Boring Systems
Explore our comprehensive range of CNC boring systems, featuring versatile solutions such as boring heads, cartridges, boring holders, and extensions. Our CNC boring systems offer superior rigidity, concentricity, and adaptability, ensuring optimal performance in various boring applications.
Haas Boring System
The Haas Boring System is designed for use with milling machines and consists of tool holders, one or more extensions (if necessary), rough bore heads for roughing operations, and finish bore heads for finishing operations. Each bore head takes cartridges that hold carbide inserts, which are what perform the cutting operation. A few boring heads take a range of different cartridges to expand the boring range of the head. Collectively, the Haas Boring System can bore holes from 20mm (0.787”) to 154.1mm (6.0669”).
- Produces precise, tight tolerance holes.
- Interchange a range of different heads and cartridges to bore holes from 20mm (0.787”) to 154.1mm (6.0669”) diameter.
- Add optional extension bars to increase depth capability.
- Fine bore heads allow precise adjustments down to 2 microns (.00008”).
Boring is the process of enlarging a pre-existing hole and is used to achieve greater accuracy of the diameter and location of a hole. Drills tend to “walk” or “deflect” a little bit when cutting a hole. This can produce holes that are “bell-mouthed” meaning the diameter is larger at the top of the hole and smaller at the bottom of the hole.
The boring process can enlarge a drilled hole and eliminate the location error, taper, and bell-mouth conditions of drilled holes. This, along with precise adjustments down to 2 microns (.00008”) on the finish boring heads makes boring the best way to produce precise, tight tolerance holes.
1. Pull Stud | 2. Basic Holder |3. Rough Bore Head | 4. Rough Cartridges | 5. Fine Bore head | 6. Fine Cartridge | 7. Optional Extension Bar
Rough Boring Heads
Rough Bore heads have a twin-bore configuration and are used for rough boring holes. They are capable of removing up to 10% of the final bore diameter. The heads come in 5 sizes but they all share the same characteristics. They use two cartridges that each hold a carbide insert. Each cartridge can be individually adjusted. They should be adjusted to the same diameter, producing a “two-flute” boring tool. Symmetrical adjustment of the two cartridges produces the best concentricity.
Drilled holes or holes produced by other means such as end milling may lack the precise location required of tight tolerance holes. In such cases, it is beneficial to use a rough boring head to produce bored holes that are spot-on location and leave a consistent amount of stock for the fine or finish boring head to produce high-tolerance bores with very accurate location, near-perfect roundness, and excellent surface finish.
Chip control is key in rough boring applications, especially when boring blind holes. If there is no place for the chips to evacuate the bore, it is extremely important that the chips are broken and flushed out of the bore. All Haas boring heads are equipped with holes for through-tool coolant. If your machine is equipped with a through spindle coolant option, use it!
- Twin bore configuration
- Capable of removing up to 10% of the final bore diameter
- Heads come in 5 sizes
- Each cartridge can be individually adjusted
- Produces high-tolerance bores with very accurate location
- Equipped with holes for through-tool coolant
Rough Boring Cartridges should be arranged symmetrically for the best concentricity. They can remove up to 10% of the final bore diameter. Program the feed rate as a two-flute cutter.
(D1 minimum = D*0.9)
Ajusting Boring Diameter
The task of setting the boring head diameter is easy and accurate when performed using a tool pre-setter like the Haas HTS-400. It allows you to set the correct diameter and adjust both cartridges to the same diameter for consistent, balanced stock removal and the best concentricity.
Follow the steps below to adjust the boring diameter.
- Turn the LOCK SCREW counterclockwise to release the lock (see image 1)
- Move the ADJUST SCREW clockwise using the WRENCH to increase the BORING DIAMETER. (see image 2)
- Each graduation on the scale is approximately 0.0787” or 2mm diameter. (see image 3)
- Turn the LOCK SCREW clockwise to lock the cartridge in place (see image 4)
- The CARTRIDGE on the other side is also operated in the same way as in steps 1, 2 & 4. Set the cartridge to the same position on the scale.
Perform a rough boring operation. - Measure the bore diameter. If the diameter is smaller than the tolerance after measurement, repeat steps from 1 to 6 above to adjust the bore diameter.
