The manufacturability of the designs is the most critical factor in project processes. The diversity of production processes and the necessity of subsequent operations significantly affect a project's costs, production lead times, and production quality, from design to production.
Some key considerations in the design process for parts intended for machining help create parts in the most straightforward manner without excessive process variation, keeping overall process costs reasonable while maintaining the desired level of quality.
In machining, especially in 3-axis and 5-axis operations, paying attention to the following recommendations in your designs when you are certain that they do not affect the functionality of the parts will help you optimize production by keeping costs, manufacturing lead times, and part quality at their ideal levels.
1 - Preferring radiused corners over sharp inside corners in your design eliminates additional processes and costs. In standard situations, using minimum 2mm radius turns up to a depth of 10mm at corners allows for the part's production on vertical machining centers. When the depth increases, the radius can be increased, or special tools can be created. If sharp corners are required, corner shaping can be achieved with additional processes using plunge erosion.
2 - If sharpness can be achieved through chamfering on horizontal lines, then a radius should not be preferred. While radiused designs are feasible for horizontal lines, they increase the processing time and, in turn, the cost.
3 - Radii or chamfered edges should be specified in the technical drawing, while in the 3D data, they should be removed.
4 - Holes to be threaded should be left without threads in the 3D data file at the pre-hole diameter. For example, for a hole to be threaded with an M6 thread, the pre-hole diameter should be left at 5mm, and for a hole to be threaded with an M4 thread, the pre-hole diameter should be 3.2mm.
5 - Keeping hole depths within standard ranges helps eliminate the need for special tools and keeps costs at a standard level. Therefore, it is preferable to choose situations where hole depths do not exceed five times the hole diameter. For example, with a 5mm hole diameter, a hole depth of 25mm allows for operations with standard tools.
6 - Avoiding designs that exceed three times the hole diameter in guide depths, similar to hole depths, will reduce operational costs.
7 - Unless necessary, holes should not be placed too close to the edges of the part. For example, a 2.5mm diameter hole should be at least 1mm away from the edge of the part. For holes larger than 2.5mm, values greater than 1mm should be preferred.
8 - In designs where general steel types will be machined, holes with a diameter of less than 1.5mm should be avoided.
9 - Stock materials are typically supplied in dimensions that are multiples of 5. When the volumetric dimensions of the part in your design are exact multiples of 5, the stock size increases, leading to more material waste and longer machining times. Having your parts in your designs with dimensions like 28 x 48 x 98 ensures that the nearest stock size is a standard measurement. For instance, an aluminum part measuring 22 x 28 x 95 mm with a 3 mm allowance for clamping can be machined from a stock piece of 30 x 30 x 100 mm. However, a part measuring 25 x 30 x 95 mm that requires material removal from all surfaces will necessitate sourcing a stock of 30 x 40 x 100 mm.
10 - To facilitate easy alignment during the machining of parts with curved surfaces, guide holes that allow for easy clamping should be added to the design.
11 - In cases where parts in 3-axis machining require multiple fixturing, it is advisable to use reference surfaces that are perpendicular and parallel to each other. This will enhance the accuracy of the part zeroing process.
12 - Precision surfaces and dimensions like bearing seats should be specified in the technical drawing, and if possible, the bearing or machine element to be mounted on the part should be provided to ensure it is machined to the desired clearance value.
13 - In our standard operations, we work with a surface quality of Ra 1.6 – Ra 3.2. Please specify any surfaces that require higher quality in the technical drawing, as an increase in surface quality will affect our machining costs.
14 - In our standard operations, we use ISO 2768 Medium tolerance. If you require ISO 2768 Fine or ISO 2768 Coarse tolerance, please specify it separately.
15 - Please specify the required process for parts that need a measurement report or CMM measurement. We have the capability to perform CMM measurements.
Kommentare