Digital Dream Technology support

Title: Poor work G28 [Print This Page]

Author: Nikolay81 Time: 2018-7-19 23:47
Title: Poor work G28
Hello.
How do I get G28 to work properly?
For example, I need to send the z-axis to the machine home.
I am writing G90 G28 Z0
The tool first goes to point 0 in the current coordinate system (for example, G54), and then all axes go to machine 0.
How to move, only one axis in the machine 0?

Author: ytliu Time: 2018-7-20 08:22
Hi Nikolay81:
According to your request, I have changed the implementation of G28 (O9028) in slib.nc, Unzip the attachment and reinstall slib.nc on the controller.

slib.zip

1.79 KB, Down times: 1090

Author: Nikolay81 Time: 2018-7-20 17:32

ytliu Posted at 2018-7-20 08:22
Hi Nikolay81:
According to your request, I have changed the implementation of G28 (O9028) in slib.nc ...

Many thanks! Now the Z can be parked separately from other axes. But, as before, with the command G90 G28 X0 Y0 Z0, the axes first go to 0 of the current coordinate system, and only then, to machine zero. Can I have them go straight to the machine zero?

Author: Nikolay81 Time: 2018-7-20 17:43
Also, the G53 command, which many like, works incorrectly with the Z axis. For example, G90 G53 Х0 У0 will send the X and Y axes to the machine 0. Аnd G90 G53 Z0 will move the z-axis to the machine coordinate -19mm. Can you fix this command?

Author: ytliu Time: 2018-7-21 16:21

Nikolay81 Posted at 2018-7-20 17:43
Also, the G53 command, which many like, works incorrectly with the Z axis. For example, G90 G53 Х0 ...

G28 instruction format: G28X_Y_Z_A_
Among them, X, Y, Z, A are the coordinates of the intermediate point (below the current workpiece coordinate system) when returning to the machine zero. After the command is executed, all controlled axes will be quickly positioned to the intermediate point and then from the intermediate point to the machine zero.
If you want to return an axis directly to the machine zero via the G28 command, such as the Z axis, use:
G91G28Z0

In the DDCSV system, G53 is not a machine coordinate system movement command. The slib.nc in the attachment expands the G153 command for you. By this command, the tool can be moved to the desired machine coordinate position.

install(2018-07-21-96).zip

575.49 KB, Down times: 1515

Author: Nikolay81 Time: 2018-7-21 19:30

ytliu Posted at 2018-7-21 16:21
G28 instruction format: G28X_Y_Z_A_
Among them, X, Y, Z, A are the coordinates of the intermediate ...

Many thanks. G28 works correctly. G153, also works, but not quite right. In G53 you can set the speed. A G153 moves the X and Y axes at a speed of G0, and the Z axis with speed "Z axies lifting protection speed". In the case G53, I write G53 G0 X1 Y-1 Z-1 and all the axes go to the point X1 Y-1 Z-1 with the speed G0 . Or I write G53 G1 Х1 Y-1 Z-1 F800 and all the axes go to the point Х1 Y-1 Z-1 at a speed of 800. With the G153 command this does not work. Can you add a change in speed to G153? Or, at least, to make the z-axis move at a speed G0?

Author: ytliu Time: 2018-7-21 20:19
Last edited by ytliu In 2018-7-21 20:23 Editor

Nikolay81 Posted at 2018-7-21 19:30
Many thanks. G28 works correctly. G153, also works, but not quite right. In G53 you can set the sp ...

Attachment installation file supports G153 speed control

install(2018-07-21-96).zip

575.49 KB, Down times: 1654

Author: Nikolay81 Time: 2018-7-23 16:48

ytliu Posted at 2018-7-21 20:19
Attachment installation file supports G153 speed control

Thank you very much! Now everything works perfectly.

Author: ytliu Time: 2018-7-23 16:54

Nikolay81 Posted at 2018-7-23 16:48
Thank you very much! Now everything works perfectly.

Author: Nikolay81 Time: 2018-7-24 00:32

ytliu Posted at 2018-7-23 16:54

I was happy early.
Adding the G153 command made additional bugs.
I launch the program:
G90 G21 G54
G153 Z-2 F2000
M0(tool name)
G0 Z0.5
M3 S21000
G0 X24.50Y-6.00
On the line "M0 (tool name)" it should pause and write on the screen "M0 (tool name)" - that is, the name of the tool.
But he writes an empty line. If before "M0 (tool name)" is for example "G91 G28 Z0" everything will be fine.
Further, after "M0 (tool name)", while the machine is paused, I bring the tool manually to the billet and zero all axes.
Then I press start.
Further, it should raise the Z axis by 0.5 mm and run the spindle. And in the previous firmware, it happened.
But now, he first raises Z to an arbitrary large number (from 19 to 25mm, I do not know what it depends on), and then lowers it to 0.5mm. In this case, it can rest against the axis limit.
How to fix these 2 problems?

