14 Frequently Asked Questions in Mold Manufacturing Field [Part 2]

Time:2024-07-10 09:21:41 / Popularity: / Source:

8. Why are round insert milling cutters most often used as the first choice for mold roughing tools?

If a square shoulder milling cutter is used for rough milling of cavity, a large amount of step-shaped cutting allowance must be removed during semi-finishing. This will cause cutting forces to change, causing tool to bend. Result is an uneven machining allowance left for finishing, thereby affecting geometric accuracy of mold.
If you use a square shoulder mill with a weak tip (with a triangular insert), unpredictable cutting effects will occur. Triangular or diamond-shaped inserts also generate greater radial cutting forces, and because insert has a smaller number of cutting edges, they are less economical roughing tools.
Round inserts, on the other hand, can mill in a variety of materials and in all directions. If used, transition between adjacent tool passes will be smoother, you can also leave a smaller and more uniform machining allowance for semi-finishing. One of characteristics of round inserts is that chip thickness they produce is variable. This allows them to use higher feed rates than most other inserts.
Entering angle of round insert changes from almost zero (very shallow cuts) to 90 degrees for a very smooth cutting action. At maximum depth of cutting, leading angle is 45 degrees. When cutting along a straight wall with an outer circle, leading angle is 90 degrees.
This also explains why round insert tool is strong - cutting load gradually increases. Roughing and semi-roughing should always use a round insert mill such as CoroMill 200 (see Mold Making Catalog C-1102:1) as the first choice. In 5-axis cutting, round inserts are very suitable, especially since they have no limitations.
With good programming, round insert mills can largely replace ball end mills. Round inserts with small runout combined with finely ground, positive rake angles and light cutting geometries can also be used for semi-finishing and some finishing operations.
Mold Manufacturing 

9. What is effective cutting speed (ve) and why it is always important for basic calculations of effective cutting speed on highly productive diameters.

Since table feed depends on rotational speed at a certain cutting speed, if effective speed is not calculated, table feed will be calculated incorrectly.
If nominal diameter value (Dc) of tool is used when calculating cutting speed, effective or actual cutting speed will be much lower than calculated speed when depth of cut is shallow. Tools such as round insert CoroMill 200 tools (especially in small diameter range), ball nose end mills, large nose radius end mills and CoroMill 390 end mills (see Sandvik Coromant's mold manufacturing catalog C-1102:1 for these tools).
From this, calculated feed rate is also much lower, which severely reduces productivity. What's more, cutting conditions of tool are below its capabilities and recommended application range.
When doing 3D cutting, diameter changes during cutting, which is related to geometry of mold. One solution to this problem is to define steep wall areas of mold and geometrically shallow part areas. Good compromises and results can be achieved if dedicated CAM programs and cutting parameters are programmed for each area.

10. What application parameters are important for successful milling of hardened mold steel?

When finishing hardened mold steel using high-speed milling, a major factor to adhere to is use of shallow cuts. Cutting depth should not exceed 0.2/0.2mm (ap/ae: axial cutting depth/radial cutting depth). This is to avoid excessive bending of tool holder/cutting tool and to maintain tight tolerances and high precision in mold being machined.
It is also very important to choose a very rigid clamping system and tool. When using solid carbide tools, it is important to use tools with the largest core diameter (maximum bending stiffness). A rule of thumb is that if you increase diameter of a tool by 20%, say from 10mm to 12mm, bending of tool will decrease by 50%.
It can also be said that if tool overhang/protrusion is shortened by 20%, bending of tool will be reduced by 50%. Large diameter and tapered shank further increases stiffness. When using a ball end mill with indexable inserts (see mold manufacturing sample C-1102:1), if tool holder is made of solid carbide, bending rigidity can be increased by 3-4 times.
When finishing hardened mold steel with high-speed milling, it is also important to select a specific geometry and grade. It is also very important to choose a coating with high thermal hardness like TiAlN.

11. When should we use down milling and when should we use up milling?

Main advice is: use climb milling as much as possible.
In climb milling, chip thickness can reach its maximum value when cutting edge is just cutting. In reverse milling, it is minimum value. In general, tool life is shorter in up milling than in down milling because heat generated in up milling is significantly higher than in down milling. When chip thickness increases from zero to maximum in up milling, more heat is generated because friction experienced by cutting edge is stronger than in climb milling. Radial forces are also significantly higher in up milling, which has a negative effect on spindle bearings.
In down milling, cutting edge is mainly subjected to compressive stress, which has a much more favorable effect on carbide inserts or solid carbide tools than tensile forces generated in up milling. Of course there are exceptions. When using a solid carbide end mill (see tool in tooling sample C-1102:1) for side milling (finishing), especially in hardened materials, up milling is preferred.
This makes it easier to achieve tighter tolerances for wall straightness and better 90 degree angles. If there is any mismatch between different axial tool passes, cutting marks will be very small. This is mainly due to direction of cutting forces. If a very sharp cutting edge is used in cutting, cutting force will tend to "pull" knife toward material. Another example where up milling can be used is when milling with an older manual milling machine that has a larger lead screw with a larger clearance. Up-milling generates cutting forces that eliminate gaps, making milling action smoother.

