Re: [Emc-users] G33.1 error then g-code file parsed

[Nicklas SB Karlsson]

Using the last version 2.10.0~pre0 this problem is solved so time to
pass this discussion to the trashbin.

Should of course have checked the latest version before starting the
discussion.

Nicklas Karlsson


ons 2023-06-14 klockan 12:27 -0700 skrev John Dammeyer:
> Does your spindle have an encoder and the spindle at speed?
> 
> https://forum.linuxcnc.org/38-general-linuxcnc-questions/43124-g33-1-rigid-tapping
> 
> 
> -Original Message-
> From: Nicklas SB Karlsson [mailto:n...@nksb.eu] 
> Sent: June 14, 2023 12:14 PM
> To: emc-users@lists.sourceforge.net
> Subject: [Emc-users] G33.1 error then g-code file parsed
> 
> I put the lines below into a file:
> 
>  � M3 S100
>  � G33.1 Z-30.474 K0.8 I3.000
>  � M5
>  � M2
> 
> Then I read into Linuxcnc I get error message:
> 
>  � parse_file interp_error
> 
> Removing the line with G33.1 then no error message so it is something
> with this row. Program do however execute as expected with G33.1 line
> even though there is an error message so no real problem. Also
> execute 
> without an error message if run manually in MDI mode. Use
> origin/master 
> last commit Mon May 8 16:10:03 2023 +0200 
> 404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar
> problem?
> 
> 
> Nicklas Karlsson
> 
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
> 
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

One more addendum to this and then I'll leave it alone.
I played around with a few more Z axis accel and spindle speed values.

It looks like it only starts decelerating the spindle to 0 after the Z
distance has finished.  Then Z decelerates as does the spindle.  Since the Z
position after it's stopped exceeds the Z starting point it then moves the Z
back.  So there's an extra Z move in there that wasn't apparent when the
line following the G31 was G01 Z 0.5.
When I removed the Z 0.5 it became clear the Z has overshot Z=0.0 and is
brought back to Z=0.0..

And it looks like Z tries to track the spindle as it decelerates but can't
keep up when the spindle speed is too high and has a high ACCEL value.  

One other interesting side effect.
S200 M3
G33.1 Z-0.7 K0.05 I12

Tapping is done at 200 RPM and  Z=10 IPM.  The return RPM is 2400 RPM and Z
should be 120 IPM.  Both speeds are within the capability of the system.
However it just stops at the end of the retraction point.  The S200 M3
doesn't occur.  No fault message.

John




> -Original Message-
> From: John Dammeyer [mailto:jo...@autoartisans.com]
> Sent: July 5, 2023 12:08 AM
> To: 'Enhanced Machine Controller (EMC)'
> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
> 
> Hi Gene,
> 
> > -Original Message-
> > From: gene heskett [mailto:ghesk...@shentel.net]
> > That Z following until the spindle is completely stopped is a
> > possibility I hadn't considered. And I don't read src code that easily.
> > I have always considered the sync was released when z had been
> withdrawn
> > to the starting point even though inertia is going to make it over shoot
> > and either motion or the PID's are going to force the reset to the
> > starting position, doing it independently.  So if you're correct then
> > we've both learned something.  And your fix would appear to be the
> > correct one. If the z is your knee, turning that around and bringing it
> > back up to 2 or 4 thou is the hardest part of the job.
> >
> > I also don't have any machines with a heavy knee. Out of sight, out of
> > mind. I'll get my coat now.
> >
> 
> I've done some other tests too.  With the reduced acceleration on the
> spindle it takes a while now for it to go from 0 to 3000 RPM.  Here's
what's
> interesting. If I tell it S0 it sets the speed to 0 and does the M5 and
stops
> instantly.  If I do an S1 it slows from 3000 RPM down to 1 RPM and no M5.
> Now if I then do an M5 it stops.  All that makes sense.
> 
> Next.  I have it running at S1200 M4 (CCW).  I then tall it S200 M3.  I
get the
> slow smooth deceleration and then change in direction and acceleration
back
> up to 200 RPM with the new ACCEL values.  Still fairly smooth.
> 
> Therefore I'm guessing that at the end of the I6 which is turning 1200 RPM
> CCW the internal behavior is like immediately executing an M3 with
tracking
> disabled since we no longer want the Z to move the work into the tap
again.
> (or the tap into the work).
> 
> If I put the higher spindle accel values back the change from 600 RPM CCW
to
> 200 RPM CW (the original M3 speed for tapping) is almost instant.
> 
> So why might that be?  My theory is that Z tracks the spindle until it's
reached
> the original start position.
> 
> G33.1 Z-0.7 K0.05 I3.0
> Let's take a look at trajectory planning here remembering like threading
on a
> lathe the Z axis tracks the spindle speed.  The question is what does it
do as
> it's unscrewing the tap.
> 1.  The hole was -0.7" deep.
> 2. Z takes 0.1" to decelerate at 30 ipm (the I3 speed) so starts to
decelerate at
> Z=-0.1 to reach Z0.0.
> 3. The trajectory planner should decelerate the spindle to 0 RPM during
that
> last  0.100" Z axis motion using the Z ACCEL value
> 4. When Z is back at the start (Z=0.000) the spindle should also be
stopped
> and at this point the G33.1 command is complete..
> 5. Except we have to put the spindle back to where we were when it started
> which was S200 M3.
> 
> Except maybe, the system issues the S200 M3 at the -0.1" Z position
> assuming the Z will finish it's deceleration and the spindle will stop and
go
> back to CW at 200 RPM.
> Z (Joint 2) is still tracking the spindle which is now decelerating way
too fast
> and we get the following error.
> 
> Or maybe at Z=-0.1 the system issues an M5 to stop the spindle which it
does
> almost instantly and Z can't keep up and a following error.
> 
> When I change the spindle acceleration so it slows down to zero at a rate
that
> Z can keep up with and I don't get a following error.
> 
> Anyway, the behaviour is now repeatable and I suspect how the I parameter
> is handled with respect to tracking is a problem.
> 
> John
> 
> 
>

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

Hi Gene,

> -Original Message-
> From: gene heskett [mailto:ghesk...@shentel.net]
> That Z following until the spindle is completely stopped is a
> possibility I hadn't considered. And I don't read src code that easily.
> I have always considered the sync was released when z had been withdrawn
> to the starting point even though inertia is going to make it over shoot
> and either motion or the PID's are going to force the reset to the
> starting position, doing it independently.  So if you're correct then
> we've both learned something.  And your fix would appear to be the
> correct one. If the z is your knee, turning that around and bringing it
> back up to 2 or 4 thou is the hardest part of the job.
> 
> I also don't have any machines with a heavy knee. Out of sight, out of
> mind. I'll get my coat now.
>

I've done some other tests too.  With the reduced acceleration on the spindle 
it takes a while now for it to go from 0 to 3000 RPM.  Here's what's 
interesting. If I tell it S0 it sets the speed to 0 and does the M5 and stops 
instantly.  If I do an S1 it slows from 3000 RPM down to 1 RPM and no M5.
Now if I then do an M5 it stops.  All that makes sense.

