(1) parts drawing

Figure 1-1

(2) Analysis of Parts Drawings
The surface of the part is composed of a cylinder, a straight arc, an inverse arc, a cone, a groove, a thread, a hole, and the like. The dimensioning is complete. The blank is 45# steel Φ50mm×120mm. Heat treatment: Modulation treatment, HRC25-35 has no hardness requirement.

(3) Determine the processing method:
The principle of selection of the processing method is to ensure the processing accuracy and surface roughness of the machined surface.
Because there are many processing methods for obtaining the same level of precision and surface roughness, comprehensive considerations such as the shape, size, and tolerance requirements of the shape and position of the parts must be taken into account in the actual selection. In the figure, several precisions require higher dimensions. Because the tolerance value is small, no average is taken during programming and its basic size is taken. There is a taper of 1:5 and an arc cut point on the contour line, and its coordinates (29.7,0) (34, 16.5) (46, 22.5) are required during programming.
Through the above data analysis, considering the processing efficiency and economical processing, the most ideal machining method is turning. Considering that the part is mass-processed, the machining equipment uses a CNC lathe. The CJK6032 CNC machine tool was selected based on the shape and material conditions of the machined parts.

(4) Determine the processing plan
More sophisticated processing on the part surface often through roughing, semi-finishing and finishing gradually achieved. It is not enough to select the appropriate final processing method for these surfaces based only on quality requirements. The processing plan from the blank to the final forming should also be correctly determined.
Blank first holding the right end, turning the left end of the outline 50mm, the left edge processing Φ46mm, Φ29.7mm, slope 1:5 slope, R6 arc, drilling Φ20mm hole, 镗 Φ20mm hole and C1.5 chamfer.
Heading clamping has been processed Φ46mm outer circle, right-end processing Φ36mm, cut back sipe, processing thread M27 × 1.5, Φ20mm, SΦ20mm, and down to the size.
The typical axis processing sequence is:
Preparation — Turning Faces — Roughing Left End Profiles — Finishing Turning Left End Profiles — Drilling — Rough Borings — Fine Boring Holes — Workpiece U-turn — Rough turning right end profile — finish turning right end profile — Cut out sipe — rough turning thread — finish Turning thread.

(5) Determine the positioning reference and mounting method:
(1) Positioning datum: It is determined that the billet axis and the outer circle plane are the reference for positioning.
(2) Clamping scheme: Adopt three-jaw self-centering chuck, centering and clamping.

(6) Determine the processing sequence and feed route:
The processing sequence is determined from rough to fine and from near to far.
That is to say, from the right to the left, rough turning (leaving a 0.25 mm finish turning margin),
Then finish turning from right to left and finally turning the screw thread.

(7) Tool selection
(1) Use a Φ5mm center drill to drill the center hole.
(2) Use Φ20mm high speed steel twist drill.
(3) Rough turning and flat end face use 90° carbide turning tool.
(4) Use a kerf knife with a width of 5mm.
(5) The thread is made of cemented carbide 60° external thread turning tool, and the radius of the tip radius is smaller than the minimum arc radius, and 0.15-0.2 mm is appropriate. The selected tool parameters are entered into the NC tooling card (see table) for easy programming and operation management.
CNC machining tool card

Product name or code		Part Name	Typical axis		Part number
No.	Tool number	Tool specification name	Quantity	Machining surface		Note
1	T01	High-speed steel Φ5mm center drill	1	Drill left center hole
2	T02	High Speed Steel Φ20mm Twist Drill	1	Drill left Φ20mm hole
3	T03	Carbide 45° external turning tool	1	Turning outer contour, end surface
4	T04	5mm grooving knife	1	Grooving
5	T05	Inner bore boring cutter	1	Fine bore
6	T06	60° external thread turning tool	1	Turning thread

Table 4-1


8) Selection of cutting amount
(1) back to eat knife selection, contour rough turning cycle selection 3mm, finish turning selection 0.25mm, thread rough turning selection 0.4 mm, reducing knife by knife, finish turning is 0.1 mm.
(2) Spindle speed selection, turning straight and arc, choose rough turning cutting speed of 90m/min, finish turning cutting speed 120m/min, then use the formula to calculate the spindle speed: rough turning: 500r/min, finish turning :1200 r/min
(3) The selection of feed speed, look-up table choose rough turning, finish turning feed per revolution, and then according to the actual situation of processing to determine rough turning per revolution feed is 0.4 mm/r, finish turning zero per revolution is 0.15 mm/r, Finally, rough turning is calculated according to the formula. The finish turning feedrate is 200 mm/min and 180 mm/min, respectively.
Comprehensively analyze the various contents of the previous analysis and fill it into the NC process card. This represents the main basis for the preparation of the processing program and the guidance documents for the NC machining operations performed by the operator.
The main contents include: the order of the work steps, the content of the work steps, the cutting tools and cutting amount used for each work step.