Digital Dream Technology support

Title: Poor work G83 [Print This Page]

Author: Nikolay81 Time: 2018-8-1 14:55
Title: Poor work G83
One of the most important problems of DDCSV is the incorrect operation of the G83 drilling cycle.
You probably know what I'm talking about, so I will not write much.
Briefly, after the retract (withdrawal of the drill), it returns the drill bit to the quick feeder, not to the point where it finished drilling, but above it by 1.5 mm.
This greatly increases the drilling time.
I repaired this cycle (the file is attached to the message). Now, it works correctly. But I'm a bad programmer and a stupid person. Therefore, it turned out not very beautiful.
It was necessary to understand, where an error with variables #9 and #10. And I just added another variable #15.
I ask you to repair the G83 command correctly, without variable #15.

There is still a problem with the parameter K. It must drill symmetrically located holes.
Instead, he just drills the same hole again. In our time, nobody uses the K parameter.
I suggest, just remove it. So as not to mislead people.

In the future, it is desirable to add a cycle G73.
There are people who use it.

slib.rar

1.72 KB, Down times: 646

Author: ytliu Time: 2018-8-1 18:49
Last edited by ytliu In 2018-8-1 18:52 Editor

Modified the definition of G83 in slib.nc and added G73 support. Increase #2020(G73 Retraction amount) and #2021(G83 Retraction amount)

G73.png (69.34 KB, Down times: 750)

G83.png (110.96 KB, Down times: 830)

install.zip

579.21 KB, Down times: 1058

Author: ytliu Time: 2018-8-1 19:09
Last edited by ytliu In 2018-8-1 19:11 Editor

Execute G99G83X10Y10Z-15R0Q5, if #2021=0, decomposition action:
G0X10Y10
G0Z0
G1Z-5
G0Z0
G0Z-5
G1Z-10
G0Z0
G0Z-10
G1Z-15
G0Z0
If #2021=1, the decomposition action:
G0X10Y10
G0Z0
G1Z-5
G0Z0
G0Z-4
G1Z-10
G0Z0
G0Z-9
G1Z-15
G0Z0

Execute G99G73X10Y10Z-15R0Q5, if #2020=0, decomposition action:
G0X10Y10
G0Z0
G1Z-5
G1Z-10
G1Z-15
G0Z0
If #2020=1, the decomposition action:
G0X10Y10
G0Z0
G1Z-5
G0Z-4
G1Z-10
G0Z-9
G1Z-15
G0Z0

Author: Nikolay81 Time: 2018-8-1 21:03
Last edited by Nikolay81 In 2018-8-1 21:04 Editor

ytliu Posted at 2018-8-1 19:09
Execute G99G83X10Y10Z-15R0Q5, if #2021=0, decomposition action:
G0X10Y10
G0Z0

Yes. It's perfect.
Many thanks.
If you can, you need to add a little improvement.
For cycle G83, parameter "G83 Retraction amount" will usually be equal to 0.
In most cases, it is not needed. Since the drill is output completely, at each step.

But for cycle G73, parameter "G73 Retraction amount" is necessary.
Without this parameter, the cycle G73 does not differ from G81.
And for drills of different thicknesses, the value of "G73 Retraction amount" should be different. It is very inconvenient to install the program and change the value in the settings.
Therefore, many manufacturers of CNC machines and postprocessors add one more input parameter to the G73 command. For example, "I".
In this case, it should be used instead of variable # 2020, if specified in the command.
Or, it should temporarily replace the value # 2020, and then return the variable # 2020 to the value specified in the settings.

That is, the command will look like this: G73X0 Y0 Z-5 R0 Q1 K1 I0.5
And in G83 it would be nice to add parameter "I".
Then, they generally can be removed from the settings, so as not to litter them with unnecessary items.

Author: ytliu Time: 2018-8-1 21:33
Last edited by ytliu In 2018-8-1 21:36 Editor

Nikolay81 Posted at 2018-8-1 21:03
Yes. It's perfect.
Many thanks.
If you can, you need to add a little improvement.

I made changes as per your request. Instruction format: G83(G73)X_Y_Z_R_Q_I_K_

slib.zip

1.85 KB, Down times: 672

Author: Nikolay81 Time: 2018-8-1 22:24

ytliu Posted at 2018-8-1 21:33
I made changes as per your request. Instruction format: G83(G73)X_Y_Z_R_Q_I_K_

The G83 cycle now works perfectly.
It is better not to think up.
The G73 cycle does not work properly
With the command G73X0Y0Z-6R0Q2I1K1 F10
From should do such actions:
G0X0Y0
G0Z0
G1Z-2 F10
G0Z-1
G0Z-2
G1Z-4 F10
G0Z-3
G0Z-4
G1Z-6 F10
G0Z0
Instead, it does:
G0X0Y0
G0Z0
G1Z-2 F10
G0Z-1
G1Z-4 F10
G0Z-3
G1Z-6 F10
G0Z0
That is, the drilling time is greatly increased.
The drill is lowered on the working feeder "idle".
That is, it drills air.

Author: ytliu Time: 2018-8-1 22:35

Nikolay81 Posted at 2018-8-1 22:24
The G83 cycle now works perfectly.
It is better not to think up.
The G73 cycle does not work prope ...

try it out

slib.zip

1.85 KB, Down times: 663

Author: Nikolay81 Time: 2018-8-1 23:02

ytliu Posted at 2018-8-1 22:35
try it out

Ideally.
On behalf of all users of DDCSV - thank you very much.
Now their machines will drill, much better.

Settings # 2020 (G73 Retraction amount) and # 2021 (G83 Retraction amount) are no longer needed.
I suppose they can be removed.

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