1. Benefits of ramping
Benefit 1: Improve processing efficiency
For keyway milling of solid materials, most of the time you use a drill to drill holes first, and then mill them in layers. In ramp milling, the tool directly enters the solid material to remove material, which reduces tool changing time and improves efficiency.
Benefit 2: Increase tool life.
In the processing of difficult materials, work hardening is prone to occur, resulting in old wear of the blade at one point.
picture
So how to solve this problem? Qingfeng I gave a simple method: adjust the (Ap) depth of cut in the processing parameters, that is, don't always let the blade contact the hardened skin in one place. The tool path of ramping milling is exactly in line with this.
picture
Add WeChat: Yuki7557 to receive a copy of the macro program tutorial
Second, why use macro programs?
The ramping milling program is very simple. We can easily do it by manual programming. Why do we need to use macro programming?
Benefit 1: Streamlined procedures
If the groove is relatively deep, no matter whether the program processed by the software or your ordinary manual programming, the program will be too long, while the macro program will be short and concise.
Benefit 2: Convenient for workers to debug on site
I know that correct programs written by programmers will have more or less problems during on-site debugging. For example, the depth of cut is unreasonable and the depth of cut needs to be reduced. Then the macro program only needs to assign values to variables to complete. In ordinary programs, many values need to be modified.
Benefit 3: The program has good versatility
The biggest feature of macro programs is their good versatility. For example, there may be N many parts in a workshop with similar shapes and different sizes, so writing one program can satisfy N many products.
3. How to program [Ramping Milling]?
picture
1. Calculate the cutting depth of each tool #30
picture
As shown in the diagram above, according to the Pythagorean theorem TAN[#2]=#30/#7
The depth of each knife can be calculated #30=#7*TAN[#2]
2. Calculate the number of tool passes #31
The total depth is #11, then the number of tool passes can be calculated, that is, #31=#11/#30, which is the total depth divided by the depth of each tool.
The problem is, if the result of the division has a decimal, such as 5.6 times, such as 5.1 times, etc., then the number of tool passes must be calculated as 6 times.
So #31=FUP[#11/#30]
Remark:
FUP means converting the decimal part into an integer 1 and adding it to the integer part.
For example, #31=5.06 The value after FUP[#31] operation is 6.
#31=0.01 Then the value after FUP[#31] operation is 1.
3. Calculate the actual cutting depth #32
When calculating the number of tool passes, the decimal part is taken as an integer. If calculated according to #30, there will be overcutting. How to calculate the actual depth of cut #32 for each knife?
The answer is: the total depth divided by the number of passes is the actual cutting depth. That is #32=#11/ #31
4. Set knife points #24 and #25
#24 The X coordinate value of the cutting center in the workpiece coordinate system
#25 The Y coordinate value of the cutting center in the workpiece coordinate system
5. Think about why you need to calculate these variables in the first four steps?
For example, the depth of cut per cut is calculated as #30. With the depth of cut per cut, I can divide the total depth of #11 by the depth of each cut to calculate the number of processing times.
With the number of processing times, we can use macro program statements to set conditions and let the program cycle through processing until the size is reached.
However, we rounded the decimal part of the calculated number of machinings. If calculated based on the depth of cut of #30 per tool, there will be overcutting, so the actual cutting per tool is calculated by dividing the total depth by the number of machining times. depth.
The procedure is as follows:
%
#24=0
#25=0
#11=30
#2=5
#7=60
G0X#24Y#25 (Tool rapid cutting point)
Z2.0
G01Z0.F200
#30=TAN[#2]*#7(depth of each cut)
#31=FUP[#11/#30](The total depth is divided by each depth of cut to calculate the number of cycles, [rounded up])
#32=#11/#31 (actual cutting depth each time)
#33=0 (Counting variable, this value starts counting from 0)
N10#33=#33+1 (the variable increases automatically, and the count value increases by 1 for each operation)
G91G01X#7Z-#32F#9
X-#7
IF[#33LT#31]GOTO10 (when the value of the count variable is less than the number of processing times, jump to the N10 line block)
G0Z150.
M30
%
The program simulation is as follows:
