ATC + TOOL_CHANGE_QUILL_UP
- HalaszAttila
- Offline
- Premium Member
Less
More
- Posts: 142
- Thank you received: 5
04 May 2019 15:05 #132740
by HalaszAttila
ATC + TOOL_CHANGE_QUILL_UP was created by HalaszAttila
Hello,
a working on retrofit Emco VMC100 milling machine.
Before changing the tool (rotating the magazin), Z axis must move to top end position (Z machine coord = 0.0 mm) (restricted area).
I solved this whit setting the TOOL_CHANGE_QUILL_UP = 1 in INI file.
But, would be required to inhibit (motion.feed−inhibit) the axis motion when machine is not in tool change execution,
and Z axis enter in restricted area (halui.axis.N.pos−feedback > -85.0 - checked with comp.N. component)).
-My plan was to use iocontrol.0.tool−change signal to disable checking the position of Z axis and inhibit the motion when it goes above -85.0mm, but this signal is set after moving Z up.
-My second plan was to check the state of motion.motion−type signal (4: Tool change). But when moving Z axis during tool change the value of variable is 1: Traverse (like rapid move), not 4: Tool change (when would be this variable equal 4? )
-My third plan is to remap M6, but is seems complicated, because i do not find docs how to do it.
Can you help me how to solve this problem, easy?
Thanks.
a working on retrofit Emco VMC100 milling machine.
Before changing the tool (rotating the magazin), Z axis must move to top end position (Z machine coord = 0.0 mm) (restricted area).
I solved this whit setting the TOOL_CHANGE_QUILL_UP = 1 in INI file.
But, would be required to inhibit (motion.feed−inhibit) the axis motion when machine is not in tool change execution,
and Z axis enter in restricted area (halui.axis.N.pos−feedback > -85.0 - checked with comp.N. component)).
-My plan was to use iocontrol.0.tool−change signal to disable checking the position of Z axis and inhibit the motion when it goes above -85.0mm, but this signal is set after moving Z up.
-My second plan was to check the state of motion.motion−type signal (4: Tool change). But when moving Z axis during tool change the value of variable is 1: Traverse (like rapid move), not 4: Tool change (when would be this variable equal 4? )
-My third plan is to remap M6, but is seems complicated, because i do not find docs how to do it.
Can you help me how to solve this problem, easy?
Thanks.
Please Log in or Create an account to join the conversation.
04 May 2019 18:53 #132762
by andypugh
Replied by andypugh on topic ATC + TOOL_CHANGE_QUILL_UP
I would use M6 remap. Then the quill up is a g53 g0 move.
linuxcnc.org/docs/2.7/html/remap/remap.h...s_including_tt_m6_tt
This section explains the minimum way to do an M6 remap.
linuxcnc.org/docs/2.7/html/remap/remap.h...s_including_tt_m6_tt
This section explains the minimum way to do an M6 remap.
The following user(s) said Thank You: HalaszAttila
Please Log in or Create an account to join the conversation.
- HalaszAttila
- Offline
- Premium Member
Less
More
- Posts: 142
- Thank you received: 5
08 May 2019 14:22 #133146
by HalaszAttila
Replied by HalaszAttila on topic ATC + TOOL_CHANGE_QUILL_UP
Thanks for suggestion.
I first time try to use M6 remap, and write a atc.ngc file, and it works - sometimes.
1-2 times out of 10 tool changing, the line after M6 in atc.ngc stops, and not executed to end.
The line after M6 (in remap) is G53 G0 Z-92 this moves Z axis back to safety zone (disconnect spindle from the magazin).
When executing the atc.ngc file (Called T1M6 from G code program), every time the M6 (in ngc file) is finished properly (the magazin rotated to desired position and in HAL file i set the iocontrol.0.tool−changed pin),
and after linuxcnc starts executing next line (G53 G0 Z-92) moving Z down but after few mm (not fix length!!! sometimes few tenth mm, sometimes 2-3mm) the moving stops and the tool changing is finished with no error, no message. It seems everything is finished properly, but unfortunately the magazin is stays in restricted area - connected with magazin, and if in the G code program after tool change T1M6 follow spindle start S5000 M3 it will rotate the magazin with high speed and something will brake. Ufffff.
I attached the ngc file.
Please can someone help me what i made wrong?
I use <on_abort> macro. But it not called, that means the atc.ngc finished properly by LinuxCNC.
INI section for remap:
ON_ABORT_COMMAND=O <on_abort> call
# REMAP:
REMAP= M6 modalgroup=6 ngc=atc
[PYTHON]
# where to find Python code
PATH_PREPEND=python
# import the following Python module
TOPLEVEL=python/toplevel.py
# the higher the more verbose tracing of the Python plugin
LOG_LEVEL = 8
I first time try to use M6 remap, and write a atc.ngc file, and it works - sometimes.
1-2 times out of 10 tool changing, the line after M6 in atc.ngc stops, and not executed to end.
The line after M6 (in remap) is G53 G0 Z-92 this moves Z axis back to safety zone (disconnect spindle from the magazin).