Next.  I have it running at S1200 M4 (CCW).  I then tall it S200 M3.  I get the 
slow smooth deceleration and then change in direction and acceleration back up 
to 200 RPM with the new ACCEL values.  Still fairly smooth.

Therefore I'm guessing that at the end of the I6 which is turning 1200 RPM CCW 
the internal behavior is like immediately executing an M3 with tracking 
disabled since we no longer want the Z to move the work into the tap again.  
(or the tap into the work).

If I put the higher spindle accel values back the change from 600 RPM CCW to 
200 RPM CW (the original M3 speed for tapping) is almost instant.

So why might that be?  My theory is that Z tracks the spindle until it's 
reached the original start position.

G33.1 Z-0.7 K0.05 I3.0
Let's take a look at trajectory planning here remembering like threading on a 
lathe the Z axis tracks the spindle speed.  The question is what does it do as 
it's unscrewing the tap.
1.  The hole was -0.7" deep.  
2. Z takes 0.1" to decelerate at 30 ipm (the I3 speed) so starts to decelerate 
at Z=-0.1 to reach Z0.0.
3. The trajectory planner should decelerate the spindle to 0 RPM during that 
last  0.100" Z axis motion using the Z ACCEL value
4. When Z is back at the start (Z=0.000) the spindle should also be stopped and 
at this point the G33.1 command is complete..
5. Except we have to put the spindle back to where we were when it started 
which was S200 M3.

Except maybe, the system issues the S200 M3 at the -0.1" Z position assuming 
the Z will finish it's deceleration and the spindle will stop and go back to CW 
at 200 RPM.
Z (Joint 2) is still tracking the spindle which is now decelerating way too 
fast and we get the following error.

Or maybe at Z=-0.1 the system issues an M5 to stop the spindle which it does 
almost instantly and Z can't keep up and a following error.

When I change the spindle acceleration so it slows down to zero at a rate that 
Z can keep up with and I don't get a following error.

Anyway, the behaviour is now repeatable and I suspect how the I parameter is 
handled with respect to tracking is a problem.

John




If the system knows that at Z ACCEL values it takes say 0.1" to come to a halt 
then it likely tells spindle to now slow down to 0 as the Z axis decelerates to 
0 arriving at the Z starting point of the tapping process.
 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[gene heskett]

On 7/4/23 20:09, John Dammeyer wrote:

On 7/4/23 18:18, gene heskett wrote:

On 7/4/23 16:49, John Dammeyer wrote:

Hi Gene,
I think you are overthinking the problem.  .


Lets clarify where the error is, because the turn around at the bottom
of the hole is synchronized, the turn around at the top is not.
So where is it when the error was reported?


The error occurred after the I3 completed.  Recall I3 tells the spindle to turn 
3x as fast CCW as it turned in the other direction CW so 600 RPM.
The spindle is started earlier with an S200 M5.  If  the spindle is up to speed 
at 200 RPM the knee heads up accelerating up to 10 IPM and the tap threads the 
hole.  At the bottom of the hole the spindle is instructed to slow down and the 
Z axis tracks that from 10 IPM down to 0 IPM so that the thread isn't ruined or 
tap broken.

Once the spindle is completely stopped (and the Z axis would be too) the 
spindle is accelerated up to 600 RPM CCW and at the same time the knee is 
accelerated to 30 IPM which is also 3x the amount when it went down.   It has 
no trouble following that because I suspect the acceleration is likely based 
smaller of the two accelerations which is the Z axis acceleration.  After all 
it's a tracking operation so it may not even use the max accel values or the 
min of the two so they can both keep up.

Now,  at the top of the hole once the tap is out the synchronized motion is 
complete and the spindle direction now has to be reversed to return to where it 
was set with the M5 CW rotation.  Here's where it screws up.

It's no longer _required_ to have the Z axis track so I suspect the Spindle 
MAX_ACCEL value is now used.  However from the Z axis perspective it may still 
be trying to track the  CCW spindle until the spindle is stopped.  Therefore we 
have the spindle with a MAX_ACCEL value of 300 and a Z axis MAX_ACCEL  value of 
10.  The Joint2 axis (Z) just can't keep up and that’s when the following error 
happens.

That Z following until the spindle is completely stopped is a 
possibility I hadn't considered. And I don't read src code that easily. 
I have always considered the sync was released when z had been withdrawn 
to the starting point even though inertia is going to make it over shoot 
and either motion or the PID's are going to force the reset to the 
starting position, doing it independently.  So if you're correct then 
we've both learned something.  And your fix would appear to be the 
correct one. If the z is your knee, turning that around and bringing it 
back up to 2 or 4 thou is the hardest part of the job.


I also don't have any machines with a heavy knee. Out of sight, out of 
mind. I'll get my coat now.



So by reducing my spindle acceleration to a more reasonable value which doesn't 
really appear to create problems the Z axis, which I suspect still has tracking 
enabled can now keep up as the spindle slows.  And now I can speed out at I6 or 
1200 RPM  which it does without any Joint 2 tracking errors.

John




That reads like the spindle stop time is overly long to me.


Nope.



Actually the spindle stops so quickly that I can hear the splines
rattle in the pulley driver.


The stop should be so violent the rattle is preloaded to silence.

Do like I've done, add 2 timers in your hal file, one triggered by the
motions direction output, to start when the reverse come in, and is
stopped when the spindle has has stopped as indicated by another timer
set to retrigger for 10 milliseonds on every edge the comes out of the
spindle encoder. The idea it to use this 10 ms lag to indicate the
spindle is slowed enough to be reversed w/o tripping breakers all the
way to the substation, and display the time the first timer is stopped
at in a pyvcp box. I have additional hal stuff to block the reverse from
the spindle control until t is everything but dea stopped, then and only
then do I allow the reversed direction signal into the spindle control,
and the same limit3 then ramps it back up to the chosen speed, with a
mux4 steering the input to the limit3. So the stop is a very fast ramp
down, and the accel ramps it back up to the same speed in the other
direction. 3k max spindle speed fwd to 3k speed in reverse, in under 400
ms. z s/b able to follow that. If not, slow the limit3, giving z a
chance to catch up.� That is assuming the following fault is being
blamed on z..

I'm still convinced a lengthy stop is the problem.
Z is following the encoder.
So block the direction change by making a stop out of it until its
stopped, then allow the direction change thru and ramp it back up to
speed.� To do that right needs a 4 quadrant control.

Your stepper/servo's may be quite precise, but are they true 4 quadrant
control? IDK, but very few stepper drives we can afford are.

Jon's pwm-servo is, a vfd programmed correctly is. Both can stop the
motor by sucking the spin back out, storing that recovered energy in the
psu's filter caps, then using that over voltage to re-accell the motor

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

On 7/4/23 18:18, gene heskett wrote:
> On 7/4/23 16:49, John Dammeyer wrote:
Hi Gene,
I think you are overthinking the problem.  .

> Lets clarify where the error is, because the turn around at the bottom 
> of the hole is synchronized, the turn around at the top is not.
> So where is it when the error was reported?