Author: Nikolay81 Time: 2018-7-24 01:32
Last edited by Nikolay81 In 2018-7-24 02:38 Editor

A simpler example.
Program:
G153 Z-2 F2000
M0(tool name)
First, he lifts the z-axis to -2mm in the machine coordinates,
then will raise to the value of parameter # 89 (I have 2mm) - will be 0 in machine coordinates, then put it on pause.
If immediately, press start, the z axis will go to position -2 in machine coordinates.
If, before this, put down the z axis with buttons and reset to zero, and then press start, a bug will occur.
The z axis will go to (it's hard to explain, better to see for yourself) the position of the machine coordinate system is -2mm, but what it was
in the current coordinate system until the z axis is zeroed. That is, if it is zeroed below point 0 in G54, the axis does not reach
limit. If higher - rests on the limit.In any case, it's very bad. The z axis after the pause must go to the point of the parameter #89 in the current coordinate system, not the machine coordinate system.
How to fix it?

Author: ytliu Time: 2018-7-24 11:19

Nikolay81 Posted at 2018-7-24 01:32
A simpler example.
Program:
G153 Z-2 F2000

I don't know how to describe this problem. I made some changes to the program according to my understanding. Let's see if it can achieve your intention.

install.zip

566.7 KB, Down times: 1336

Author: Nikolay81 Time: 2018-7-24 15:15

ytliu Posted at 2018-7-24 11:19
I don't know how to describe this problem. I made some changes to the program according to my unde ...

Dear ytliu.
I will explain my situation.
I am the chief engineer of the company Aerotechservice http://aerots.ru/. My name is Nikolai Zvyagintsev.
At the moment we are repairing the components of the aircraft, but we want to start producing CNC milling machines in addition to the main production.
For now, with manual tool change.
At the moment, in our production we use several machines on Purelogic controllers.
But at them, too small maximum frequency of a signal Step / Dir. So, for the basis of our new machines, I chose the DDCSV2.2 controller.
But its software is still too raw.
Incidentally, I saw that there was technical support for these controllers, and the management of our organization, decided to wait until the software of these controllers will be brought to a commercially acceptable level.
The main problem, in a convenient manual change of tools. Since, the machines will be commercial, this should be organized, really convenient.
In those machines where we work now, manual tool change occurs according to the following algorithm:
-the end of the operation;
-The Z axis lifts to the height of the SafeZ;
-the spindle stops;
-the axis is raised to the very top, to the point 0 in the machine coordinates (to make it convenient to change the cutter) at the speed G00;
-axis X and Y are moved to the point 0, 0 in the current coordinate system (zero of the billing) at the speed G00
-A sound signal is heard
-The machine pauses and writes the name of the new cutter on the screen, which you need to insert;
-The operator changes the cutter, pushes the new cutter to the billing with the buttons and uses a piece of paper to define 0 along the z axis;
-By leaving the paper clamped, he presses the start button;
-The machine itself self-zeroes the z-axis, in the current coordinate system;
-The Z axis is raised to the SafeZ height and the operator pulls out the paper;
-The spindle spins and the next operation begins.

As you can see, the algorithm is convenient, does not require the operator to press the buttons once more.

I ask for your help, organize such an algorithm for changing the tool on DDCSV2.2.
If this does not work out, the managers of our company will choose the verified Purelogic controllers and we will not be able to continuously purchase DDCSV2.2

I'm not asking for it for free.
We will pay for your work, and also post free created postprocessors and instructions.

It is necessary to solve the following problems:
-organize such a pause from the g-code, in which the z-axis does not move (while keeping the function of the pause button unchanged). Because the operator on a pause changes the tool and manually sets it to 0. After that, naturally the z axis should not make unauthorized movements, so as not to stick the cutter into the table.
-add the ability to play the audio signal from the g-code
-add the ability to zero the axes from the g-code
-can write all this in the macro of the command m6 (T.nc). Or, can organize it from the g-code. No difference.

Which of these tasks can you solve?

Author: ytliu Time: 2018-7-24 19:56

Nikolay81 Posted at 2018-7-24 15:15
Dear ytliu.
I will explain my situation.
I am the chief engineer of the company Aerotechservice ht ...

Hi,Nikolay81!
I basically understand your needs, I will try to design an example according to the process you said. In addition, the "-add the ability to play the audio signal from the g-code" that you mentioned is not very clear. Is it controlled by an IO?

Author: Nikolay81 Time: 2018-7-24 20:08

ytliu Posted at 2018-7-24 19:56
Hi,Nikolay81!
I basically understand your needs, I will try to design an example according to the ...

For example M300 S5000 P280.
The command works in 3D printers.
It reproduces the sound, built-in buzzer, 5000 milliseconds, 280 hertz.
But the frequency can not be set. It is enough that the machine squeaks when it is necessary to replace the instrument.

Excuse me. I accidentally pressed the "support" button.
I hope I did not mess up anything on the forum :-)

Welcome Digital Dream Technology support (http://bbs.ddcnc.com/)