[Case Study] Using 5-axis Machining for Advanced CNC Prototyping

Our company has a milling machine equipped with 5 controlled axes - DMU monoBLOCK 75 (figure 1), which provides enormous possibilities for machining many details of varying degrees of complexity. It is characterized by a rigid structure, which is equipped with, among others, a spindle with a rated power of 35 kW and a maximum rotational speed of 20,000 rpm. It has a work table measuring 800x650mm equipped with a rotary table with a diameter of 650mm, on which elements weighing up to 600 kg can be machined. Additionally, the tool magazine contained in it can hold up to 60 pieces of machining tools.

Fig. 1. DMU 75 monoBLOCK owned by SOLIDEXPERT INNOVATION

This article presents the technology developed by SOLIDEXPERT INNOVATION for manufacturing a detail, the model of which is shown in Figure 2. The part is a prototype, so the preparation of the machining program focused primarily on obtaining dimensional and shape accuracy while using moderate machining parameters.

Fig. 2. The obtained model of the part to be machined.

.

The part is made of Aluminum 5083 alloy, which is characterized by high corrosion resistance and high fatigue strength. A semi-finished product (figure 3) in the form of a cube with dimensions of 260x120x85 was used.

Fig. 3. Shape and dimensions of the semi-finished product [mm].

The developed technology for machining the above element required the use of the following list of tools supplied by Ceratizit:

1. Deburring cutter 8 mm (90)

2. AluLine 10 mm shank cutter

3. Frez do obróbki zgrubnej AluLine 16 mm

4. Frez trzpieniowy AluLine 16 mm

5. Frez z czołem kulistym AluLine 10 mm

6. Frez z czołem kulistym 8 mm

7. Frez nasadzany A 490-12 MaxiMill 80 mm

A 5-axis vice provided secure fixing of the semi-finished product in the machine's workspace. It allowed the machining of the element in one clamping, with different angular positions of the machine's table. Figure 4 shows the method of fixing the processed element, on which most of the planned machining operations have already been performed.

Fig. 4. Clamping the workpiece in a five-axis machine vice.

The five-axis machining center, thanks to the additional rotary axes A and C, allows for the production of many milling settings without the need to change the setting and re-clamp the workpiece. Examples of the rotary table and cradle positions are shown in the drawings below, for which the values of the A and C axes were:

a) Rotation axis (cradle) A = 0°

Rotation axis C = 0°

b) Rotation axis (cradle) A = 90°

Rotation axis C = 0°

c) Rotation axis (cradle) A = 90°

Rotation axis C = 270°

d) Rotation axis (cradle) A = 90°

Rotation axis C = 90°

Fig.5. Machine table positions (simulation in Virtual Machine).

Programming the machining process in CAMWorks:

1. Roughing of the outer profile

The first stage of processing covered the convex surface of the outer outline of the detail in question.
For this purpose, a multi-surface property was created in CAMWorks, based on which the Area Offset operation was created, which belongs to the group of 3-axis operations. The paths obtained in the three operations are shown in Figure 6. Additionally, it should be noted that
that the generated tool paths were obtained in three separate milling setups.

Fig.6. Volumill toolpaths in roughing.

The VoluMill strategy was used as the path model, which primarily allowed for a significant reduction in cycle time and tool wear. A 16 mm end mill was used for machining roughing, which proved to be ideal during the HSM process. A 0.25 mm allowance was left on the machined surfaces for later shaping. The result of the above procedures is shown in the drawing below.

Fig.7. The effect of performing the first operations - roughing

2. Planning

The next machining step was to plan the surface from the side of the irregular pocket. A milling head and a planning operation were used for this purpose, the programmed paths of which are shown in Figure 8a. The green color of the surface in Figure 8b confirms that the machined the surface after the process matches the part model and does not require additional processing.

Fig.8. Surface planning: a) tool paths, b) comparison of the machined part with its model.

The other side of the detail was processed in an identical manner, the result of which is shown in the drawing below.

Fig.9. The effect of planning the bottom of the discussed part

3. Contouring the external profile

The next stage of the process is to finish the surface, which was previously roughed using the VoluMill strategy. The machining was carried out with a 16 mm end mill, in particular using the blades located on its cylindrical surface. The tool paths were programmed in such a way that the tool was inserted outside the material, and the entry was in an arc. The part was machined in two milling settings, as shown in Figure 10 below.

Fig.10. Paths showing the contouring of the external profile

4. Machining the bottom of the part

The previously used operations concerned primarily the external surfaces from the convex side of the discussed part. The next step is the processing of the bottom, i.e. the side of the detail, which was modeled with an edge rounding of R=10 mm ( figure 11)

Fig. 11. Rounded surfaces of the bottom of the part with a radius of 10 mm.

First, the material was selected from the concave side of the part (clamping side) to a depth of 20 mm using a 10 mm diameter end mill.

Figure 12 shows the tool paths with a 0.2 mm allowance on the side surface, which was left for later shaping machining. The value of the cutting depth a_p was set at 2 mm using the following machining parameters: v_c=250 m/min and f_z=0.07 mm/tooth.

Fig.12. Roughing paths to a depth of 20 mm.

Then, the above-described roundings were cut using a ball-end milling cutter.
with a diameter of 10 mm. The 3-axis operation Z Level was used for this purpose. The Roughness Height method was set as the depth parameter in the CAMWorks program with a value of 0.02 mm, which allowed for the optimal distribution of tool paths on the machined surface (Figure 13a). As a result of the above actions, the result was obtained, which is visible in Figure 13b.

Fig. 13. Machining the bottom of the part: a) cutting with a ball-shaped cutter, b) the surfaces of the part after finishing operations.

