issues in high speed servo control are feed rate planning and servo control loop laws. The users and/or the machine tool builders have to choose between path error and feed rate error. If the path error is allowed, the machine tries to run at the programmed feed rate; however, the trajectory is not guaranteed. If the path error has to be low, the machine keeps

In free form milling, the linear interpolation of straight line segments means a high volume of information to be processed by the CNC. Therefore, in order to manage the tasks to be carried out in real time during machining movements (i.e.: machine control loop, jerk limitation, interpolation, and so on), the CNC reduces the feed rate according to

corrections can be accomplished by the CNC getting feedback from other controllers.

the path accuracy, but the feed rate can be lower than the programmed one.

estimated by CAM becomes very inaccurate [COELHO et al, 2010].

**4.4.1 Feed rate oscillation in free form milling** 

be found ahead in this chapter.

**4.4.2 Machine control** 

its capacity.

**4.4 Machine limits** 

$$R\_{ef} = \sqrt{R^2 - (R - ap)^2} \tag{2}$$

Where:

*Ref* = Effective radius [mm]

*ap* =axial depth of cutting [mm]

*R* = Tool radius [mm]

Another weakness of this process is the surface roughness. First, the cutting speed is zero in the extreme centre of the cutting tool. Therefore, when the centre of the tool is in the cutting area, the tool smash and do not cut the material. This phenomenon affects negatively the surface roughness. The ball mill also leaves a material remain between the cutting passes, known as cusp high. The cusp high depends upon the axial (ap) and radial depth per cut (ae), tool diameter and surface curvature (see Figure 8).

Where:

Ac= cup high [mm]

ae = radial depth of cut [mm]

R = tool radius [mm]