The error occurred after the I3 completed.  Recall I3 tells the spindle to turn 
3x as fast CCW as it turned in the other direction CW so 600 RPM.
The spindle is started earlier with an S200 M5.  If  the spindle is up to speed 
at 200 RPM the knee heads up accelerating up to 10 IPM and the tap threads the 
hole.  At the bottom of the hole the spindle is instructed to slow down and the 
Z axis tracks that from 10 IPM down to 0 IPM so that the thread isn't ruined or 
tap broken.

Once the spindle is completely stopped (and the Z axis would be too) the 
spindle is accelerated up to 600 RPM CCW and at the same time the knee is 
accelerated to 30 IPM which is also 3x the amount when it went down.   It has 
no trouble following that because I suspect the acceleration is likely based 
smaller of the two accelerations which is the Z axis acceleration.  After all 
it's a tracking operation so it may not even use the max accel values or the 
min of the two so they can both keep up.

Now,  at the top of the hole once the tap is out the synchronized motion is 
complete and the spindle direction now has to be reversed to return to where it 
was set with the M5 CW rotation.  Here's where it screws up.  

It's no longer _required_ to have the Z axis track so I suspect the Spindle 
MAX_ACCEL value is now used.  However from the Z axis perspective it may still 
be trying to track the  CCW spindle until the spindle is stopped.  Therefore we 
have the spindle with a MAX_ACCEL value of 300 and a Z axis MAX_ACCEL  value of 
10.  The Joint2 axis (Z) just can't keep up and that’s when the following error 
happens.

So by reducing my spindle acceleration to a more reasonable value which doesn't 
really appear to create problems the Z axis, which I suspect still has tracking 
enabled can now keep up as the spindle slows.  And now I can speed out at I6 or 
1200 RPM  which it does without any Joint 2 tracking errors.

John


>>
>> That reads like the spindle stop time is overly long to me.

Nope.

>>
>> Actually the spindle stops so quickly that I can hear the splines 
>> rattle in the pulley driver.
> 
> The stop should be so violent the rattle is preloaded to silence.
> 
> Do like I've done, add 2 timers in your hal file, one triggered by the 
> motions direction output, to start when the reverse come in, and is 
> stopped when the spindle has has stopped as indicated by another timer 
> set to retrigger for 10 milliseonds on every edge the comes out of the 
> spindle encoder. The idea it to use this 10 ms lag to indicate the 
> spindle is slowed enough to be reversed w/o tripping breakers all the 
> way to the substation, and display the time the first timer is stopped 
> at in a pyvcp box. I have additional hal stuff to block the reverse from 
> the spindle control until t is everything but dea stopped, then and only 
> then do I allow the reversed direction signal into the spindle control, 
> and the same limit3 then ramps it back up to the chosen speed, with a 
> mux4 steering the input to the limit3. So the stop is a very fast ramp 
> down, and the accel ramps it back up to the same speed in the other 
> direction. 3k max spindle speed fwd to 3k speed in reverse, in under 400 
> ms. z s/b able to follow that. If not, slow the limit3, giving z a 
> chance to catch up.� That is assuming the following fault is being 
> blamed on z..
> 
> I'm still convinced a lengthy stop is the problem.
> Z is following the encoder.
> So block the direction change by making a stop out of it until its 
> stopped, then allow the direction change thru and ramp it back up to 
> speed.� To do that right needs a 4 quadrant control.
> 
> Your stepper/servo's may be quite precise, but are they true 4 quadrant 
> control? IDK, but very few stepper drives we can afford are.
> 
> Jon's pwm-servo is, a vfd programmed correctly is. Both can stop the 
> motor by sucking the spin back out, storing that recovered energy in the 
> psu's filter caps, then using that over voltage to re-accell the motor 
> in the other direction and the only problem is the few ms of the 
> resultant over voltage on the filter caps. The over voltage spike is 
> there and gone again long before the caps fail short from overheating 
> due to the leakage at that voltage peak. I think that high voltage pulse 
> helps to keep an electrolytic formed. Both of my bigger machines are 
> past due for a 5 year recommended shotgun replacement with no sign of 
> ageing yet.
> 
> You may need to check the addf order in your half file, the basic rule 
> is that all addf's should be in an order where a single signal coming in 
> from the machine, should fall thru all processing and 

Re: [Emc-users] G33.1 error then g-code file parsed

[gene heskett]

On 7/4/23 18:18, gene heskett wrote:

On 7/4/23 16:49, John Dammeyer wrote:
The problem is under the covers somewhere and the Joint 2 following 
error isn't totally accurate but is what happens later.

John


Lets clarify where the error is, because the turn around at the bottom 
of the hole is synchronized, the turn around at the top is not.

So where is it when the error was reported?


That reads like the spindle stop time is overly long to me.

Actually the spindle stops so quickly that I can hear the splines 
rattle in the pulley driver.


The stop should be so violent the rattle is preloaded to silence.

Do like I've done, add 2 timers in your hal file, one triggered by the 
motions direction output, to start when the reverse come in, and is 
stopped when the spindle has has stopped as indicated by another timer 
set to retrigger for 10 milliseonds on every edge the comes out of the 
spindle encoder. The idea it to use this 10 ms lag to indicate the 
spindle is slowed enough to be reversed w/o tripping breakers all the 
way to the substation, and display the time the first timer is stopped 
at in a pyvcp box. I have additional hal stuff to block the reverse from 
the spindle control until t is everything but dea stopped, then and only 
then do I allow the reversed direction signal into the spindle control, 
and the same limit3 then ramps it back up to the chosen speed, with a 
mux4 steering the input to the limit3. So the stop is a very fast ramp 
down, and the accel ramps it back up to the same speed in the other 
direction. 3k max spindle speed fwd to 3k speed in reverse, in under 400 
ms. z s/b able to follow that. If not, slow the limit3, giving z a 
chance to catch up.  That is assuming the following fault is being 
blamed on z..


I'm still convinced a lengthy stop is the problem.
Z is following the encoder.
So block the direction change by making a stop out of it until its 
stopped, then allow the direction change thru and ramp it back up to 
speed.  To do that right needs a 4 quadrant control.


Your stepper/servo's may be quite precise, but are they true 4 quadrant 
control? IDK, but very few stepper drives we can afford are.


Jon's pwm-servo is, a vfd programmed correctly is. Both can stop the 
motor by sucking the spin back out, storing that recovered energy in the 
psu's filter caps, then using that over voltage to re-accell the motor 
in the other direction and the only problem is the few ms of the 
resultant over voltage on the filter caps. The over voltage spike is 
there and gone again long before the caps fail short from overheating 
due to the leakage at that voltage peak. I think that high voltage pulse 
helps to keep an electrolytic formed. Both of my bigger machines are 
past due for a 5 year recommended shotgun replacement with no sign of 
ageing yet.


You may need to check the addf order in your half file, the basic rule 
is that all addf's should be in an order where a single signal coming in 
from the machine, should fall thru all processing and go back out to the 
machine in the write at the bottom of same invocation of that thread. 
Violate that rule and all sorts of problems can crawl out of the woodwork.


