[VIDEO_HERE]

Hello everyone, I’m Old Wang, Engineer Wang. Today, let’s continue our discussion on machining multi-process parts. Listen up, this isn’t a job you can do with your eyes closed; it’s all about experience and attention to detail. Let’s start from the beginning and talk about machining the front face (Face A).

Roughing Strategy and Tool Path Optimization for the First Face

Fixturing and Workpiece Positioning

First, workpiece clamping. For roughing the front face (Face A), we’ll start by securing the raw material firmly with a vise. Why? Because roughing involves high cutting forces, and poor rigidity can easily lead to chatter, or even tool ejection, which would cause serious trouble. Positioning must be precise, and datums must be clear; this is the foundation for all subsequent precision machining.

Roughing Tool Selection and Feed Strategy

I just repositioned the tool start point; I accidentally clicked the wrong location earlier. We’ll continue roughing with a large-diameter flat-bottom tool with a corner radius (either a ball nose end mill or a corner radius end mill). For instance, here, we’ll choose a Φ32mm (approx. 1.26 inch), R0.8mm (approx. 0.03 inch) corn end mill, or a large face mill with a corner radius. This type of tool balances cutting efficiency and strength. The corner radius effectively distributes cutting stresses, extends tool life, and reduces stress concentration at sharp corners. For the tool path, the Depth of Cut (DOC) is set to 2mm (approx. 0.08 inch). However, we’ll initially leave a bottom stock of 0.8mm (approx. 0.03 inch), and some on the sides as well. This is to provide sufficient material for finishing, preventing the finishing tool from taking heavy impacts directly.

For the tool path, we’ll start with a Zig-zag pattern to quickly remove most of the material. If the tool path doesn’t feel ideal—for example, too many air cuts or unstable machining—we need to adjust it. Siemens NX offers many strategies. Don’t just rely on software simulation; consider whether the cutting sparks on the actual machine are consistent and if the sound is smooth. No matter how advanced the software, it can’t fully replace the ears and eyes of an experienced machinist.

Tool Path Optimization to Avoid Excessive Tool Engagement

As mentioned, if the tool path strategy isn’t ideal, we need to adjust it. For example, switching from a Zig-zag pattern to an Offset pattern. The offset pattern provides more uniform tool engagement along the contour edges, preventing the tool from engaging too deeply in corners, which can lead to chipping or workpiece deformation. Especially when machining near edges, if a zig-zag pattern tends to cause overcutting or vibration, an offset pattern offers better control over cutting forces. We’ll set the Stepover to 85% of the tool diameter. This ensures both efficiency and sufficient material allowance for the finishing pass.

After machining, check the part. We’re left with a bottom stock of 0.15mm (approx. 0.006 inch), which is an acceptable size, making it convenient for the subsequent single-pass finishing operation.

Finishing and Detail Processing for the First Face

Finishing Stock Control

Once roughing is complete, it’s time for finishing. As usual, copy the roughing program and then modify the parameters. Finishing stock must be strictly controlled, with all allowances set to 0. However, pay attention: some side walls require a separate finishing pass with a smaller tool. Therefore, we can temporarily leave 0.25mm (approx. 0.01 inch) on the side walls. Don’t remove everything in one go; that can easily lead to “tool deviation” or failure to meet surface finish requirements.

Planar Contour Milling and Boundary Control

In Siemens NX, for finishing flats and contours, the “Planar Mill” or “Contour Mill” strategies are commonly used. If the workpiece contour is complex or has open boundaries, we cannot simply use a zig-zag pattern. We must use Planar Contour Milling and properly define the cutting region (face or curve) and boundary type (open or closed). For example, here, we’ll set the cutting direction for one open area to “Right” and another to “Left”, ensuring the tool path covers the entire area without cutting into unintended regions.

We’ll still use the Φ32mm (approx. 1.26 inch), R0.8mm (approx. 0.03 inch) tool. Set the Depth of Cut (DOC) and stock allowance to 0, which means a single pass to the final depth, finishing the bottom face. This completes the large-area finishing.