12. Copy milling or contour cutting?

In cavity milling, the best way to ensure a successful climb milling toolpath is to use a contour milling path.
Contour milling of outer circle of a milling cutter (such as a ball end mill, see Mold Making Sample C-1102:1) often results in high productivity because there are more teeth cutting on a larger tool diameter. If speed of machine tool spindle is limited, contour milling will help maintain cutting speed and feed rate.
With this tool path, workload and direction changes are also small. This is particularly important in high-speed milling applications and processing of hardened materials. This is because if cutting speeds and feeds are high, cutting edge and cutting process are more susceptible to adverse effects from changes in workload and direction, which can cause changes in cutting forces and tool bending. Copy milling along steep walls should be avoided whenever possible. When copying milling, chip thickness is large at low cutting speeds.
In the center of ball-nosed knife, there is also danger of blade chipping. If control is poor, or machine tool does not have a pre-reading function, it will not be able to decelerate quickly enough, and risk of edge breaking is most likely to occur in the center. Up profile milling along steep walls is better for cutting process because chip thickness is at its maximum at favorable chip speeds.
In order to get the longest tool life, cutting edge should be kept cutting continuously for as long as possible during milling process. If tool enters and exits too frequently, tool life will be significantly shortened.
This increases thermal stress and thermal fatigue on cutting edge. Modern carbide tools are more beneficial to have uniform and high temperatures in cutting area than large fluctuations. Copy milling paths are often a mixture of up and down milling (zigzag), which means frequent engagement and retraction during cutting. This tool path also has a negative impact on mold quality.
Every time knife is struck, it means that knife is bent and there will be a raised mark on the surface. As the tool exits, cutting forces and tool bending decrease, and there is a slight "overcut" of material in exit portion.
Mold Manufacturing 

13. Why do some milling cutters have to have different tooth pitches?

Milling cutters are multi-cutting edge tools and number of teeth (z) is variable. There are some factors that help determine the pitch or number of teeth for different types of machining.
Materials, workpiece size, overall stability, overhang dimensions, surface quality requirements and available power are factors related to processing. Tool-related factors include adequate feed per tooth, having at least two teeth cutting at the same time, and chip capacity of tool, to name just a few.
Pitch (u) of a milling cutter is distance from a point on cutting edge of insert to same point on next cutting edge. Milling cutters are divided into sparse, dense and super-fine pitch milling cutters. Most Coromant milling cutters have these three options, see mold manufacturing sample C-1102:1. Close pitch means there are more teeth and adequate chip space, allowing cutting at high metal removal rates. Generally used for medium load milling of cast iron and steel. Fine pitch is the first choice for general purpose milling cutters and is recommended for mixed production.
Sparse pitch means there are fewer teeth and a large chip space on circumference of milling cutter. Sparse pitch is often used from rough machining to finishing of steel. In steel machining, vibration has a great influence on machining results. Coarse pitch is a real problem solver and is the first choice for long overhang milling, low power machines or other applications where cutting forces must be reduced.
Ultra-fine pitch cutters have very little chip space and can use higher table feeds. These tools are suitable for cutting interrupted cast iron surfaces, roughing cast iron and small stock removals of steel, such as side milling. They are also suitable for applications where cutting speeds must be kept low. Milling cutters can also have uniform or unequal tooth pitches. The latter means that teeth on tool are not equally spaced, which is also an effective way to solve vibration problem.
When vibration problems exist, it is recommended to use sparse-tooth unequal pitch milling cutters whenever possible. With fewer blades, there is less chance of increased vibration. Small tool diameters can also improve this situation. A combination of geometry and grade that works well should be used - a combination of a sharp cutting edge and a tough grade.

14. In order to obtain the best performance, how should milling cutter be positioned?

Cutting length is affected by position of milling cutter. Tool life is often related to length of cut cutting edge must bear. A milling cutter positioned in the center of workpiece has a short cutting length. If milling cutter is deviated from center line in any direction, cutting arc will be long.
Remember, how cutting forces act, there must be a compromise. With tool positioned in the center of workpiece, direction of radial cutting force changes as insert cutting edge enters or exits cut. Clearance in machine tool spindle also intensifies vibration, causing blade to vibrate.
By off-centering tool, a constant and favorable cutting force direction is obtained. The longer overhang, the more important it is to overcome all possible vibrations.
Another beneficial effect of constant machining stock is low negative impact on machine tool - guide rails, ball screws and spindle bearings.

Go To Top