Five-axis Programming and Machining Technology of Pump Body Parts Based on UG

With the rapid development of high-end manufacturing sectors such as aerospace, automotive, and medical devices, the demand for machining complex and precision parts is growing steadily.

Industry Background and Role of Five-Axis CNC Machining

Against this backdrop, five-axis CNC machining technology has gradually emerged as a key technology for achieving high-precision, high-efficiency manufacturing, thanks to its multi-axis interpolation capabilities and the ability to complete complex surface machining in a single setup.

This is particularly true when dealing with complex parts featuring deep cavities, irregular surfaces, and high-precision hole patterns.

Traditional three-axis machining methods, which require multiple setups, not only increase positioning errors but also struggle to meet the dual demands of modern manufacturing for both precision and efficiency.

• Structural Complexity of Pump Housing Components

As a core component in fluid systems, pump bodies feature complex structural integration, deep cavities, and intersecting multi-directional hole patterns, as well as complex features such as surfaces with varying curvatures and irregular blade slots, significantly increasing machining difficulty.

Taking a specific pump housing model as an example, as shown in Figure 1, it consists of three parts: the lower housing, the volute, and the upper cover.

The lower housing has a complex structure that requires multi-axis rotational positioning for symmetrical machining, and it includes six non-circular blade slots that require five-axis simultaneous machining, imposing strict requirements on tool edge length;

Additionally, deep holes and five-axis fixed-angle drilling operations are required, which demand extremely high machining accuracy and necessitate reaming; the upper cover features a thin-walled, openwork structure with numerous curved surfaces and complex spatial angles, and it imposes stringent requirements on surface quality and geometric accuracy (e.g., ϕ(73±0.025) mm, parallelism 0.015, surface roughness Ra 0.8 μm, etc.).

Furthermore, the material is 6061 aluminum alloy, which is lightweight and easy to machine but prone to deformation, posing significant challenges for the clamping process.

• Existing Research Limitations and Technical Challenges

Currently, researchers have achieved certain results in five-axis CNC machining process planning, toolpath optimization, and fixture design; however, systematic process research on integrated pump-body-type multi-feature composite parts remains insufficient.

In particular, there is significant room for improvement in areas such as multi-process transitions, programming strategy optimization, and simulation verification.

• Research Objectives and Innovations

Based on the UG software platform and using pump body parts as the research subject, this paper systematically conducts research on five-axis CNC machining process analysis and programming methods, focusing on a comprehensive solution spanning the entire process from part structural analysis, process planning, programming implementation, simulation optimization, to actual machining.

The research covers key technical aspects such as toolpath optimization, coordinate system setup, cutting parameter configuration, and fixture design, aiming to address issues such as deformation, difficult clamping, and low precision in the five-axis machining of complex structural parts.

The innovations of this paper are as follows: first, the proposal of a five-axis machining process planning method based on structural feature recognition to achieve efficient toolpath planning for parts with multiple features; second, the integration of the UG CAM module to optimize the five-axis programming workflow, thereby enhancing programming efficiency and machining accuracy; and third, the development of a replicable and scalable five-axis machining process solution through simulation and actual machining validation.

The research findings will provide theoretical support and practical guidance for the CNC machining of similar complex parts, holding significant practical significance for promoting the application of five-axis CNC technology in the high-end manufacturing sector.

Analysis of the Pump Housing Component Structure and Technical Requirements

• Structural Characteristics of the Bottom Housing

The pump housing bottom shell is used for the assembly of the top cover and the worm gear.

It requires high positioning accuracy during assembly and features a complex geometric configuration, as shown in Figure 1(b).

Multiple areas require symmetrical machining with five-axis rotational positioning, and high dimensional accuracy is essential.

There are six irregular blade slots that require five-axis simultaneous machining, which imposes specific requirements on the cutting tool’s edge length.

There are two deep-hole drilling operations in cavities and four five-axis fixed-angle deep-hole drilling operations.

