UGNX Academy

Tag: Toolpath Optimization

  • Siemens NX Dynamic Milling in Practice: Master Wang Teaches You Toolpath Optimization, Risk Mitigati

    📝 Key Takeaways: ** Master Wang guides you through Siemens NX Dynamic Milling, from cutting strategies to parameter optimization. He’ll show you step-by-step how to avoid the notorious “fragile central remnant” during machining, achieve safe and efficient “hole-milling style” center material removal, and enhance machining accuracy and efficiency for complex parts through refined non-cutting move management. **

    In-Depth Analysis of Dynamic Milling Strategies

    Initial Stock Handling and Toolpath Direction

    Master Wang: “Listen up. Last lesson, we discussed tool engagement length. With dynamic milling, you’ve got to understand the actual condition of your raw material stock. Especially when the stock height exceeds the programmed start plane, the tool must begin cutting from above – that’s common sense. Siemens NX will automatically plan the initial entry point based on your defined stock information. But that’s just the basic setup; the real magic comes later.”

    Risks of Traditional Helical Milling

    Master Wang: “Take a look at this diagram, especially when performing Corner Cleanup or machining deep cavities. If we stick to the default helical milling strategy, it spirals outwards layer by layer. It looks like it’s clearing the material, but the problem arises at the very end, especially when you reach the center, where it can leave behind a ‘fragile central remnant.’ This thing is like an isolated island, with no support. If the tool sweeps across it, at best it’ll get knocked off, spraying chips everywhere. At worst, it’ll cause tool breakage or even damage the workpiece. This is serious business, understand? Core Pain Point: Default helical milling often leaves a thin-wall ‘fragile central remnant’ in the center area, which can easily shatter, damaging the tool and the part.“

    “Hole-Milling Style” Center Material Removal

    Master Wang: “So, when you encounter this situation, we need to switch our approach. Just like we mill a hole, we need to ‘mill out’ the material in the center, spiraling from top to bottom. In Siemens NX, we can switch to this mode, and it won’t leave that ‘fragile central remnant’ in the middle. The tool will act like a drill, first plunging to the bottom, then spiraling upwards or downwards to lift and cleanly remove all the remaining material from the entire central area. This method is safe, stable, and good for both the tool and the workpiece. Solution: Employ a ‘hole-milling style’ center material removal strategy to ensure residual material is safely removed from the center outwards, avoiding thin-wall remnants.“

    Practical Siemens NX Parameter Optimization Techniques

    Cutting Direction and Toolpath Generation

    Master Wang: “Next, let’s talk about toolpath direction. In Siemens NX dynamic milling, there’s a ‘Transform Direction’ option. By default, it’s usually climb milling, where the tool’s cutting direction is the same as the feed direction, ensuring stable cutting and good chip evacuation. But if you set this percentage to 50%, it will switch between climb milling and conventional milling. The toolpath might look ‘prettier’ and run ‘smoother,’ reducing the number of retracts. But old Master Wang here has to warn you, this is not recommended for all materials. For some materials, like titanium alloys and superalloys, conventional milling can lead to work hardening, increased tool wear, and even chipping. So, unless you have absolute confidence in the material properties and tool performance, it’s generally advisable to maintain a single climb milling direction to ensure machining stability. This is a lesson from experience that textbooks might not emphasize.”

    NX Parameter Path: Connect -> Tool Path -> Transform Direction (Step %)

    Non-Cutting Moves: Refined Control of Retract Height

    Master Wang: “Next up are non-cutting moves, which we often call ‘retracts’ or ‘lifts.’ In 2D dynamic milling, I’ve talked about ‘Retract Distance’ and ‘Large Distance.’ In 3D, these two parameters are integrated. Specifically, this ‘Rapid Transfer‘ parameter controls the tool’s retract height when moving between adjacent cutting regions. The default value might be set very high, say 100mm. Think about it, if you retract that high for every transfer, your air cutting time becomes excessive, completely wasting efficiency! Unless the raw stock is unusually tall or there are obstacles, I generally recommend setting it to 3mm or 5mm, or even 1mm is often enough. Go as low as possible; that’s how you squeeze out efficiency.”

