Five-axis milling of impeller

The impeller refers to the disc equipped with moving blades. Commonly used materials for impellers include cast iron, bronze, stainless steel, manganese bronze, Monel, INCONEL, and non-metallic materials.

Processing requirements for the impeller: 1) It can provide a large energy head; (2) The loss of gas flowing through the impeller should be small, that is, the efficiency of gas flowing through the impeller should be high; (3) When the gas flows out of the impeller, the parameters should be appropriate. The flow loss when the gas flows through the fixed components behind is smaller; (4) The impeller type can make the stable operating area and high-efficiency area of the stage or complete machine performance curve wider. Therefore, five-axis linkage machine tool technology must be used for milling the impeller.

Step 1: Blade profile milling

Blade profile milling uses a tapered annular cutter (diameter 3mm, cutting edge length 30mm), as shown in Figure 2. The solution used to process a single blade profile of an impeller – copy milling between 2 curves, and the tool milling range is controlled within the two curves. Among them, the selection of cutting type “depends on the cutting quantity”, and the cutting quantity is controlled by the cutting quantity, thereby generating a cutting path, see Figure 3. The cutting method is “single path”, and the type of unidirectional addition is defined as “clockwise”. The above two parameters can be defined according to the process requirements, and the specific shape of the blade should also be considered, see Figure 4.

1. Define geometry

Select the outer edge of the blade as the “first” curve, select the inner edge of the blade as the “second” curve, and select the surface between the two blades as the “guiding surface”. The above three items are required and are the basis for generating “code” Require.

The “first” curve uses the outline of space to limit the curved surface processing trajectory, so that the trajectory is within the restriction area 1; the “second” curve uses the outline of space to limit the surface processing trajectory, so that the trajectory is within the restriction area 2 Carry out processing; “guiding surface” defines the surface object to be processed on the product, see Figure 5.

2. Define tool axis control

The tool axis tilt method is defined as “tilt according to the cutting direction”. Considering that the tool side edge needs to be used for processing, the tool axis vector needs to be reasonably controlled at this time. The tool is tilted according to the cutting direction, so that the tool generates a tool path along the natural direction of the curved surface shape, and the parts processed with such a tool path are smoother. Set the “inclination angle on one side in the cutting direction” to 85°. This is mainly due to the taper angle of the cutting tool (using the side edge of the milling cutter to process the curved surface in space can greatly improve the finishing efficiency of the curved surface). See the picture. 6.

Note that the above value is 85°, which will cause the machine tool to continuously rotate to observe the machine tool simulation. The rotation mentioned here is due to the interference check. When we use 80° or 85°, observe the changes in the tool and the changes in the machine tool in the machine tool simulation, and compare. The tool taper angle is transformed to 2.5°, and the settings are reset to compare the differences.

3. Define interference inspection

Define the first interference check option: select the guiding surface as the interference check surface, and the system will automatically use the added surface as the interference check surface. The application of this situation is mainly to solve the phenomenon of interference between the twisted guide surface and the tool after being processed, see Figure 7.

Define the second interference check option: Select the surface between the two blades again as the second interference check surface. If the tool interferes, it will be “indented along the direction of the tool axis.” The check surface refers to the interference surface of the tool when used for space surface processing. See Figure 8.

4. Definition of continuous knife

Define the continuous tool type as “cylindrical parallel to the Z axis” within the safe range. Since it passes through the X0, Y0, and ZO points and is parallel to the Z axis, the transition between the tool paths will be connected by a cylinder with a radius of 1OOmm and the axis passing through the 0 point and parallel to the 7-axis, see Figure 10. Select “Use Infeed Macro” in the first feed, select “Use Retract Macro” in the last retract point, the feed macro program type is “Arc Tangent”, and the arc sweep is set to 45 °, through the above settings, the tool path entry and exit can be further controlled, see Figure 11-14.

The advancing and retracting tools have the same macro settings, so the same results must be produced in the tool path for blade machining (the same for each layer), see Figure 15.