These holes require high precision and require reaming.

Therefore, based on an analysis of the lower housing’s features, the process requires high-precision machining equipment and flexible, adaptable five-axis toolpaths.

Consequently, the process schedules the lower housing for machining on Machine A (a dual-turret five-axis machining center) in two separate operations on both sides.

• Structural Features and Machining Challenges of the Top Cover

The pump housing cover part, shown in Figure 1 (a), is used to secure the impeller and balance the inlet port.

It has high dynamic balancing requirements, complex and precision-critical surfaces, and a complex structure, including multiple surfaces, irregular holes, and variable-section features such as deep cavities (depth 18.2 mm), thin walls (minimum wall thickness 2.1 mm), circular transitions (R4/R6), and multiple C0.5 chamfers, necessitating multi-axis simultaneous machining.

Geometric and positional accuracy requirements are stringent, with dimensional tolerances typically controlled within ±0.05 mm and surface roughness required to be below Ra 0.8 μm.

The use of aluminum alloy results in poor heat dissipation, low strength, and susceptibility to deformation, making machining challenging.

• Process Optimization Requirements and Research Focus

Traditional clamping and positioning methods cannot meet machining requirements, resulting in low processing efficiency and complex process routes that require coordination across multiple operations and workstations, including rough machining, finish machining, and inspection.

Therefore, researching and optimizing the machining process steps, improving clamping and positioning methods, and optimizing programming parameters to enhance machining efficiency and ensure quality are essential and critical to resolving these issues.

The worm gear shown in Figure 1 is a machined standard part used solely as an assembly component; this paper does not include a process analysis of it.

Process Planning for Pump Housing Machining

The pump housing consists of three components and standard bearings.

The process analysis and optimization are as follows:

(1) The worm gear is a standard part used solely as an assembly component and is already being mass-produced;

(2) The pump body lower housing is the main component, as shown in Figure 2(a).

High-precision main equipment A handles production scheduling.

First, five-axis CNC machining completes the pump body’s bottom surface.

Then, the process disassembles and repositions the part and performs five-axis CNC machining on the front surface.

The part remains assembled; production resumes after machining the internal surface of the upper cover.

(3) Machine B performs machining of the end cover’s internal surfaces, as shown in Figure 2(b).

(4) After completing internal machining, the process removes the upper cover and assembles it onto the pump body on Machine A using M6 bolts.

No re-centering occurs; only height data requires setting to complete all external machining of the upper cover.

(5) After completing 90% of the external machining on the upper cover, secure it to the pump body with M5 screws, then remove the M6 bolts to complete the remaining 10% of machining.

The entire upper cover machining is completed in approximately 20 minutes, significantly improving production efficiency, as shown in Figure 2(c).

Machining Sequence Planning for the Pump Housing

• Bottom Housing Machining Process

The raw material for the bottom housing component is a 90 mm × 90 mm × 60 mm aluminum alloy block. Machine A, a Linak-system dual-turntable five-axis machining center, has been selected.

First, machine the 60 mm × 60 mm square platform on the bottom of the housing, along with the contours of the octagonal perimeter, countersinks, and markings.

Complete two deep drilling operations for cavities and four five-axis fixed-angle deep drilling operations.

Next, perform reaming and chamfering of sharp edges. Then, the process dismounts the part, flips it, and clamps it at the 60 mm × 60 mm square platform position; it centers and aligns the bottom, and sets the workpiece coordinate system origin at the bottom.

The process completes machining of the front surface features of the bottom shell, focusing on the six blade slots and M4 threads, as shown in Figure 3.

• Upper Cover Internal Machining

The raw material for the top cover part is a 75 mm × 75 mm × 25 mm aluminum alloy block.

Machine B, a dual-turret five-axis machining center, is selected.

A D12 flat-bottom end mill performs rough machining of the upper internal and external contours using fixed-contour milling and depth-contour milling; a D6 flat-bottom end mill then performs finish machining of the bottom surface and walls using depth-contour milling and bottom-wall milling paths.