    NX Parameter Path: Non-Cutting Moves -> Rapid Transfer -> Retract Height

    Safe Initial/Final Retracts and Efficient Intermediate Transfers

    Master Wang: “But there’s a pitfall here, listen closely! If you set the ‘Rapid Transfer’ too low across the board, then the retracts for the very first cut and the very last cut will also be low. If the safety clearance isn’t sufficient for the first cut onto the workpiece, you’re looking at a collision. The same goes for the last cut: if the program finishes with the tool at a low position, an operator might accidentally bump it. So, we need to balance safety and efficiency. The solution is this: In ‘Non-Cutting Moves,’ find the ‘Initial‘ and ‘Final‘ retract settings. Change their type from ‘Relative to Plane’ to ‘Absolute,’ and then set both to 100mm (or a higher safe value). This way, at the start and end of the program, the tool will safely retract to a high position, while intermediate rapid transfers will use our defined low retract (e.g., 3mm), ensuring efficiency. Now that’s experienced operating!”

    NX Parameter Path: Non-Cutting Moves -> Initial/Final -> Type changed to “Absolute” -> Distance set to 100

    Advanced Application: Creating In-Process Workpiece (IPW)

    Understanding the Function and Significance of “Create Workpiece”

    Master Wang: “After the program runs, you might need to machine the next operation, or perhaps flip the part for machining. Siemens NX has a very practical function here called ‘Create Workpiece.’ After a simulation, you can click ‘Create,’ and it will generate an independent geometric body representing the remaining material after the current program is finished. What’s the use of this, you ask? It’s simple: it becomes the ‘stock’ for your next operation! For example, after milling one side, you generate this workpiece. Then, you flip the part and directly set this generated workpiece as the initial stock for the second side. This avoids repetitive measurements and ensures more accurate data. For multi-sided machining and fine-finishing complex surfaces, this is an absolute game-changer, greatly improving programming efficiency and subsequent machining accuracy!”

    NX Function Path: After Simulation -> Create (Create Workpiece)

    Summary: Pitfall Avoidance Guide

    • Beware of the “Fragile Central Remnant”: When dynamic milling deep cavities or performing Corner Cleanup, pay close attention to whether the toolpath might leave a “fragile central remnant” of material in the center area. This residual material is extremely unstable and can easily be knocked off by high-speed tool cutting, leading to tool breakage, workpiece damage, or even safety hazards. Always switch to a “hole-milling style” or similar strategy to ensure safe removal of central residual material.

    • Don’t Blindly Set Retract Height: Never allow the tool to retract too high during intermediate rapid transfers; otherwise, excessive air-cutting time will severely reduce efficiency. Based on actual conditions, set the ‘Rapid Transfer‘ to a low value of 3-5mm, or even 1mm, to minimize air time and boost overall efficiency.

    • Initial and Final Safety Are Non-Negotiable: When setting intermediate transfer retracts, remember to separately configure the ‘Initial‘ and ‘Final‘ retracts to a safe height (e.g., 100mm). This ensures the tool starts from a safe high position at the beginning of the program and safely retracts from the workpiece at the end, preventing collision risks due to low-position entry or low-position program completion.

    • Cleverly Utilize Workpiece Linking: For multi-operation or multi-sided machining, you must use the ‘Create Workpiece‘ function after simulation. Generating the remaining material from the current operation as the initial stock for the next operation will significantly improve the accuracy and efficiency of subsequent programming. This is an essential skill for complex part machining.

    • Cutting Direction is Not Trivial: Switching between climb milling and conventional milling should not be done casually. While mixing both directions might make the toolpath appear “prettier,” conventional milling can lead to work hardening and rapid tool wear when machining special materials. Until thoroughly validated, maintaining a single climb milling direction is often more stable and safer.

    👤 About the Author:
    The author is a veteran CNC machining professional with 15 years of industry experience, specializing in UG NX programming. This article is an original work representing personal practical insights.

    ⚠️ Copyright Notice: Unauthorized reproduction or distribution without prior communication is strictly prohibited.