We need an analyzer script to check that Andy.  Hint hint ;o)>


   I suspect that the spindle stops and then starts back in the 
clockwise direction  too quickly and the Z axis can't do that fast enough.


My spindle is an AC Servo run with step/dir so I could change some 
values in the ini file.


[SPINDLE_9]
MAX_VELOCITY = 50.0
#MAX_ACCELERATION = 30.0
MAX_ACCELERATION = 300.0
# The values below should be 25% larger than MAX_VELOCITY and 
MAX_ACCELERATION

# If using BACKLASH compensation STEPGEN_MAXACCEL should be 100% larger.
STEPGEN_MAXVEL = 62.50
STEPGEN_MAXACCEL = 375.00

The acceleration values of the spindle are dramatically faster than 
the Z axis.

[JOINT_2]
TYPE = LINEAR
HOME = 0.0
FERROR = 0.05
MIN_FERROR = 0.01
# 3.2:1 Max Speed
MAX_VELOCITY = 2.50
MAX_ACCELERATION = 10.0
# The values below should be 25% larger than MAX_VELOCITY and 
MAX_ACCELERATION

# If using BACKLASH compensation STEPGEN_MAXACCEL should be 100% larger.
STEPGEN_MAXVEL = 2.75
STEPGEN_MAXACCEL = 20.0




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users
.


Cheers, Gene Heskett.


Cheers, Gene Heskett.
--
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author, 1940)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[gene heskett]

On 7/4/23 16:49, John Dammeyer wrote:

The problem is under the covers somewhere and the Joint 2 following error isn't 
totally accurate but is what happens later.
John



That reads like the spindle stop time is overly long to me.

Actually the spindle stops so quickly that I can hear the splines rattle in the 
pulley driver.


The stop should be so violent the rattle is preloaded to silence.

Do like I've done, add 2 timers in your hal file, one triggered by the 
motions direction output, to start when the reverse come in, and is 
stopped when the spindle has has stopped as indicated by another timer 
set to retrigger for 10 milliseonds on every edge the comes out of the 
spindle encoder. The idea it to use this 10 ms lag to indicate the 
spindle is slowed enough to be reversed w/o tripping breakers all the 
way to the substation, and display the time the first timer is stopped 
at in a pyvcp box. I have additional hal stuff to block the reverse from 
the spindle control until t is everything but dea stopped, then and only 
then do I allow the reversed direction signal into the spindle control, 
and the same limit3 then ramps it back up to the chosen speed, with a 
mux4 steering the input to the limit3. So the stop is a very fast ramp 
down, and the accel ramps it back up to the same speed in the other 
direction. 3k max spindle speed fwd to 3k speed in reverse, in under 400 
ms. z s/b able to follow that. If not, slow the limit3, giving z a 
chance to catch up.  That is assuming the following fault is being 
blamed on z..


I'm still convinced a lengthy stop is the problem.
Z is following the encoder.
So block the direction change by making a stop out of it until its 
stopped, then allow the direction change thru and ramp it back up to 
speed.  To do that right needs a 4 quadrant control.


Your stepper/servo's may be quite precise, but are they true 4 quadrant 
control? IDK, but very few stepper drives we can afford are.


Jon's pwm-servo is, a vfd programmed correctly is. Both can stop the 
motor by sucking the spin back out, storing that recovered energy in the 
psu's filter caps, then using that over voltage to re-accell the motor 
in the other direction and the only problem is the few ms of the 
resultant over voltage on the filter caps. The over voltage spike is 
there and gone again long before the caps fail short from overheating 
due to the leakage at that voltage peak. I think that high voltage pulse 
helps to keep an electrolytic formed. Both of my bigger machines are 
past due for a 5 year recommended shotgun replacement with no sign of 
ageing yet.


You may need to check the addf order in your half file, the basic rule 
is that all addf's should be in an order where a single signal coming in 
from the machine, should fall thru all processing and go back out to the 
machine in the write at the bottom of same invocation of that thread. 
Violate that rule and all sorts of problems can crawl out of the woodwork.


We need an analyzer script to check that Andy.  Hint hint ;o)>


  I suspect that the spindle stops and then starts back in the 
clockwise direction  too quickly and the Z axis can't do that fast enough.


My spindle is an AC Servo run with step/dir so I could change some values in 
the ini file.

[SPINDLE_9]
MAX_VELOCITY = 50.0
#MAX_ACCELERATION = 30.0
MAX_ACCELERATION = 300.0
# The values below should be 25% larger than MAX_VELOCITY and MAX_ACCELERATION
# If using BACKLASH compensation STEPGEN_MAXACCEL should be 100% larger.
STEPGEN_MAXVEL = 62.50
STEPGEN_MAXACCEL = 375.00

The acceleration values of the spindle are dramatically faster than the Z axis.
[JOINT_2]
TYPE = LINEAR
HOME = 0.0
FERROR = 0.05
MIN_FERROR = 0.01
# 3.2:1 Max Speed
MAX_VELOCITY = 2.50
MAX_ACCELERATION = 10.0
# The values below should be 25% larger than MAX_VELOCITY and MAX_ACCELERATION
# If using BACKLASH compensation STEPGEN_MAXACCEL should be 100% larger.
STEPGEN_MAXVEL = 2.75
STEPGEN_MAXACCEL = 20.0




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users
.


Cheers, Gene Heskett.
--
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author, 1940)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

Update!

[SPINDLE_9]
MAX_VELOCITY = 50.0
MAX_ACCELERATION = 30.0
# The values below should be 25% larger than MAX_VELOCITY and
MAX_ACCELERATION
# If using BACKLASH compensation STEPGEN_MAXACCEL should be 100% larger.
STEPGEN_MAXVEL = 62.50
STEPGEN_MAXACCEL = 37.50

Now I can run S200 for tapping and I6 for the retract and it sounds overall
much smoother.

Not sure why I had the spindle acceleration set so high.
John


-Original Message-
From: John Dammeyer [mailto:jo...@autoartisans.com] 
Sent: July 4, 2023 1:48 PM
To: 'Enhanced Machine Controller (EMC)'
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

> The problem is under the covers somewhere and the Joint 2 following error
isn't totally accurate but is what happens later.
> John
> 

That reads like the spindle stop time is overly long to me.

Actually the spindle stops so quickly that I can hear the splines rattle in
the pulley driver.   I suspect that the spindle stops and then starts back
in the clockwise direction  too quickly and the Z axis can't do that fast
enough.  

My spindle is an AC Servo run with step/dir so I could change some values in
the ini file.