A 4.2 mm drill bit drills the M5 pilot holes; an M5 tap taps the threads; a D6 chamfering cutter chamfers all sharp edges to C0.5; finally, an R3 ball-nose end mill finishes the internal curved surface of the end cap. The total machining time for the upper cover interior is approximately 15 minutes, and the machining results are shown in Figure 4.

After completion, the process disassembles the part and mounts it on Equipment A, then attaches it to the pump body using M6 bolts.

The process requires no centering; it measures the total height after assembly and inputs it into the coordinate system for compensation.

Since the workpiece coordinate system has already been defined on the bottom surface of the workpiece and is consistent with the programming coordinate system, the next machining step can proceed, as shown in Figure 5.

• Post-Assembly External Machining of the Top Cover

After assembly and positioning, select a D12 flat-bottom end mill and use fixed-contour milling and depth-contour milling to rough-machine the outer surface of the top cover.

When programming, be sure to avoid the M6 bolts and complete the machining of the bottom surface; use a D6 chamfering cutter to chamfer the M5 threaded holes;

Next, use a D10R1 round-nose end mill to finish the external curved surfaces of the end cap; then use a D6 flat-bottom end mill to rough and finish the six normal-angle irregular holes using fixed-contour milling; then install M5 screws to secure the top cover to the pump body, remove the M6 bolts, and rough and finish the M6 bolt areas;

When programming the toolpaths, pay attention to tool transition handling. Finally, chamfer the ϕ8 hole locations to complete all machining operations on the top cover.

UG-Based 5-Axis Toolpath Planning and Programming Techniques

• Rear Side Machining of the Bottom Shell Part

(1) D12 Flat-End Mill Roughing Strategy for Deep Cavity Milling

Use a D12 flat-bottom end mill for roughing. Select the “Cavity Milling” toolpath, set the cutting depth to 51 mm, choose the “Follow Contour” cutting mode, set the step size to 60% of the tool length, and set the maximum cutting distance to 3 mm.

(2) Outline Milling and 5-Axis Contour Finishing of Multi-Angle Bevels

Next, select the “Outline Milling” toolpath, specify “Wall,” and automatically generate an auxiliary bottom surface of -1 mm. Select “Contour Milling” for the drive method, select “Auto” for the tool axis, use toolpath rotation and copying to complete the fixed-axis machining of the other 4 45° bevels, then copy the toolpath, modify the selection to “Wall,” automatically generate an auxiliary bottom surface of 0 mm, and complete the 5-axis contour finishing of the 34° bevel.

(3) Deep Hole Machining Operations

Select the 5-axis drilling toolpath, specify the feature geometry to select 4 45° angled holes, choose a 5.5 mm drill bit, set the toolpath loop to “Deep Hole Chip Breaking” mode, and complete 4 5-axis fixed-angle deep drilling operations.

Then complete 2 cavity deep drilling and reaming operations.

(4) Bottom Surface Finishing Strategy

Select the “Bottom Surface Milling” toolpath, as shown in Figure 6.

Specify the bottom surface of the cutting area, set the tool axis to “Perpendicular to the First Surface,” select “Bottom Surface” for the spatial range of the cutting area, and choose “Follow Contour” for the cutting mode.

Use toolpath copying, transformations, and parameter adjustments to complete the finishing of the part’s other bottom surfaces.

(5) Outer Contour Finishing and Edge Treatment

Select the “Deep Contour Milling” toolpath, as shown in Figure 7. Adjust the “Part Side Allowance” and “Part Bottom Allowance” parameters.

Assign different “vectors” to the tool axis based on the specific surface.

Complete the finishing of the part’s outer contour through toolpath copying and transformation, parameter adjustments, and other operations.

Finally, chamfer the sharp edges.