Finish Boring Heads
Finish Boring heads, also referred to as fine boring heads, are used to produce high-precision bored holes. The amount of stock removal should be limited to the size of the nose radius on the carbide insert. Also, stock removal should not be less than one-half of the nose radius. See more details below.
If the drilled or cast hole to be bored is within that diameter range determined by the size of the nose radius, the finish boring head can be used to finish the bore. If there is more stock in the hole, the stock must be removed before finishing the bore. The stock can be removed with a variety of cutting tools including end mills and shell mills. For deeper holes, use a twin-bore roughing tool to produce the best results before finishing.
Steps to setting for the finish boring head for high precision results.
- Loosen the set screw to unlock the graduated dial. (see image 1)
- Adjust the approximate diameter on the graduated dial. (see image 2)
- Each division on the graduated dial is 0.01mm or 0.0004”. Each division on the fine bore head body is 0.002mm or 0.00008”. (see image 4)
- Use a tool pre-setter to adjust the diameter to the center of the desired tolerance.
- Tighten the set screw to lock the graduated dial (see image 3)
- Take a cut approximately 5 to 10mm (.200 to .400”) deep.
- Measure the diameter bored diameter.
- Make a final adjustment on the graduated dial.
- Cut the bore again.
- Check the bore diameter to verify that it is correct.
There are three main factors that affect finish boring performance:
The amount of stock to remove, commonly referred to as Depth of Cut (DOC)
- The feed rate
- The cutting speed
Stock
Too much stock for removal or a feed rate that is too fast will produce higher cutting forces and can make consistent bore size difficult to achieve. Too little stock to remove or feed rates that are too slow increase the probability of chatter and unwanted vibration in the cut.
A good rule for stable finish boring is to leave stock (DOC) for finishing that is between one half and one full nose radius of the insert used. When this is the case, cutting forces are generated in the axial direction where the boring tool is strongest. Too little stock (DOC) produces radial or side-cutting forces increasing the probability of unwanted vibration. Typically, smaller nose radii will produce more consistent results.
Cutting forces are radial when the Depth of Cut (DOC) is less than half of the nose radius.
There is a greater chance of chatter or deflection.
1. Cutting Forces 2. DOC < 1/2 Tool Nose Radius
Cutting forces are axial when the Depth of Cut (DOC) is greater than half of the nose radius.
There is less chance of chatter or deflection.
1. Cutting Forces 2. DOC > 1/2 Tool Nose Radius
Feed Rate
Inserts are designed with a honed edge on the tip. A feed per revolution that is lower than the width of that honed edge can cause deflection and chatter in the cut. Increasing the feed per revolution will enhance the effectiveness of the chip breaker on the insert and produce a more stable cut. Don’t worry about finding the size of the honed edge on your inserts. If you get chatter in the cut, try increasing the feed per revolution. Always follow the speed and feed recommendations for the insert and workpiece material.
Cutting Speed (RPM)
Again, follow the speed recommendations from the speed and feed chart for the insert. Higher speeds will produce a better surface finish, evacuate chips better, and shorten the cycle time. Higher speed also increases the possibility of chatter. Lower speed is typically just the opposite. The surface finish may be worse, the cycle time is longer, and premature insert wear is possible. The benefit of slower cutting speed is that it can reduce or eliminate chatter.
The length-to-diameter ratio of the boring tool and the insert’s nose radius are the two biggest factors in determining the perfect speed. For example, you should be able to run at the recommended speed and feed for an insert and material when the nose radius is 0.8mm (0.032”) and the length-to-diameter ratio is 4 to 1 or less. You always want to use the shortest boring tool to achieve the cut. Excessive length increases the chances of complications and poor results.
| Length to Diameter Ratio | Maximum Insert Radius (If Available) | Percentage of RPM Reduction |
| 4:1 | 0.8 mm/0.0312" | 100% |
| 5:1 | 0.4 mm/0.0156" | 75% |
| 6:1 | 0.2 mm/ 0.0078" | 60% |
| 7:1 | 0.2 mm/ 0.0078" | 50% |
Related Videos