  • UG NX 1980 Cutting Parameter Strategy & Stock Management Tutorial

    📝 Key Takeaways: Master Wang provides a hands-on tutorial for setting cutting parameter strategies and stock in UG NX 1980. Learn how to select cutting directions, control undercut, and precisely manage various stock allowances to avoid common mistakes and improve efficiency and accuracy in real-world machining.

    Hello everyone, I’m Master Wang. Let’s pick up where we left off. Once we cover this section today, we’ll have basically wrapped up this page of work.

    Cutting Strategy: More Than Just Direction

    Let’s open up Cutting Parameters. There are quite a few commands in here, so we need to break them down one by one. First, let’s look at the ‘Strategy’ section.

    Cutting Direction: Climb vs. Conventional Milling, Different Jobs

    Initially, you’ll see a cutting direction, mainly referring to the Cutting Angle. When it’s moving in the negative direction, this cutting angle appears. It’s actually quite simple: it’s either climb milling (順銑) or conventional milling (逆銑).

    Typically, we mostly choose climb milling. We rarely opt for conventional milling. However, in special working conditions, conventional milling does have its place. Just remember these two methods; climb milling is generally sufficient.

    Automatic Cutting Angle: The Software’s ‘Cleverness’

    Have you ever noticed that at the beginning of a program, the tool always starts cutting from a specific direction, then follows a certain path? For instance, why does it always start cutting from this direction, and not the opposite? This is the result of automatic control of the cutting angle.

    Click it, and you’ll see a bunch of options like ‘Specify’, ‘Longest Edge’, ‘Fixed Vector’, ‘Receive Vector’. Don’t panic, we’ll start with the most commonly used ones.

    For example, choose Fixed Vector (Specify Vector). Click it, and you’ll see four directional arrows on the part. Click on any directional arrow, say this one, then ‘Specify’, and generate the toolpath. You’ll notice:

    • If you select a vertical arrow, the tool will perform vertical machining.
    • If you select a horizontal arrow, the tool will perform horizontal machining.

    In short, this command is used to change the machining direction, whether it’s milling horizontally or vertically, you decide. If you deselect the specified vector, it will revert to automatic determination.

    Specify Angle: Fine Control for Multi-Axis Machining

    Let’s look at ‘Angle’ within ‘Specify’. When the angle is 0 degrees, the toolpath is horizontal. If we change the angle to 90 degrees, and look at the arrow, it’s clearly pointing upwards, and the tool will machine vertically.

    This function simply allows you to change the tool’s machining direction. You can also try 45 degrees, which can also machine, but in actual work, we rarely use such diagonal machining methods; most of the time, it’s either horizontal or vertical.

    So, the meaning of ‘Cutting Angle’ is to let you control the tool’s path. Those parameters we didn’t cover are generally less used in face milling, and in most cases, automatic mode is sufficient.

    Add Finishing Pass: A ‘Redundant’ Feature for Face Milling

    The ‘Add Finishing Pass’ option below is generally not very useful for face milling. We can ignore it for now.

    Allow Undercut: A ‘Sharp Tool’ for Deep Cavities

    Here’s an important one! As soon as you turn on ‘Allow Undercut’, you’ll see the effect. Look at this small icon: the first pass is fine, but what about the second?

    Did you notice that it has overcut, milling away the entire side wall? This is the function of ‘Allow Undercut’; it enables the tool to machine into internal corners of a part, even cutting into areas smaller than the tool’s diameter.

    If you don’t allow undercut, it will only follow the largest outer contour, unable to reach deeper or narrower areas. Of course, if you’re using a special tool like a T-slot cutter, allowing undercut for machining side walls is perfectly fine.

    However, typically, to avoid unnecessary overcutting, we do not enable ‘Allow Undercut’ unless you have specific machining requirements, such as machining undercuts or reverse angle slots.

    Cutting Mode and Toolpath Direction: Choosing Your Strategy

    When we change the ‘Strategy’ to ‘Follow Part’, you’ll notice the Cutting Angle option disappears. Why? Because it doesn’t involve whether you’re machining horizontally or vertically, so naturally, this option isn’t there; only ‘Climb’ and ‘Conventional’ directions remain.