• Front-side Machining of the Bottom Housing Component

(1) D12 Flat-End Mill Roughing Strategy for Deep Cavity Milling

Machining the chamfers around the ϕ68 blade slots, as shown in Figure 8. Load the R3 ball-nose end mill, select the “Fixed Contour Milling” toolpath, set the drive method to “Area Milling,” select “Follow Contour” for the non-steep cutting mode, choose “Inward” for the toolpath direction, “Sequential” for the cutting direction, “Constant” for the step size, and set the maximum distance to 0.1 mm, among other parameter settings.

(2) Finish machining the blade slot walls, as shown in Figure 9. Select a custom ball-nose end mill as the tool. Select the 5-axis “Contour Milling” toolpath.

In the parameter settings, specify the wall, select the blade slot wall, choose “Contour Milling” as the drive method, select “Auto” for the tool axis, and configure other parameters.

Be sure to set non-cutting movement parameters; set the feed type to “Linear,” and set the rapid traverse distance to 200% of the tool diameter.

Set the part safety distance to 3 mm, select “Envelope” in the safety settings, and set the safety distance to 3.

Use the toolpath simulation to verify the tool’s safe path and avoid collisions.

• Machining of the Upper Cover

(1) Internal Rough Machining of the Upper Cover

For rough machining of the upper cover’s interior, select “Fixed Contour Milling.”

Choose “Curved Surface Area” as the drive method, “Helical” as the cutting mode, and set the number of passes to 50.

Leave a 0.2 mm allowance for surface offset. Select the tool axis as the projection vector, and choose an arc (parallel to the tool axis) with a radius of 50% for the approach type.

Set the approach position 1 mm above the surface and use a top-to-bottom spiral machining path.

The tool runs smoothly and machining is efficient, as shown in Figure 10.

(2) Deformation Control and Chamfering Strategy

To ensure that the top cover does not deform during external machining and to maintain its structural integrity, the process excludes machining the interiors of the six normal-oriented irregular holes.

However, a 0.5 mm chamfer must be applied.  Select 5-axis variable contour milling.

For the drive method, select “Surface Area”; for tool position, select “Tangent”; for cutting mode, select ‘Unidirectional’; for step count, select 0; and for projection vector, select “Tool Axis.”

Set the tool axis to “Relative to Drive Body,” with a rake angle of 0° and a flank angle of -45°.

For non-cutting motion parameters, set the approach type to “Plunge,” the approach position to “Distance,” and the height to 200% of the tool length.

Under the “Common Safety Settings” options, select “Sphere,” and set the tip radius to 40, as shown in Figure 11.

(3) Assemble the top cover onto the pump body.

After setting the coordinate system height, select the D12 flat-bottom end mill, choose the fixed-contour milling toolpath, and use the surface-curve-driven method.

Set the cutting mode to “Helical,” leave a 0.2 mm stock allowance, and set the number of passes to 50.

Select “Tool Axis” for the projection vector and use a bottom-up spiral path for roughing to remove the excess material from the end cap shell, as shown in Figure 12.

(4) Multi-Feature Hole Machining (Roughing and Finishing)

Rough-machine the 6 non-circular holes; use a D6 flat-bottom end mill.

Select the “5-axis variable contour milling path,” choose “Surface Area” as the drive method, set the internal parameter “Surface Offset” to 0.2 mm, select “Helical” for the cutting mode in the drive settings, and set the number of passes to 8. select “Side-edge drive body” for the tool axis, ensuring the side-edge direction is outward, choose “Grid or Trim” for the line type, and set the side tilt angle to 0°.

After configuring the toolpath parameters, use toolpath transformation to select “Rotate around point,” then copy the toolpath 6 times at 360° intervals to complete the rough machining of the remaining non-circular holes, as shown in Figure 13.

(5) Feed Rate Optimization Strategy for Finishing Six Normal-Angle Slots

The finishing of the 6 normal-angle slots is shown in Figure 14.

A D6 flat-bottom end mill is selected; the roughing toolpath is copied and the parameters are modified.

