Description of settings

ytliu

Hi,Nikolay81!
In the four-axis machining, the feed rate F is directly used as the composite vector speed in the conventional algorithm. Since the dimension (angle) of the A-axis and the dimension (distance) of the XYZ axis are different, the actual cutting speed is unpredictable. In response to this problem, the DDCSV system adds a four-axis speed optimization algorithm that first calculates the cutting line displacement of the tool relative to the workpiece surface in each command segment, and then uses the feed rate F to control the speed of its line displacement. In order to complete the calculation of the line displacement, we first need to know the structure of the machine. The #6 parameter is the function. If #6 is configured as 3 (not rotate), the optimization algorithm will be closed, and the conventional algorithm will be used. In addition, after using the optimization algorithm, the closer the tool tip is to the material axis, the higher the actual rotation speed of the A axis is at the same feed speed F, which may exceed the tolerance of the A axis, so we designed #5 Parameters to protect this.

#104"A axis optimal path when G0 run"，For example, if the current position of the A axis is 30 degrees and execute the G0A720 command. If #104=0(NO), the A axis will move 690 degrees in the forward direction; if #104=1 (YES), the A axis will move 30 degrees in the negative direction.

#124 "Circular centrifugal acceleration", in the case of the same feedrate F during machining, the smaller the radius of the arc command, the greater the impact on the machine tool. The DDCSV system adjusts the actual feed rate of the arc segment based on the configuration of the Circular centrifugal acceleration.  If #124=0, the system assigns it using #99(operation acceleration).

#125 "Circular speed adjustment factor", used to set the actual given speed of the arc segment F=program feedrate F*#125, note that this parameter is only for the arc segment, and the straight segment is still controlled according to the programmed feedrate.

#435 "X axis protection speed", #436 "Y axis protection speed", during processing, the component speed of the XY axis does not exceed the range set by these parameters.

#108 "M Bus IO command response", #109 "M Bus IO default status", DDCSV system can extend IO through RS232 interface, the specific protocol refers to http://bbs.ddcnc.com/forum.php?mod=viewthread&tid=7&extra=&page=2, #108=1(YES) will enable this function, #109 determines the state of the 32-way extended IO in the reset state.

#68 "Tool Setting function mode" (description of Mode 1 and 2), mode 1 is described in detail in the manual; mode 2 is relatively simple, the customer needs to know the thickness of the tool block in advance and record it to #69. When the tool is set, the tool block is placed on the surface of the workpiece. When the tool setting signal is detected, the workpiece coordinate of the Z axis becomes #69, and the tool setting is completed.

#434 "A/B phase signal level on MPG", used to set the initial level state of the AB phase of the handwheel. Even if this parameter setting does not match the actual one, the opponent wheel function has no effect. Therefore, this parameter does not matter.

#448 "MPG control mode" , please refer to http://bbs.ddcnc.com/forum.php?mod=viewthread&tid=1

#2 "Display response during working", some nc file may be composed of a large number of dense small line segments. It is possible that the speed of code analysis cannot keep up with the processing speed, which will cause the processing to be stuck. At this time, this parameter can be increased, allows code parsing to get more CPU time and avoid this.

#120 "U disk partition type", some U disk may have a partition. Please configure this parameter in conjunction with the actual situation of the U disk to ensure that the directory is in the expected directory when the file page is opened.

#396 "Number of line", the number of path segments of the look-ahead algorithm. Adjusting this parameter has little effect on the processing effect and can be ignored.

#495 "interpolation period", lowering this parameter will increase the machining accuracy, but the processing time will increase.

#499 "user access key", the parameter under the configuration page can be set when the parameter is 888888.

ytliu

Kev0 Posted at 2018-10-9 22:46
Will the #124 affect a normal G02/G03 as well?

yes

ytliu

maxx2000 Posted at 2018-10-13 01:53
Hi Ytliu .
maybe you have the opportunity to give a detailed description of other settings as you ex ...

Hi maxx2000.

When #113=0, the system adopts an improved Min-error interpolation method. The accuracy of the ordinary Min-error interpolation method is 1 pulse, and the improved method achieve can achieve 0.5 pulse precision. Since the algorithm is implemented in fpga, I call it "hard algorithm". Using this algorithm to perform G2/G3, the speed is stable and the accuracy is high, but the pulse equivalent of the circular plane axis must be the same.

When #113=1, the software will cut the arc into small segments and then perform line interpolation, so I call it "soft algorithm".

When using soft algorithm, the software will draw these small segments in turn, and normally, it will not cause problems.

When using hard algorithm, the software will draw the arc as a whole, and will reset the arc parameters according to the display scale, and then use the Min-error interpolation method to draw points one by one on the screen, so sometimes the drawing may be incorrect.

I will modify the software for the suggestion of "the split parameter # 224"