[SPINDLE_9]
MAX_VELOCITY = 50.0
#MAX_ACCELERATION = 30.0
MAX_ACCELERATION = 300.0
# The values below should be 25% larger than MAX_VELOCITY and
MAX_ACCELERATION
# If using BACKLASH compensation STEPGEN_MAXACCEL should be 100% larger.
STEPGEN_MAXVEL = 62.50
STEPGEN_MAXACCEL = 375.00

The acceleration values of the spindle are dramatically faster than the Z
axis.
[JOINT_2]
TYPE = LINEAR
HOME = 0.0
FERROR = 0.05
MIN_FERROR = 0.01
# 3.2:1 Max Speed
MAX_VELOCITY = 2.50
MAX_ACCELERATION = 10.0
# The values below should be 25% larger than MAX_VELOCITY and
MAX_ACCELERATION
# If using BACKLASH compensation STEPGEN_MAXACCEL should be 100% larger.
STEPGEN_MAXVEL = 2.75
STEPGEN_MAXACCEL = 20.0




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

> The problem is under the covers somewhere and the Joint 2 following error 
> isn't totally accurate but is what happens later.
> John
> 

That reads like the spindle stop time is overly long to me.

Actually the spindle stops so quickly that I can hear the splines rattle in the 
pulley driver.   I suspect that the spindle stops and then starts back in the 
clockwise direction  too quickly and the Z axis can't do that fast enough.  

My spindle is an AC Servo run with step/dir so I could change some values in 
the ini file.

[SPINDLE_9]
MAX_VELOCITY = 50.0
#MAX_ACCELERATION = 30.0
MAX_ACCELERATION = 300.0
# The values below should be 25% larger than MAX_VELOCITY and MAX_ACCELERATION
# If using BACKLASH compensation STEPGEN_MAXACCEL should be 100% larger.
STEPGEN_MAXVEL = 62.50
STEPGEN_MAXACCEL = 375.00

The acceleration values of the spindle are dramatically faster than the Z axis.
[JOINT_2]
TYPE = LINEAR
HOME = 0.0
FERROR = 0.05
MIN_FERROR = 0.01
# 3.2:1 Max Speed
MAX_VELOCITY = 2.50
MAX_ACCELERATION = 10.0
# The values below should be 25% larger than MAX_VELOCITY and MAX_ACCELERATION
# If using BACKLASH compensation STEPGEN_MAXACCEL should be 100% larger.
STEPGEN_MAXVEL = 2.75
STEPGEN_MAXACCEL = 20.0




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[gene heskett]

On 7/4/23 03:15, John Dammeyer wrote:

Hi Gene,

I suspect the problem is a bit strange in my case.

I can run the knee at 150 ipm.  The tapping in this case happens at 10 ipm.  
The I3 parameter means it returns at 30 IPM.  I can jog up and down at say 60 
IPM and never get a following error for Joint 2 which is the Z axis.

Since this showed up during the G33.1 I'm going to guess that the deceleration 
of the Z axis compared to the spindle doesn't match what is expected.   Since Z 
can move with G0 motion  (150 ipm) without following errors the problem has 
something to do with the timing of the I3.

I changed the value to S100 so now tapping is at 5 IPM.  It does not create a 
following error with I6 which is 30 IP the same failure speed when it's 10 IPM 
and I3 for 30 IPM.

That suggests again that it's not as obvious as it might appear.  Note in my 
sample below I also move the Z to 0.5 with a G0 .  That's again 150 IPM.  No 
following error.  Therefore given the above experiments the Z axis motion for 
tracking the S200 spindle at I3 has an issue yet doesn't at S100 and I6 which 
is the exact same speed.

The problem is under the covers somewhere and the Joint 2 following error isn't 
totally accurate but is what happens later.
John



That reads like the spindle stop time is overly long to me.

Have you timed the m3/m4 turnaround of the spindle? Mine is a brushed dc 
rated at 1 hp. but at 90 volts, 9.7 amps. The psu can do 25 amps, 
tripping the 20 amp service breaker if it wasn't for the currant limit 
set in Jom Elsons pwm-servo amp, but for the reversal I have some hal 
trickery in the reversal that doesn't just shut the motor down and wait 
for it to coast to a stop, but blocks the reverse dir until its 
essentially stopped by ramping the speed down rapidly, letting the PICO 
pwm-servo, which it a full 4 quadrant servo, pull the rotation energy 
back out of the motor, running that 126 volt supply up to about 170 
volts, actually above the rating of the caps in that supply. By using 
the motor as a generator, the stop can be accomplished from around 10g's 
at the motor is less than 150 ms. Then the fact that an encoder edge 
hasn't arrived recently, the actual dir change is the allowed to get to 
the PID, and the speed is ramped back up to the set revs in the other 
direction, which because of the extra voltage in the psu's caps, can put 
that motor back at speed using that energy in the caps. And its been 
doing that for over 5 years. The actual time to achieve that reversal, 
at 3g's spindle speed is around 400 ms, correspondingly faster at lower 
revs. And my shop lights don't blink, the reversal power bill is 99% 
paid by the 4 quadrant controller.


I'm doing much the same thing on my Sheldon lathe once I had installed 
clamps to keep from unscrewing the chuck, but because that 8" chuck is 
nearly 40 lbs, its hard to stop. I've some hal code there that measures 
the over-travel so I could get an idea of how close I could come to the 
bottom of a blind hole w/o breaking the tap. At 100 rpm, an m4 stop that 
triggers that measurement, displayed on the pyvcp panel, is .24 to .25 
of a revolution. A little math will convert that into actual distance 
the tap will overshoot, which if I write the gcode correctly will be 
subtracted from the depth of that tap preventing the breakage. And 
because the 3 phase synthed controller vfd can be a 4 quadrant control, 
that too works by re-using the stored energy gained from the stop to 
re-accel the motor in the other direction.  And I can do that once a 
second without blinking the shop lights. For several minutes. In this 
case however, there is no PID being used.  The idea is essentially the 
same but a spinx1 is making the analog speed signal for the vfd. The 
encoder is also a much lower resolution, its shop made, ATS-667's hall 
effects watching the teeth of the 60 tooth bull gear on the spindle.


 > -Original Message-

From: gene heskett [mailto:ghesk...@shentel.net]
Sent: July 3, 2023 5:49 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

On 7/3/23 19:32, Nicklas SB Karlsson wrote:

Which version of Linuxcnc did you try it on?


Den 2023-06-28 kl. 19:52, skrev John Dammeyer:

So this morning I whipped up a small g-code program to test the
tapping.� I
started a fresh LinuxCNC so that most of the parameters were default.
Did� a HOME command and then moved to the logical home position with a
G0 X0
Y0 G0 Z0.
Then loaded this program.

G17 G20 G40 G90
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
g0 Z0.5
M5
M2
%

The program loaded without errors.
What's interesting is that this time although the knee went back down
at 3x
the speed after tapping the end result was a "Joint 2 following error"
Remove the I3.0 and the following error does not happen.� Works with I1.5
but not I2.0.


I suspect it should throw a following error at I3 in any event. The docs
are quite conci

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

Hi Gene,

I suspect the problem is a bit strange in my case.

I can run the knee at 150 ipm.  The tapping in this case happens at 10 ipm.  
The I3 parameter means it returns at 30 IPM.  I can jog up and down at say 60 
IPM and never get a following error for Joint 2 which is the Z axis.

Since this showed up during the G33.1 I'm going to guess that the deceleration 
of the Z axis compared to the spindle doesn't match what is expected.   Since Z 
can move with G0 motion  (150 ipm) without following errors the problem has 
something to do with the timing of the I3.