Side Wall Finishing and Dedicated Tools

The side walls we mentioned earlier still have 0.25mm (approx. 0.01 inch) of stock remaining; now it’s their turn. These side walls typically require a better surface finish or smaller radii. We’ll need to switch to a small-diameter flat end mill, such as a Φ10mm (approx. 0.39 inch) flat tool, or even a smaller one for the finish cut. Set the stock allowance to 0, and change the cutting method to “Along Boundary” or “Follow Profile”. With a single pass, machine the side wall cleanly. This ensures both surface finish and perpendicularity. Don’t underestimate this 0.25mm allowance; it’s your margin for error, preventing large steps or damage from occurring during roughing with a larger tool.

When finishing side walls, pay attention to the tool stick-out length. If the tool protrudes too far, it can easily lead to chatter, affecting surface finish, or even cause tool breakage. Therefore, keep it as short as possible. Here, my tool stick-out is a bit long, but for demonstration purposes, we’ll proceed as is. In actual machining, I would try to shorten the stick-out length as much as possible or opt for a reinforced tool holder.

Hole Machining: Preparation Before Drilling and Tapping

Hole Recognition and Optimized Drilling Sequence

After machining the faces, next come the holes. Hole machining cannot be careless, especially when high dimensional accuracy is required. Siemens NX’s “Hole Machining” module is very powerful and can automatically recognize all holes. What we need to do is optimize the drilling sequence to minimize air cuts. Drill smaller holes first, then larger ones, or go from inside to outside, or high to low. This avoids multiple tool changes and unproductive movements, saving time and thus cost!

First, use a center drill (or spot drill) to spot the holes for positioning and to prevent the drill bit from wandering. Then, use a twist drill for drilling the holes. Here, we’ll select a center drill to spot the hole locations.

“Drawing is King” Principle for Drilling Depth and Dimensions

After spot drilling, proceed with drilling. Here, I checked the hole diameter and found it to be 6.8mm (approx. 0.268 inch). This is clearly the pilot hole for an M8 thread. This means that after drilling this hole, an M8 thread will need to be tapped. The hole depth is absolutely subject to the “drawing is king” principle! Some holes are through holes, others are blind holes, and their depths vary. Never rely on intuition; always carefully cross-reference the drawing for each hole’s depth and requirements. If the drawing specifies a flat bottom for a blind hole, then a flat-bottom drill must be used for machining.

For demonstration, I’ll set a random depth for now. But during actual operations, better slow than wrong! Especially before tapping, the pilot hole’s size and depth are critical. If the pilot hole is too small, tapping can easily break the tap; if it’s too large, the thread strength will be insufficient. These are lessons learned the hard way.

Here, we’re just outlining how to program it. But for actual machine operation, you must be even more diligent, striving for perfection, especially regarding depth and tool life.

Flip Machining: Establishing and Inheriting the Second Face Datum

Datum Face Selection and Workpiece Preparation

With the front face machined, it’s time to flip the part and machine the back face (Face D). The most critical aspect of flip machining is the establishment and inheritance of datums. We typically choose a previously machined, high-accuracy face as the secondary datum face for clamping. If the raw material edges have a large amount of stock from roughing, they can even be lightly cleared on a manual milling machine before CNC finishing. This ensures better clamping stability.

I checked the raw material condition of the back face (Face D), and it’s quite similar to the previous Face B (side face). Can we directly reuse the tool path from Face B? After analysis, if the stock allowance and geometry are essentially identical, then absolutely!

Tool Path Reuse and Parameter Adjustment

Since the back face and Face B are similar, we’ll directly copy the roughing program from Face B. But remember, the face must be updated to select the new back face as the machining surface. Tool parameters and stock allowance will follow the previous Φ32mm (approx. 1.26 inch), R0.8mm (approx. 0.03 inch) tool, ensuring ample stock. While tool path reuse is convenient, the actual conditions of each face and each hole may differ, so parameter adjustment is essential—no cutting corners!

One point to note here is the choice between Perpendicular to tool axis and Parallel to tool axis. When machining inclined or curved surfaces, this option directly affects the tool’s cutting posture and efficiency. Here, we’ll simply select a face and let the software automatically generate the path. During machining, do not use a Reciprocate (zig-zag) pattern; instead, follow the contour directly. This will result in more stable cutting.

