Five-Axis CNC Pump Body Machining Using UG ( Ⅱ )

This section presents advanced five-axis toolpath planning and programming techniques for machining complex pump body components using UG software.

It covers the systematic machining of the base shell, bottom housing, and upper cover, addressing challenges such as deep cavities, irregular surfaces, thin walls, and multi-feature geometries.

By combining fixed and variable contour milling, five-axis drilling, helical and spiral toolpaths, and precise tool axis control, the workflow ensures high efficiency, positional accuracy, and surface quality.

The methods outlined provide a comprehensive reference for achieving smooth, collision-free toolpaths, minimizing deformation, and optimizing programming and clamping strategies for high-precision CNC manufacturing.

Five-Axis Toolpath Planning and Programming Techniques Using UG

In five-axis machining, toolpath planning and programming play a crucial role in achieving high precision, surface quality, and machining efficiency. 

By utilizing UG (Unigraphics NX) software, complex machining operations can be effectively planned through accurate definition of machining features, tool orientations, and cutting strategies. 

Proper toolpath design enables full use of the five-axis machine’s flexibility, allowing simultaneous control of multiple axes to handle inclined surfaces, deep cavities, and intricate contours with fewer setups.

This chapter focuses on practical five-axis programming methods using UG, introducing step-by-step toolpath strategies for different machining stages. 

For example, the backside machining of the base shell part is presented first to illustrate the workflow from roughing to finishing, highlighting key parameter settings and toolpath generation techniques.

Back Side Machining of the Base Shell Part

•  Select the D12 flat-bottom milling cutter for roughing.

Select “Cavity Milling” with 51 mm depth, “Follow Perimeter” mode, 60% step size, and 3 mm max cutting distance.

• Switch to the “Profile Milling” toolpath, specify the “Wall,” and automatically generate an auxiliary bottom surface at -1 mm.

Select “Profile Milling” as the drive method and ‘Auto’ for the spindle orientation.

Utilize toolpath conversion to rotate and replicate the path, completing the fixed-axis machining of the remaining four 45° bevels.

Duplicate the toolpath, set geometry to “Wall,” add a 0 mm auxiliary bottom, and finish the 34° bevel contour.

•  Select the 5-axis drilling toolpath. Specify the feature geometry as 4 x 45° helical holes. Use a 5.5 mm drill bit.

Set the toolpath cycle to “Deep Hole Chip Breaking” mode to complete 4 x 5-axis fixed-angle deep drilling operations.

Subsequently, complete 2 x cavity deep drilling and reaming operations.

• Use “Bottom Wall Milling” (Figure 1) with perpendicular tool axis and “Follow Perimeter,” duplicating for other surfaces.

• Use “Deep Contour Milling” (Figure 2), adjust allowances and tool axis vectors, replicate for outer contour finishing, then chamfer edges.

Front Face Machining of Bottom Housing Part

• Machine the ϕ68 blade slot taper (Figure 3) with an R3 ball-nose cutter using fixed contour milling and a 0.1 mm step.

• Blade slot wall finishing, as shown in Figure 4. Select a custom ball-nose cutter.

Select the 5-axis “Contour Milling” toolpath. In parameter settings, specify the wall by selecting the blade slot wall.

Choose “Contour Milling” as the drive method, select ‘Auto’ for the tool axis, and configure other debugging parameters.

Note: Set non-cutting movement parameters, set the feed type to “Linear,” and configure the rapid traverse distance to 200% of the tool diameter.

Set the part safety distance to 3 mm. For safety settings, select the Envelope Block option with a safety distance of 3.

Simulate the toolpath to verify the safe tool approach route and prevent collisions.

Upper Cover Part Machining

• Rough the upper cover interior with fixed contour milling in spiral mode, 50 points, 0.2 mm offset.

Select tool axis for projection vector, with feed type set to arc (parallel to tool axis) at 50% radius.

Start 1 mm above the surface and use a top-to-bottom helical path for smooth, efficient machining (see Figure 5).

• To avoid deformation, the six non-standard holes in the upper cover are left unmachined.

Apply a 0.5 mm chamfer using five-axis contour milling with a tangential axis and unidirectional cutting.

Set the tool axis at 0° front and -45° side tilt; use plunge feed and 200% tool length for non-cutting moves.

Under Transfer Common Safety Settings, select “Sphere” and specify point radius as 40, as shown in Figure 6.

• Assemble the upper cover, set height, and helical mill with a D12 end mill, 0.2 mm allowance, 50 steps.

Use “Tool Axis” and rough in a bottom-up spiral to remove the end cover allowance (Figure 7).

• Rough the six holes with a D6 end mill using five-axis helical contour milling, 0.2 mm offset, and 0° tilt.

Rotate the toolpath 360° and duplicate six times to rough the other holes (Figure 8).

• Finish the six holes (Figure 9) using a D6 end mill, duplicating the roughing path with 0.2 mm offset.

Set “Feed Rate” to 50% and “First Cut Feed” to 20% to minimize impact and deformation.

Rotate 360° and replicate six times to finish the other holes.

• Finish end cap curves with a D10R1 end mill, skip M6 bolts, then machine bolt areas and chamfer ϕ8 holes (Figure 10).

Conclusion

This paper tackles five-axis pump body machining via process design, fixtures, toolpaths, and programming, achieving:

Five-axis machining with a unified coordinate system ensures positioning accuracy of ≤0.01 mm and tolerance of ≤0.02 mm in a single-setup, multi-directional process.

UG12.0 modular toolpaths with transformations cut programming time for similar complex parts by over 40%.

“3+2” and five-axis finishing reduced upper cover machining time to 35 min—a 35% cut—optimizing efficiency and cost while keeping precision.

Flexible five-axis toolpaths with ≤0.5° vector error and 5°–15° tilt enable deep-cavity machining with Ra < 0.8 μm and ≤0.05 mm deformation.

Layered allowances ≤0.1 mm, 30% corner feed slowdown, and 20% spindle speed reduction at curves improve stability and surface quality.

This paper presents a five-axis workflow optimizing process, programming, and toolpaths for multi-feature parts.

It highlights AI and digital twin verification to replace manual path design, guiding intelligent CNC machining.