5. Pocket Processing

a) Roughly

The first stage of pocket machining was theRoughing operation, which belongs to the 2.5D operations group. A necessary condition is to first define the 2.5 axis property called Irregular pocket.

The pocket in the discussed detail is characterized by a large depth (70 mm) compared to its width, which is variable and oscillates in the range (20 ÷ 12 mm). This requires the use of a long tool, which will also be characterized by its long working part.

Roughing was programmed with a 3° ramp entry and a down-cut cutting method. A 0.2 mm allowance was left on the side surfaces and a _p depth of cut was set to 3 mm. With these settings, a cutting speed of 250 m/min and a feed of 0.05 mm/tooth were used. The resulting tool paths are shown in Figure 14.

Fig. 14. Tool path in roughing a pocket.

The depth of the previous machining reached the beginning of the rounding of the bottom edge of the discussed detail. From this point, an 8mm ball milling cutter was then used, the movement of which was programmed
using Multi-axis operation.The tool paths obtained as shown in Figure 15 constituted rough machining of the pocket bottom, leaving an allowance of 0.2 mm.

Fig. 15. Roughing paths for the bottom of an irregular pocket.

The paths in the above operation were very dense due to the large reach of the tool
and machining with a ball-shaped cutter. Additionally, the option of tilting the cutter relative to the cutting direction as Normal to the surface was introduced, while limiting its angular movement in the range of 2 (Figure 16), which was intended to minimize the risk of collision of the tool shank with the upper edge of the pocket.

Fig. 16. Tool tilt angle limitation window in CAMWorks.

b) Finishing

The final surfaces forming the pocket of the discussed part were obtained using two machining operations. The first one – Contouring was programmed to finally obtain vertical surfaces. Down-cut milling with entry was used tools in an arc,
and the cutting depth was set at 10 mm, which resulted in the tool paths shown in Figure 17a.

The bottom with roundings was finished with a ball-nose cutter using the Multi-axis operation (figure 17b). Similarly to roughing, the tool tilt angle was also limited during the cutting process.

Fig. 17. Pocket contouring: a) finishing paths of the vertical walls of the workpiece, b) tool paths for bottom machining.

As a result of the above procedures, the finished pocket surfaces were obtained, which are shown in the drawing below.

Fig.18. The result obtained after finishing the irregular pocket.

As a result of machining on a large overhang and in a relatively tight space, the risk of collision of the tool shank with the edges of the workpiece pocket has increased. For this purpose, the technology department specialists used an additional option to simulate and verify programmed paths, which is the Virtual Machine. Using the 3D model of the machine (figure 19a) and the kinematics imposed on its assemblies, there is the possibility of the most realistic and reliable verification of the prepared machining. Virtual preview of the movement of machine assemblies with collision detection in the Eureka program is an additional and currently the best solution used to verify programmed machining. Figure 19b shows the described process for rowing the bottom of the pocket with a ball-shaped cutter.

Fig. 19. Virtual Machine Simulation: a) model of the machine used in the process, b) verification of the pocket bottom machining.

6. Machining of the detail from the side of its mounting

The next stage of the part machining process involved its surfaces located on the side where the stock was clamped in the vise. For this purpose, contouring operations were used, which
with the use of roughing cutters allowed for effective removal of unnecessary material, leaving an allowance of 0.5 mm on the walls of the element. The paths shown in Figure 20a were obtained in two separate milling settings.

Then the same surfaces were subjected to finishing treatment (Figure 20b), which
using the appropriate tool and machining parameters (v_c=200 m/min, f_z=0.1 mm/tooth) allowed to remove the remaining allowance and obtain the desired quality
and surface accuracy.

Fig.20. Machining of the part on the clamping side: a) rough contouring, b) finishing contouring.

The noticeable lack of paths in the middle of the part's surface was programmed intentionally. The material left behind will be processed in the last operation, the purpose of which is to cut off the finished part from the remaining semi-finished product, the surfaces of which have so far served as mounting points for the part in a machine vice. The result of the above machining operations is shown in Figure 21.

Fig.21. Condition of the part after contouring the surface on the mounting side.

7. Chamfering

Using the 2.5D property named Curve Property a contouring operation was created with the chamfer machining option selected (the resulting paths are shown in Figure 22). In the milling head, there is a place found a tool for deburring sharp edges (8 mm, 90 milling cutter). This operation was performed on two edges of the workpiece that required deburring.

Fig. 22. Paths showing the tool paths for deburring sharp edges.

8. Cut off

The last operations performed on the part in question were those responsible for cutting it off from the remaining material and then finishing the surface that had been connected to it up to that point.

The cut-off was performed with the material clamped directly to the machine table using clamping clamps. The contouring operation was used to program this machining, which left a 0.5 mm allowance for later finishing machining. The tool paths (figure 23) were programmed so that the tool entered in an arc. Then the cut-off surface was subjected to final machining to obtain the appropriate quality and accuracy of the machined surface.

Fig. 23. Programmed tool paths to cut off parts from remaining material.

To sum up, many factors influenced the execution of the discussed part. First of all, it is necessary to mention the DMU 75 monoblock machining center, which, thanks to five-axis control, reduced the number of workpiece clampings to a minimum, which significantly shortened the machining time and increased its accuracy. The high-class tools from Ceratizit used in the technological process also ensured the smoothness and efficiency of the machining process. First of all, it is necessary to mention the CAMWorks software, thanks to which the technological department of SOLIDEXPERT programmed the appropriate machining operations, which, in connection with the appropriate machine
and tooling allowed us to obtain a finished part (Figure 24) and customer satisfaction.

Rys.24. Zdjęcie przedstawiające gotowy detal.