After roughing is complete, check again if there are any areas still needing roughing. Oh, right, the side faces and internal holes haven’t been roughed yet!

For these internal holes, we can perform roughing using a Helical Ramp method, or directly use Trochoidal Milling, as long as it doesn’t damage the tool and is efficient. We’ll still use the Φ32mm (approx. 1.26 inch), R0.8mm (approx. 0.03 inch) tool. The Depth of Cut (DOC) can be larger, for example, 21.5mm (approx. 0.85 inch) (I deliberately went a bit deeper here; actual depth should be based on the drawing), leaving a 0.2mm (approx. 0.008 inch) stock allowance. The entry and exit paths must also be adjusted for safety. Pay attention to tool stick-out length; mine is a bit long here, but it should be shortened for actual operation.

Finishing Strategy for Blind Holes and Irregular Holes

For blind holes or irregular holes that may appear on the back face, the finishing strategy is similar to the front face. First, use a small-diameter flat end mill to finish the side walls, ensuring perpendicularity and surface finish. For blind hole bottoms, if high precision is required, a bottom corner cleanup tool must be used for corner cleanup to ensure a flat bottom. These details are crucial for determining the final product accuracy. Remember, ±0.005mm (approx. ±0.0002 inch) accuracy is achieved through this cumulative attention to detail and optimization.

Summary: Pitfall Avoidance Guide

Alright, today we’ve covered the roughing and finishing of multi-process parts, as well as hole processing. Finally, I’ll summarize a few points for you—these are pitfall avoidance experiences gained from hands-on practice:

1. Datum First, Secure Clamping: Any machining operation must start from the most stable and precise datum. Poor clamping renders all efforts futile. During roughing, ensuring rigidity is even more critical.
2. Stock Control, Distinct Stages: Leave sufficient stock for roughing, then uniformly remove it during finishing. Don’t attempt a single-pass finish; that will only lead to a loss of both accuracy and surface quality. Typically, roughing leaves 0.15-0.5mm (approx. 0.006-0.02 inch), and finishing leaves 0.05-0.1mm (approx. 0.002-0.004 inch). For special materials like titanium alloys and high-temperature nickel-based alloys, stock control must be even more cautious due to their severe work hardening tendency.
3. Tool Selection, Material-Specific: Different materials and different machining stages require different tools. For example, a Φ32mm (approx. 1.26 inch), R0.8mm (approx. 0.03 inch) tool is efficient for roughing; a Φ10mm (approx. 0.39 inch) flat end mill is suitable for finishing side walls and corner cleanup. Don’t expect one tool to do everything; that’s impossible. For high-temperature alloys, carbide tools must be used, and cutting parameters should be slow to prevent chipping.
4. Tool Path Optimization, Balancing Efficiency and Stability: The tool path generated by the software isn’t necessarily optimal; always combine it with real-world considerations. Minimize air cuts, avoid sharp turns, and maintain stable cutting forces. For thin-walled or easily deformable parts, consider gradual cutting strategies, or even multi-layer machining.
5. Drawing is King, Verify Dimensions: Never guess dimensions based on experience, especially for hole depth, diameter, and position. The drawing is your bible; cross-reference it repeatedly before machining.
6. Combine “See, Hear, Feel”: Don’t just stare at the NX simulation on the screen. On the actual machine, observe the color and shape of the cutting sparks, whether the cutting sound is smooth, and if the chip formation is normal. This is real skill you won’t learn from books. If the cutting sparks are white or the sound is harsh, it usually indicates tool wear or unsuitable parameters.
7. Prevent Heat Treatment Deformation: If the workpiece requires heat treatment, machining allowances and clamping methods must be considered in advance, reserving sufficient finishing stock to compensate for deformation.
8. Accuracy Compensation: When dealing with accuracies of ±0.005mm (approx. ±0.0002 inch), machine tool inherent errors, tool wear, and ambient temperature can all have an impact. Siemens NX allows for tool compensation, cutter compensation, and even direct fine-tuning in the G-code. However, the best approach is to optimize processes and parameters at the source to minimize cumulative errors.

In our line of work, you can’t just know how to push buttons; you need to understand why you’re pushing them. These tricks of the trade are accumulated through time and expense. I hope you all avoid unnecessary detours!