I changed the value to S100 so now tapping is at 5 IPM.  It does not create a 
following error with I6 which is 30 IP the same failure speed when it's 10 IPM 
and I3 for 30 IPM.

That suggests again that it's not as obvious as it might appear.  Note in my 
sample below I also move the Z to 0.5 with a G0 .  That's again 150 IPM.  No 
following error.  Therefore given the above experiments the Z axis motion for 
tracking the S200 spindle at I3 has an issue yet doesn't at S100 and I6 which 
is the exact same speed.

The problem is under the covers somewhere and the Joint 2 following error isn't 
totally accurate but is what happens later.
John

-Original Message-
From: gene heskett [mailto:ghesk...@shentel.net] 
Sent: July 3, 2023 5:49 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

On 7/3/23 19:32, Nicklas SB Karlsson wrote:
> Which version of Linuxcnc did you try it on?
> 
> 
> Den 2023-06-28 kl. 19:52, skrev John Dammeyer:
>> So this morning I whipped up a small g-code program to test the 
>> tapping.� I
>> started a fresh LinuxCNC so that most of the parameters were default.
>> Did� a HOME command and then moved to the logical home position with a 
>> G0 X0
>> Y0 G0 Z0.
>> Then loaded this program.
>>
>> G17 G20 G40 G90
>> G1 X0 Y0 F20
>> G1 Z0
>> S200 M3
>> G33.1 Z-0.7 K0.05 I3.0
>> g0 Z0.5
>> M5
>> M2
>> %
>>
>> The program loaded without errors.
>> What's interesting is that this time although the knee went back down 
>> at 3x
>> the speed after tapping the end result was a "Joint 2 following error"
>> Remove the I3.0 and the following error does not happen.� Works with I1.5
>> but not I2.0.
>>
I suspect it should throw a following error at I3 in any event. The docs 
are quite concise:

"I - optional spindle speed multiplier for faster return move"

And your machine is not able to follow that great a speedup.  It may 
also be suffering from excessive backlash as that move also takes time 
that throws following errors quite easily for backlash comps over a thou 
in my experience here.

YMMV of course. Since that is z motion, and heads or knees are heavy, 
there is effectively no backlash as long as the withdrawal speed is 
below gravity's acceleration AND the spindle has the speed reserve to 
keep up.

I'd try -I1.5 as a half the 3 compromise and gradually increase/decrease 
it to see where the limit might be on your machine. Or not use the I 
option. Don't forget that 3x the spindle speed may be beyond the 
spindles capability. Even a slightly out of tune PID can affect how well 
the -I option works.  I haven't used it myself, but I'd assume a -I0.5, 
would slow the return on a moving head machine. In case the weight of 
the head is almost more that the motor can lift.

Some experimentation to find the limits of your machine is in order, but 
I believe I'd tap air, its cheaper than broken taps. ;o)>

>> Not sure why that is.� It worked the other day, even from the MDI 
>> entry with
>> I3.0.� And now it also generates the following error from the MDI.
>>
>> I'm going to guess either the machine is cold and a bit stiff or there 
>> were
>> some other parameters the other day set that prevented the fault.
>> In either case, I do not get a fault loading the program.
>>
>> John
>>
>>
>> -Original Message-
>> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
>> Sent: June 28, 2023 6:30 AM
>> To: emc-users@lists.sourceforge.net
>> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
>>
>> Have used the latest origin/master not more than a few weeks old but
>> have not checked against older version. Will do this sooner or later,
>> hopefully within a week.
>>
>>
>> Den 2023-06-26 kl. 07:29, skrev John Dammeyer:
>>> OK.
>>> I'll try that for you.
>>> I'm wondering if perhaps spindle acceleration time or some other HAL
>>> parameter gets flagged with an incorrect error message.�� I've done 
>>> power
>>> tapping from .ngc files without issue but I've not used the 'I' 
>>> parameter.
>>

Re: [Emc-users] G33.1 error then g-code file parsed

[gene heskett]

On 7/3/23 19:32, Nicklas SB Karlsson wrote:

Which version of Linuxcnc did you try it on?


Den 2023-06-28 kl. 19:52, skrev John Dammeyer:
So this morning I whipped up a small g-code program to test the 
tapping.  I

started a fresh LinuxCNC so that most of the parameters were default.
Did  a HOME command and then moved to the logical home position with a 
G0 X0

Y0 G0 Z0.
Then loaded this program.

G17 G20 G40 G90
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
g0 Z0.5
M5
M2
%

The program loaded without errors.
What's interesting is that this time although the knee went back down 
at 3x

the speed after tapping the end result was a "Joint 2 following error"
Remove the I3.0 and the following error does not happen.  Works with I1.5
but not I2.0.

I suspect it should throw a following error at I3 in any event. The docs 
are quite concise:


"I - optional spindle speed multiplier for faster return move"

And your machine is not able to follow that great a speedup.  It may 
also be suffering from excessive backlash as that move also takes time 
that throws following errors quite easily for backlash comps over a thou 
in my experience here.


YMMV of course. Since that is z motion, and heads or knees are heavy, 
there is effectively no backlash as long as the withdrawal speed is 
below gravity's acceleration AND the spindle has the speed reserve to 
keep up.


I'd try -I1.5 as a half the 3 compromise and gradually increase/decrease 
it to see where the limit might be on your machine. Or not use the I 
option. Don't forget that 3x the spindle speed may be beyond the 
spindles capability. Even a slightly out of tune PID can affect how well 
the -I option works.  I haven't used it myself, but I'd assume a -I0.5, 
would slow the return on a moving head machine. In case the weight of 
the head is almost more that the motor can lift.


Some experimentation to find the limits of your machine is in order, but 
I believe I'd tap air, its cheaper than broken taps. ;o)>


Not sure why that is.  It worked the other day, even from the MDI 
entry with

I3.0.  And now it also generates the following error from the MDI.

I'm going to guess either the machine is cold and a bit stiff or there 
were

some other parameters the other day set that prevented the fault.
In either case, I do not get a fault loading the program.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 28, 2023 6:30 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Have used the latest origin/master not more than a few weeks old but
have not checked against older version. Will do this sooner or later,
hopefully within a week.


Den 2023-06-26 kl. 07:29, skrev John Dammeyer:

OK.
I'll try that for you.
I'm wondering if perhaps spindle acceleration time or some other HAL
parameter gets flagged with an incorrect error message.   I've done 
power
tapping from .ngc files without issue but I've not used the 'I' 
parameter.

John

-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 10:09 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Run from MDI then there is no error message for me either. Put the same
rows in a .ngc file adding M2 and bottom there is an interpreter error
message then loading the file and display not updated. Looking at bottom
the program is however actually loaded and seems to work OK.


Nicklas Karlsson


Den 2023-06-26 kl. 01:26, skrev John Dammeyer:

I ran the following commands from the MDI without issue from AXIS 2.8.1

with

MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
M5

Interesting watching the spindle RPM indicator, and you can hear it too

of

course.
Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
Reverses and goes up at 600 RPM.
Without the I3.0 it goes up at 200 RPM.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 9:07 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

There is positioning move XYZ in real program but happened to remove
them then I should make a small test case.