When executing the atc.ngc file (Called T1M6 from G code program), every time the M6 (in ngc file) is finished properly (the magazin rotated to desired position and in HAL file i set the iocontrol.0.tool−changed pin),
and after linuxcnc starts executing next line (G53 G0 Z-92) moving Z down but after few mm (not fix length!!! sometimes few tenth mm, sometimes 2-3mm) the moving stops and the tool changing is finished with no error, no message. It seems everything is finished properly, but unfortunately the magazin is stays in restricted area - connected with magazin, and if in the G code program after tool change T1M6 follow spindle start S5000 M3 it will rotate the magazin with high speed and something will brake. Ufffff.
I attached the ngc file.
Please can someone help me what i made wrong?
I use <on_abort> macro. But it not called, that means the atc.ngc finished properly by LinuxCNC.
INI section for remap:
ON_ABORT_COMMAND=O <on_abort> call
# REMAP:
REMAP= M6 modalgroup=6 ngc=atc
[PYTHON]
# where to find Python code
PATH_PREPEND=python
# import the following Python module
TOPLEVEL=python/toplevel.py
# the higher the more verbose tracing of the Python plugin
LOG_LEVEL = 8
Please Log in or Create an account to join the conversation.
08 May 2019 14:39 - 08 May 2019 14:39 #133148
by bevins
Replied by bevins on topic ATC + TOOL_CHANGE_QUILL_UP
Try a G4 P3 after the G0 -Z move.
Last edit: 08 May 2019 14:39 by bevins.
The following user(s) said Thank You: HalaszAttila
Please Log in or Create an account to join the conversation.
08 May 2019 15:09 #133151
by andypugh
Replied by andypugh on topic ATC + TOOL_CHANGE_QUILL_UP
I wonder if you are setting the "tool changed" pin too early and that (somehow) interrupts the sequence?
The following user(s) said Thank You: HalaszAttila
Please Log in or Create an account to join the conversation.
- HalaszAttila
- Offline
- Premium Member
Less
More
- Posts: 142
- Thank you received: 5
08 May 2019 15:22 - 08 May 2019 15:33 #133153
by HalaszAttila
Replied by HalaszAttila on topic ATC + TOOL_CHANGE_QUILL_UP
I tried to delay the tool-changed signal with timedelay (on-time = 0.1 sec). But nothing changed.
I tried that comment out the tool changing section from HAL (carousel comp etc). And the tool-changed pin is simulated:
iocontrol.tool-change timedelay..in
timedelay..out iocontrol.tool-changed.
timedelay ON time: 2.0 sec.
But not solved the problem.
I will try to put G4 P3 before M6 based on previous Replay.
I tried that comment out the tool changing section from HAL (carousel comp etc). And the tool-changed pin is simulated:
iocontrol.tool-change timedelay..in
timedelay..out iocontrol.tool-changed.
timedelay ON time: 2.0 sec.
But not solved the problem.
I will try to put G4 P3 before M6 based on previous Replay.
Last edit: 08 May 2019 15:33 by HalaszAttila.
Please Log in or Create an account to join the conversation.
08 May 2019 15:45 #133157
by bevins
Replied by bevins on topic ATC + TOOL_CHANGE_QUILL_UP
I think it needs to be in the sub
Please Log in or Create an account to join the conversation.
- HalaszAttila
- Offline
- Premium Member
Less
More
- Posts: 142
- Thank you received: 5
09 May 2019 11:04 #133234
by HalaszAttila
Replied by HalaszAttila on topic ATC + TOOL_CHANGE_QUILL_UP
Hmm it seems that problem is from turned on tool offset compensation (G43) during tool change.
When i put on the beginning of atc.ngc a G49 code to turn off compensations, the tool changing is gone without problem (dont stops G53 G0 Z-92 moving after M6).
When i put on the beginning of atc.ngc a G49 code to turn off compensations, the tool changing is gone without problem (dont stops G53 G0 Z-92 moving after M6).
Please Log in or Create an account to join the conversation.
09 May 2019 12:40 #133236
by bevins
That's weird because G53 should still work even with offsets.
Replied by bevins on topic ATC + TOOL_CHANGE_QUILL_UP
Hmm it seems that problem is from turned on tool offset compensation (G43) during tool change.
When i put on the beginning of atc.ngc a G49 code to turn off compensations, the tool changing is gone without problem (dont stops G53 G0 Z-92 moving after M6).
That's weird because G53 should still work even with offsets.
Please Log in or Create an account to join the conversation.
- HalaszAttila
- Offline
- Premium Member
Less
More
- Posts: 142
- Thank you received: 5
09 May 2019 12:56 #133237
by HalaszAttila
Replied by HalaszAttila on topic ATC + TOOL_CHANGE_QUILL_UP
On the graphics seems that (in executing atc.ngc) after finished M6 the coordinate system moves according to Z offset, after that will move Z axis down with G53 G0Z-92 line. This line interrupted after a little time (but without error or message).
With G49 on the beginning of atc.ngc the problem solved.
What you think, can i use it in this form safety?
With G49 on the beginning of atc.ngc the problem solved.
What you think, can i use it in this form safety?
Please Log in or Create an account to join the conversation.
Time to create page: 0.126 seconds