Disable probe routine to run a router
- Daddio
- Offline
- Junior Member
-
Less
More
- Posts: 30
- Thank you received: 5
30 Sep 2022 17:46 #253115
by Daddio
Disable probe routine to run a router was created by Daddio
Hi everybody,
I am trying to run a router on my plasma table that runs qtplasmac but am not able to get past the probing routine. My process so far has been to home z axis, move it to where I want it to start its plunge which is right above the material, I then zero Z axis. However, when I click cycle start it probes for the the material height which it won't find because I have the float switch locked out. Is there a way to disable the probe routine in a code snippet in SheetCAM at the beginning of a cut and then enable it at the end of cut? I'd like to be able to home z, move to the start of my plunge height, turn on the router, and then tell it to go without a probing sequence.
Thanks,
I am trying to run a router on my plasma table that runs qtplasmac but am not able to get past the probing routine. My process so far has been to home z axis, move it to where I want it to start its plunge which is right above the material, I then zero Z axis. However, when I click cycle start it probes for the the material height which it won't find because I have the float switch locked out. Is there a way to disable the probe routine in a code snippet in SheetCAM at the beginning of a cut and then enable it at the end of cut? I'd like to be able to home z, move to the start of my plunge height, turn on the router, and then tell it to go without a probing sequence.
Thanks,
Please Log in or Create an account to join the conversation.
- snowgoer540
-
- Offline
- Moderator
-
Less
More
- Posts: 2393
- Thank you received: 782
30 Sep 2022 19:03 #253119
by snowgoer540
Replied by snowgoer540 on topic Disable probe routine to run a router
Why don't you just duplicate the pertinent parts of your config and run it on another screen like Axis? QtPlasmaC/PlasmaC is built for plasma.
That said, to answer your question, you can keep Z motion with the following line in a gcode file:
Just note that this was really just intended for a diamond drag scribe, or a marker, or something like that.
linuxcnc.org/docs/devel/html/plasma/qtpl....html#_keep_z_motion
That said, to answer your question, you can keep Z motion with the following line in a gcode file:
#<keep-z-motion> = 1Just note that this was really just intended for a diamond drag scribe, or a marker, or something like that.
linuxcnc.org/docs/devel/html/plasma/qtpl....html#_keep_z_motion
Please Log in or Create an account to join the conversation.
- Daddio
- Offline
- Junior Member
-
Less
More
- Posts: 30
- Thank you received: 5
01 Oct 2022 04:20 #253142
by Daddio
Replied by Daddio on topic Disable probe routine to run a router
Yes, I am using the #<keep-z-motion> = 1 so that my z axis moves. Isn't there an M code that disables the initial probing routine and one to re-enable it? I know I can set up a new screen like Axis, but it seems like there should be a way to do it with M codes.
Please Log in or Create an account to join the conversation.
- phillc54
-
- Offline
- Platinum Member
-
Less
More
- Posts: 5698
- Thank you received: 2081
01 Oct 2022 04:43 #253144
by phillc54
Replied by phillc54 on topic Disable probe routine to run a router
Probing in QtPlasmaC is controlled by the plasmac component and it is not able to be bypassed.
Please Log in or Create an account to join the conversation.
- snowgoer540
-
- Offline
- Moderator
-
Less
More
- Posts: 2393
- Thank you received: 782
01 Oct 2022 15:57 #253183
by snowgoer540
Maybe I am a bit confused as to what you are trying to accomplish. I am not understanding why you need to disable the probe, unless you are trying to use M3 to start your spindle. In that case, I agree with Phill, there is no way to override the probe it's part of the component.
But if you are starting the spindle on your router manually, then I am not sure I understand why keep-z-motion wouldn't work for you.
Say I had this simple program to cut a 4" circle with plasma:
I could use keep z motion to do the same program with a diamond scribe, or marker, etc, but I do need to remove the M3 and M5 starts and stops:
In the latter example, you would set Z0 as the point where the tip of your tool touches the material manually before starting the program. Then when you run, it will cut .25" deep in this example.
I say all of that, but I think the easiest solution is to just make another config to call up and use a purpose built GUI like Axis when you want to use it as a router table...
Replied by snowgoer540 on topic Disable probe routine to run a router
Yes, I am using the #<keep-z-motion> = 1 so that my z axis moves. Isn't there an M code that disables the initial probing routine and one to re-enable it? I know I can set up a new screen like Axis, but it seems like there should be a way to do it with M codes.
Maybe I am a bit confused as to what you are trying to accomplish. I am not understanding why you need to disable the probe, unless you are trying to use M3 to start your spindle. In that case, I agree with Phill, there is no way to override the probe it's part of the component.
But if you are starting the spindle on your router manually, then I am not sure I understand why keep-z-motion wouldn't work for you.
Say I had this simple program to cut a 4" circle with plasma:
Warning: Spoiler!