Adding positioning move to test case make no difference. Linuxcnc 
report

a file interpretation error and do not update display but program seems
to work supposed to.

Nicklas Karlsson


Den 2023-06-23 kl. 16:20, skrev Chris Radek:

I would add positioning moves (positioning all of XYZ) before the
G33.1 because otherwise the tapped hole can be anywhere - the
program is indeterminate.  This sure might mess up any attempt by
your GUI to check the program or generate a preview.

Chris

On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:

I put the lines below into a file:

 ?? M3 S100
 ?? G33.1 Z-30.474 K0.8 I3.000
 ?

Re: [Emc-users] G33.1 error then g-code file parsed

[gene heskett]

On 7/3/23 18:47, Nicklas SB Karlsson wrote:

Trying 2.9 it did not here. Same problem with master.

Checking out 2.8 and compiling it complain python is not found. If I 
remember correct there have been change of python version. You use 2.8 
or older?


My buster machines are using python 3.7, its 3.8 and beyond that breaks 
it here.


Nicklas Karlsson


Den 2023-06-28 kl. 19:52, skrev John Dammeyer:
So this morning I whipped up a small g-code program to test the 
tapping.  I

started a fresh LinuxCNC so that most of the parameters were default.
Did  a HOME command and then moved to the logical home position with a 
G0 X0

Y0 G0 Z0.
Then loaded this program.

G17 G20 G40 G90
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
g0 Z0.5
M5
M2
%

The program loaded without errors.
What's interesting is that this time although the knee went back down 
at 3x

the speed after tapping the end result was a "Joint 2 following error"
Remove the I3.0 and the following error does not happen.  Works with I1.5
but not I2.0.

Not sure why that is.  It worked the other day, even from the MDI 
entry with

I3.0.  And now it also generates the following error from the MDI.

I'm going to guess either the machine is cold and a bit stiff or there 
were

some other parameters the other day set that prevented the fault.
In either case, I do not get a fault loading the program.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 28, 2023 6:30 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Have used the latest origin/master not more than a few weeks old but
have not checked against older version. Will do this sooner or later,
hopefully within a week.


Den 2023-06-26 kl. 07:29, skrev John Dammeyer:

OK.
I'll try that for you.
I'm wondering if perhaps spindle acceleration time or some other HAL
parameter gets flagged with an incorrect error message.   I've done 
power
tapping from .ngc files without issue but I've not used the 'I' 
parameter.

John

-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 10:09 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Run from MDI then there is no error message for me either. Put the same
rows in a .ngc file adding M2 and bottom there is an interpreter error
message then loading the file and display not updated. Looking at bottom
the program is however actually loaded and seems to work OK.


Nicklas Karlsson


Den 2023-06-26 kl. 01:26, skrev John Dammeyer:

I ran the following commands from the MDI without issue from AXIS 2.8.1

with

MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
M5

Interesting watching the spindle RPM indicator, and you can hear it too

of

course.
Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
Reverses and goes up at 600 RPM.
Without the I3.0 it goes up at 200 RPM.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 9:07 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

There is positioning move XYZ in real program but happened to remove
them then I should make a small test case.

Adding positioning move to test case make no difference. Linuxcnc 
report

a file interpretation error and do not update display but program seems
to work supposed to.

Nicklas Karlsson


Den 2023-06-23 kl. 16:20, skrev Chris Radek:

I would add positioning moves (positioning all of XYZ) before the
G33.1 because otherwise the tapped hole can be anywhere - the
program is indeterminate.  This sure might mess up any attempt by
your GUI to check the program or generate a preview.

Chris

On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:

I put the lines below into a file:

 ?? M3 S100
 ?? G33.1 Z-30.474 K0.8 I3.000
 ?? M5
 ?? M2

Then I read into Linuxcnc I get error message:

 ?? parse_file interp_error

Removing the line with G33.1 then no error message so it is something
with this row. Program do however execute as expected with G33.1 line
even though there is an error message so no real problem. Also 
execute
without an error message if run manually in MDI mode. Use 
origin/master

last commit Mon May 8 16:10:03 2023 +0200
404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar

problem?

Nicklas Karlsson



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/lis

Re: [Emc-users] G33.1 error then g-code file parsed

[gene heskett]

On 7/3/23 18:47, Nicklas SB Karlsson wrote:

Trying 2.9 it did not here. Same problem with master.

Checking out 2.8 and compiling it complain python is not found. If I 
remember correct there have been change of python version. You use 2.8 
or older?
Precisely the problem I reported 2 years ago, the bullseye version of 
python was too new. So my rpi4 is still running buster, in armv7 flavor.


Now its been a long time, couple months since I have gotten a new build 
of linuxcnc from the buildbot for armhf/buster, so I'm only getting docs 
updates when I update.  My lonely rpi4b is running the older buster 
quite well, so when do I see fresh builds of master? For buster, or has 
the new build been fixed for only arm64? I suspect latencytest will 
suffer on armv8.


I'm finding that the even faster bananapi-m5's are running my 3d 
printers quite well. They have all 4 usb ports at usb-3.1 speeds, but 
will rpspi be able to adapt to the 7i90HD interface I'm using?


So, what am I supposed to do next with all my buster machines?



Nicklas Karlsson


Den 2023-06-28 kl. 19:52, skrev John Dammeyer:
So this morning I whipped up a small g-code program to test the 
tapping.  I

started a fresh LinuxCNC so that most of the parameters were default.
Did  a HOME command and then moved to the logical home position with a 
G0 X0

Y0 G0 Z0.
Then loaded this program.

G17 G20 G40 G90
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
g0 Z0.5
M5
M2
%

The program loaded without errors.
What's interesting is that this time although the knee went back down 
at 3x

the speed after tapping the end result was a "Joint 2 following error"
Remove the I3.0 and the following error does not happen.  Works with I1.5
but not I2.0.

Not sure why that is.  It worked the other day, even from the MDI 
entry with

I3.0.  And now it also generates the following error from the MDI.

I'm going to guess either the machine is cold and a bit stiff or there 
were

some other parameters the other day set that prevented the fault.
In either case, I do not get a fault loading the program.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 28, 2023 6:30 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Have used the latest origin/master not more than a few weeks old but
have not checked against older version. Will do this sooner or later,
hopefully within a week.


Den 2023-06-26 kl. 07:29, skrev John Dammeyer:

OK.
I'll try that for you.
I'm wondering if perhaps spindle acceleration time or some other HAL
parameter gets flagged with an incorrect error message.   I've done 
power
tapping from .ngc files without issue but I've not used the 'I' 
parameter.

John

-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 10:09 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Run from MDI then there is no error message for me either. Put the same
rows in a .ngc file adding M2 and bottom there is an interpreter error
message then loading the file and display not updated. Looking at bottom
the program is however actually loaded and seems to work OK.