    This teaches us a principle: the ‘Strategy’ is determined by the ‘Cutting Mode’ we select. For example, if we change to ‘Follow Periphery’ and generate the toolpath again, you’ll find an additional option: ‘Inward’ or ‘Outward’.

    • Inward: The tool machines from outside to inside, gradually moving inwards.
    • Outward: The tool machines from inside to outside, clearly moving diagonally outwards.

    Therefore, when you choose ‘Follow Periphery’, you can flexibly select ‘Inward’ or ‘Outward’ toolpath directions.

    Option B: The Secret Weapon for Corner Cleanup

    In ‘Follow Periphery’ mode, an additional Option B will appear. What does this B mean? Typically, if you check it, you’ll find that the toolpath includes some ‘corner cleanup toolpaths’.

    Especially when machining certain corners, if your Corner Cleanup (Option B) is not enabled, you might find that some areas are not machined. In this case, enabling it can resolve the issue.

    However, if your machining is simply basic face milling and doesn’t require corner cleanup, there’s no need to enable Option B.

    Stock Settings: Key to Accuracy and Efficiency

    Now that we’ve covered strategy, let’s move on to ‘Stock’. This is crucial for part accuracy and machining efficiency!

    There’s ‘Part Stock’, ‘B Stock’, ‘Floor Stock’, ‘Blank Stock’, ‘Touch Point Stock’, ‘Inner Tolerance’, ‘Outer Tolerance’, and so on. Let’s go through them one by one.

    Part Stock: How Much to Leave on Side Walls?

    ‘Part Stock’ is simply how much stock we leave on the side walls of the specified part. Look at this image, the blue side wall. If we change the Part Stock to 0.2mm, it means we’ve left 0.2mm of stock on the side wall.

    This is crucial during roughing to leave some material for the finishing pass, preventing insufficient accuracy or excessive tool wear from trying to finish in one go.

    B Stock: Dedicated Stock for Special Features

    ‘B Stock’ refers to the stock left for the specified B entity. Since we haven’t selected a B entity yet, this B Stock is currently unused and remains 0. We typically don’t use B entities for machining, so we can skip this for now.

    Floor Stock: How Much to Leave on the Bottom?

    The stock for the ‘Specify Final Floor’, this one is quite easy to understand. For instance, set it to 0.2mm.

    Let’s replay the toolpath and then measure. See, the distance between the machined surface and our specified floor is clearly 0.2mm. This is the Floor Stock.

    In practical work, you don’t need to measure every time. Once you’ve set it correctly and you see that stock is clearly left, then it’s accurate. This relates to our Percentage of Tool parameters; if the percentage is not set reasonably, the toolpath will appear very dense.

    Summary: Strategy and Stock are Interconnected

    We’ve pretty much covered the ‘Strategy’ and ‘Stock’ pages in the cutting parameters. The remaining commands, like ‘Connect Mold Toolpath’, are less used in face milling, so we can skip them for now.

    Remember one thing: all these strategy and stock settings must be flexibly adjusted according to your actual workpiece, material, and machining requirements. There are no one-size-fits-all parameters, only the most suitable configuration for the current task.

    Summary: Pitfall Guide

    • Cutting Direction: Mostly climb milling, conventional milling for special cases, but be cautious to avoid chatter.
    • Cutting Angle: Adjust toolpath direction based on whether the machining surface is horizontal or vertical, to improve efficiency.
    • Allow Undercut: Only enable when machining deep cavities or undercuts; otherwise, use sparingly to prevent overcutting.
    • Strategy and Cutting Mode: Strategy options change with the cutting mode; understand their interrelationship.
    • Option B (Corner Cleanup): Only enable when corner cleanup is needed, to avoid unnecessary calculations and toolpaths.
    • Part/Floor Stock: Set precisely according to roughing and finishing requirements to ensure smooth subsequent operations and avoid undercutting or overcutting.
    • Coordinate System: MCS (Machine Coordinate System) is the datum; WCS (Work Coordinate System) can be placed anywhere without affecting machining.
    • Parameter Fine-tuning: In actual machining, parameters may need fine-tuning based on machine status, tool wear, etc. Don’t just rely on software simulation; watch the cutting sparks and observe the actual results!