G20 G64P0.004 G40 G49 G80 G90 G92.1 G94 G97 (preamble)
(conversational circle)
;using material #114: 30A (FineCut Low Speed) Steel 20GA
M190 P114
M66 P3 L3 Q1
f#<_hal[plasmac.cut-feed-rate]>
g0 x2.878448 y3.339448
m3 $0 s1
g2 x2.878448 y3.339448 i1.423052 j1.423052
m5 $0
G20 G64P0.004 G40 G49 G80 G90 G92.1 G94 G97 (postamble)
m2I could use keep z motion to do the same program with a diamond scribe, or marker, etc, but I do need to remove the M3 and M5 starts and stops:
Warning: Spoiler!
G20 G64P0.004 G40 G49 G80 G90 G92.1 G94 G97 (preamble)
(conversational circle)
;using material #114: 30A (FineCut Low Speed) Steel 20GA
M190 P114
M66 P3 L3 Q1
f#<_hal[plasmac.cut-feed-rate]>
#<keep-z-motion> = 1
g0 x2.878448 y3.339448
g1 z-.25
g2 x2.878448 y3.339448 i1.423052 j1.423052
g0 z0
G20 G64P0.004 G40 G49 G80 G90 G92.1 G94 G97 (postamble)
m2In the latter example, you would set Z0 as the point where the tip of your tool touches the material manually before starting the program. Then when you run, it will cut .25" deep in this example.
I say all of that, but I think the easiest solution is to just make another config to call up and use a purpose built GUI like Axis when you want to use it as a router table...
Please Log in or Create an account to join the conversation.
- Daddio
- Offline
- Junior Member
-
Less
More
- Posts: 30
- Thank you received: 5
01 Oct 2022 16:52 #253189
by Daddio
Replied by Daddio on topic Disable probe routine to run a router
I am starting the router manually from one of the user buttons connected to a relay, so I am not using M3 to start the router spindle. The problem is the float switch. Currently, I have it locked out on its floating head for router because otherwise it will constantly be tripped during operation.
There are two scenarios with the float switch at cycle start:
1. Float switch not locked out: At cycle start, Z will be able to find the material during probing routine and will be ready to run. However, the float switch will immediately be tripped when the router contacts the wood and the program will fault out.
2 Float switch locked out: At cycle start, Z will fail to find the material during probing routine and will fault out.
So it seems there are two solution paths:
1. For scenario 1, make the floating head rigid so no more float, then use the float switch for the initial probe routine to find the material, then ignore the float switch during routing. How can I ignore the float switch input after a probing routing?
2. For scenario 2, make the floating head rigid (I've already done this), manually jog the router into position, zero z, then skip the probing routine, and run the job. How can I skip the probing routine?
Thanks
There are two scenarios with the float switch at cycle start:
1. Float switch not locked out: At cycle start, Z will be able to find the material during probing routine and will be ready to run. However, the float switch will immediately be tripped when the router contacts the wood and the program will fault out.
2 Float switch locked out: At cycle start, Z will fail to find the material during probing routine and will fault out.
So it seems there are two solution paths:
1. For scenario 1, make the floating head rigid so no more float, then use the float switch for the initial probe routine to find the material, then ignore the float switch during routing. How can I ignore the float switch input after a probing routing?
2. For scenario 2, make the floating head rigid (I've already done this), manually jog the router into position, zero z, then skip the probing routine, and run the job. How can I skip the probing routine?
Thanks
Please Log in or Create an account to join the conversation.
- snowgoer540
-
- Offline
- Moderator
-
Less
More
- Posts: 2393
- Thank you received: 782
01 Oct 2022 21:08 - 01 Oct 2022 21:45 #253200
by snowgoer540
Replied by snowgoer540 on topic Disable probe routine to run a router
For scenario 1, float switch tripping makes sense. That would cause it to stop the program.
For scenario 2, I still dont understand why it's probing, unless you are leaving M3 commands in the gcode.
Can you please post the gcode you are trying to cut with the router?
For scenario 2, I still dont understand why it's probing, unless you are leaving M3 commands in the gcode.
Can you please post the gcode you are trying to cut with the router?
Last edit: 01 Oct 2022 21:45 by snowgoer540.
Please Log in or Create an account to join the conversation.
- snowgoer540
-
- Offline
- Moderator
-
Less
More
- Posts: 2393
- Thank you received: 782
02 Oct 2022 00:14 #253212
by snowgoer540
Reread this. To answer your question explicitly:
1. Remove M3/M5 commands. M3 will cause the probing routine.
2. Add the line #<keep-z-motion> = 1 near the top of the gcode file.
3. Add your appropriate Z movements before and after your cut path.
Replied by snowgoer540 on topic Disable probe routine to run a router
2. For scenario 2, make the floating head rigid (I've already done this), manually jog the router into position, zero z, then skip the probing routine, and run the job. How can I skip the probing routine?
Reread this. To answer your question explicitly:
1. Remove M3/M5 commands. M3 will cause the probing routine.
2. Add the line #<keep-z-motion> = 1 near the top of the gcode file.
3. Add your appropriate Z movements before and after your cut path.
Please Log in or Create an account to join the conversation.
Moderators: snowgoer540
Time to create page: 0.060 seconds