Continue to use the “5-axis variable contour toolpath,” select “Surface Area” for the drive method, set the internal parameter “Surface Offset” to 0.2 mm, and set the drive settings to “Helical” for the cutting mode with a step count of 0. leaving other settings unchanged.

However, the “Feed Rate and Speed” parameters can be optimized.

In the “More” options, adjust the “Feed Rate” to 50% of the cutting speed and the “First Pass Cutting” to 20% of the cutting speed.

This significantly reduces the impact force caused by the feed rate, minimizing the likelihood of deformation in the end cap workpiece.

Similarly, after setting the toolpath parameters, use the toolpath transformation function, select “Rotate Around Point,” and copy the toolpath 6 times at 360° intervals to complete the finishing of the other non-circular holes.

(6) Final Surface Finishing and Completion

Select a D10R1 round-nose end mill and use a fixed-contour toolpath to finish the outer curved surface of the end cap.

The toolpath must be set to avoid the M6 bolt. After machining is complete, remove the M6 bolt and perform roughing and finishing on the area where the M6 bolt was located.

When programming the toolpath, pay attention to tool transition handling, the selection of the cutting direction for the curved surface area, and the drive method. Finally, chamfer the ϕ8 hole locations.

The end cap part has completed all machining operations, as shown in Figure 15.

Conclusion

This paper systematically examines the challenges of five-axis machining for pump housing components, conducting research on process analysis and design, fixture positioning strategies, toolpath planning, and programming techniques, and has achieved the following key results.

(1) Precision Assurance Through Process and Clamping Optimization

Five-axis machining technology reduces the number of clamping operations to ensure precision through process and clamping methods.

A unified coordinate system is established through assembly and debugging, aligning the programming datum with the workpiece coordinate system, eliminating repeat positioning errors (positioning accuracy ≤ 0.01 mm), and ensuring positional accuracy (geometric and positional tolerances ≤ 0.02 mm).

This approach minimizes the impact of coordinate conversion errors on toolpath accuracy at the source, establishing an efficient process logic of “single clamping, multi-directional machining.”

(2) Programming Strategy Optimization and Efficiency Improvement

Based on UG 12.0 software, we encapsulate typical toolpaths for complex surfaces into modular packages and reuse them through toolpath transformations (rotation, mirroring), thereby reducing the programming cycle for similar parts by more than 40%.

Innovative “3+2” directional machining post-processing settings combined with 5-axis simultaneous finishing strategies have optimized the machining time for the pump housing cover to 35 minutes (a 35% reduction compared to traditional processes), achieving dual optimization of machining efficiency and cost while ensuring precision.

(3) Advanced Toolpath Design and Machining Stability Enhancement

Technological innovations in toolpath design: flexibly utilizing toolpath types such as fixed-contour milling and 5-axis variable-contour milling.

By adjusting flexible control parameters for the tool axis to optimize (with tool axis vector continuous variation error ≤ 0.5°), combined with tool tilt angle control (within the 5°–15° range to avoid interference), we have overcome the machining challenges of deep cavities, openwork, and thin-walled features.

The surface roughness of aluminum alloy parts reaches Ra 0.8 μm or less, and thin-wall deformation is ≤ 0.05 mm.

Furthermore, by implementing layered stock homogenization (with a stock allowance of ≤0.1 mm per layer), feed rate reduction at corners (30% reduction), and regional spindle speed matching (20% reduction in spindle speed at curved corners), we have further enhanced cutting stability and surface quality.

Through systematic optimization of “process–programming–toolpath,” this paper establishes a comprehensive technical workflow for the 5-axis machining of complex pump housing parts, overcoming bottlenecks in multi-feature machining and providing a reusable solution for similar parts.

Addressing the current limitations of toolpath optimization—which relies on manual intervention and empirical parameter design—the paper identifies the direction for upgrading toward digital twin virtual verification and AI-algorithm-driven automatic optimization, thereby providing practical guidance for the intelligent development of CNC machining within the context of smart manufacturing.