Step 2: Process the middle area of the two blades

When processing the middle area of the two blades, use a ball-nose cutter (diameter 3mm), and the curved surface path is “copying milling between 2 curved surfaces”, see Figure 1. The cutting method is “Z-shaped milling” and the cutting sequence is “from inside to outside”, see Figure 2. The relative surfaces of the two blades are defined as the “first” surface and the “second” surface respectively, and the surface between the two blades is defined as the “driving surface”, see Figure 3.

1. Define tool axis control

The cutter axis will be “tilted through the curve”, see Figure 4, the curve approach type is “close to point”, and a “tilt curve” will be established between the outer edges of the two blades, see Figure 5. The method of establishing a curve is to use the auxiliary surfaces of the two blade surfaces to create an edge curve at the top. The curved surface processing trajectory is limited by the contour of space, so that the trajectory can be processed within the restricted area, thereby controlling the trajectory range of the tool.

2Define interference inspection

Select the “Cutting Edge” of the tool to participate in the interference check, and also check “Guide Surface” and “Check Surface”, see Figure 6. The check surfaces are the inner surfaces of the two blades (that is, the “first” surface and the “second” surface mentioned earlier). Of course, the two surfaces must be selected again. When the ‘Guiding Surface’ surface is checked.

3. Definition of continuous knife

Define the first incoming knife as “use the infeed macro” and define the last retract point as “use the retract macro”, see Figure 7. All slices are connected smoothly using “mixed spline”, see Figure 8. The infeed macro program uses “vertical tangential radius” and the arc sweep is 10º, see Figure 9. The infeed and exit trajectories generated in this way are approximately a straight line, see Figure 10.

Step Three: Control of the Tool Axis in Finishing

Defining space curves is a good way to control the tool axis. It can make the tool path you define very smooth and greatly shorten the calculation time. However, defining spatial curves requires a wealth of actual processing experience, familiarity with CAD instructions, and knowledge of the relevant functions of five-axis aerospace milling. The Cimatron system will automatically calculate the swing direction of the tool to avoid interference collisions.

Select the guiding surface as the interference check surface, and define the tool path generation type. The tolerance is set to 1.6, and an amount of 0.1 is reserved here, which is the allowance for processing during the final root cleaning, as shown in Figure 1.

In order to avoid the situation where the processing is not in place, we extend the path of the knife by 10mm at the cutting/cutting place, so as to avoid such situations. As shown in Figure 2, the diameter of the tool is The percentage value is set to 10. The results obtained by this program are shown in Figure 3.

Step 4: Tool path control based on rough opening program based on finishing machining

On the basis of finishing, we will easily use the blank layering to create a roughing program. First, copy the last segment program, and the roughing milling settings are shown in Figure 4.

In the roughing tool path, define the number of layers and spacing respectively, and then define the number of layers and spacing in the machining tool path. The spacing here is the 3D distance between the two layers. Here you can also define the finishing tool path.

Define the guiding surface in the surface path, cancel the original guiding surface, and select the new surface of revolution just created. Click the “Advanced” option and select “Generate tool path on the front side”, as shown in Figure 5. If this option is not selected, toolpaths will be generated across the entire blade. This dialogue pivot can also be used to define the angle between the tool path and the surface.

Figure 5 Angle setting between tool path and surface

Calculate this program segment to obtain the roughing + finishing tool path, as shown in Figure 6.

Step 5: Add blank and optimize roughing tool path

Add blanks to each program segment to optimize the tool path. Create three curved surfaces between the blades and use these three surfaces to define the blank. The blades are shown in Figure 7.

Adjust the transparency of the blade to facilitate observation and selection of the blank. We can see that many tool paths will be generated, see Figure 8.

In addition to parts, there are many tool paths that are not involved in cutting. Now, simple settings can be used to cancel these tool paths other than the blank. Copy the previous program and edit it, open the “Blank Definition” option, and select the rough surface you just defined, as shown in Figure 9. Finally, the program is calculated to obtain the tool path trajectory, as shown in Figure 10.

If you see the tool path trajectory connected in space (after the blank is defined), it means that the blank you defined plays a certain role in the tool path calculation. If you are not satisfied with this connection method, you can click “Connecting tools” “Change the corresponding parameters in ” until you get satisfactory results.

Request For Quote


Let's have a chat

Leave your information, our sales will contact you as soon as possible!