Nicklas Karlsson


Den 2023-06-26 kl. 01:26, skrev John Dammeyer:

I ran the following commands from the MDI without issue from AXIS 2.8.1

with

MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
M5

Interesting watching the spindle RPM indicator, and you can hear it too

of

course.
Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
Reverses and goes up at 600 RPM.
Without the I3.0 it goes up at 200 RPM.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 9:07 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

There is positioning move XYZ in real program but happened to remove
them then I should make a small test case.

Adding positioning move to test case make no difference. Linuxcnc 
report

a file interpretation error and do not update display but program seems
to work supposed to.

Nicklas Karlsson


Den 2023-06-23 kl. 16:20, skrev Chris Radek:

I would add positioning moves (positioning all of XYZ) before the
G33.1 because otherwise the tapped hole can be anywhere - the
program is indeterminate.  This sure might mess up any attempt by
your GUI to check the program or generate a preview.

Chris

On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:

I put the lines below into a file:

 ?? M3 S100
 ?? G33.1 Z-30.474 K0.8 I3.000
 ?? M5
 ?? M2

Then I read into Linuxcnc I get error message:

 ?? parse_file interp_error

Removing the line with G33.1 then no error message so it is something
with this row. Program do however execute as expected with G33.1 line
even though there is an error message so no rea

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

>From way down earlier.
>> Den 2023-06-26 kl. 01:26, skrev John Dammeyer:
>>> I ran the following commands from the MDI without issue from AXIS 
>>> 2.8.1
>> with
>>> MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.

I don't rebuild LCNC on this system.  If I need to update I'll connect to
the network and do an the online apt get etc.  Biggest change I made from
2.7 to 2.8 was to add the support for Joints.  Other than that I can't
really see why I'd update to 2.9 for the same reason it took me 13 years to
go from WIN-7 to WIN-10.  No apparent value and usually a ton of extra work
to "Enhance my user experience!".
John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu] 
Sent: July 3, 2023 4:31 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Which version of Linuxcnc did you try it on?


Den 2023-06-28 kl. 19:52, skrev John Dammeyer:
> So this morning I whipped up a small g-code program to test the tapping.
I
> started a fresh LinuxCNC so that most of the parameters were default.
> Did  a HOME command and then moved to the logical home position with a G0
X0
> Y0 G0 Z0.
> Then loaded this program.
>
> G17 G20 G40 G90
> G1 X0 Y0 F20
> G1 Z0
> S200 M3
> G33.1 Z-0.7 K0.05 I3.0
> g0 Z0.5
> M5
> M2
> %
>
> The program loaded without errors.
> What's interesting is that this time although the knee went back down at
3x
> the speed after tapping the end result was a "Joint 2 following error"
> Remove the I3.0 and the following error does not happen.  Works with I1.5
> but not I2.0.
>
> Not sure why that is.  It worked the other day, even from the MDI entry
with
> I3.0.  And now it also generates the following error from the MDI.
>
> I'm going to guess either the machine is cold and a bit stiff or there
were
> some other parameters the other day set that prevented the fault.
> In either case, I do not get a fault loading the program.
>
> John
>
>
> -----Original Message-
> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
> Sent: June 28, 2023 6:30 AM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
>
> Have used the latest origin/master not more than a few weeks old but
> have not checked against older version. Will do this sooner or later,
> hopefully within a week.
>
>
> Den 2023-06-26 kl. 07:29, skrev John Dammeyer:
>> OK.
>> I'll try that for you.
>> I'm wondering if perhaps spindle acceleration time or some other HAL
>> parameter gets flagged with an incorrect error message.   I've done power
>> tapping from .ngc files without issue but I've not used the 'I'
parameter.
>> John
>>
>> -Original Message-
>> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
>> Sent: June 25, 2023 10:09 PM
>> To: emc-users@lists.sourceforge.net
>> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
>>
>> Run from MDI then there is no error message for me either. Put the same
>> rows in a .ngc file adding M2 and bottom there is an interpreter error
>> message then loading the file and display not updated. Looking at bottom
>> the program is however actually loaded and seems to work OK.
>>
>>
>> Nicklas Karlsson
>>
>>
>> Den 2023-06-26 kl. 01:26, skrev John Dammeyer:
>>> I ran the following commands from the MDI without issue from AXIS 2.8.1
>> with
>>> MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
>>> G1 X0 Y0 F20
>>> G1 Z0
>>> S200 M3
>>> G33.1 Z-0.7 K0.05 I3.0
>>> M5
>>>
>>> Interesting watching the spindle RPM indicator, and you can hear it too
> of
>>> course.
>>> Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
>>> Reverses and goes up at 600 RPM.
>>> Without the I3.0 it goes up at 200 RPM.
>>>
>>> John
>>>
>>>
>>> -Original Message-
>>> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
>>> Sent: June 25, 2023 9:07 AM
>>> To: emc-users@lists.sourceforge.net
>>> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
>>>
>>> There is positioning move XYZ in real program but happened to remove
>>> them then I should make a small test case.
>>>
>>> Adding positioning move to test case make no difference. Linuxcnc report
>>> a file interpretation error and do not update display but program seems
>>> to work supposed to.
>>>
>>> Nicklas Karlsson
>>>
>>>
>>> Den 2023-06-23 kl. 16:

Re: [Emc-users] G33.1 error then g-code file parsed

[Nicklas SB Karlsson]

Which version of Linuxcnc did you try it on?


Den 2023-06-28 kl. 19:52, skrev John Dammeyer:

So this morning I whipped up a small g-code program to test the tapping.  I
started a fresh LinuxCNC so that most of the parameters were default.
Did  a HOME command and then moved to the logical home position with a G0 X0
Y0 G0 Z0.
Then loaded this program.

G17 G20 G40 G90
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
g0 Z0.5
M5
M2
%

The program loaded without errors.
What's interesting is that this time although the knee went back down at 3x
the speed after tapping the end result was a "Joint 2 following error"
Remove the I3.0 and the following error does not happen.  Works with I1.5
but not I2.0.

Not sure why that is.  It worked the other day, even from the MDI entry with
I3.0.  And now it also generates the following error from the MDI.

I'm going to guess either the machine is cold and a bit stiff or there were
some other parameters the other day set that prevented the fault.
In either case, I do not get a fault loading the program.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 28, 2023 6:30 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Have used the latest origin/master not more than a few weeks old but
have not checked against older version. Will do this sooner or later,
hopefully within a week.


Den 2023-06-26 kl. 07:29, skrev John Dammeyer:

OK.
I'll try that for you.
I'm wondering if perhaps spindle acceleration time or some other HAL
parameter gets flagged with an incorrect error message.   I've done power
tapping from .ngc files without issue but I've not used the 'I' parameter.
John

-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 10:09 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Run from MDI then there is no error message for me either. Put the same
rows in a .ngc file adding M2 and bottom there is an interpreter error
message then loading the file and display not updated. Looking at bottom
the program is however actually loaded and seems to work OK.


Nicklas Karlsson


Den 2023-06-26 kl. 01:26, skrev John Dammeyer:

I ran the following commands from the MDI without issue from AXIS 2.8.1

with

MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
M5

Interesting watching the spindle RPM indicator, and you can hear it too

of

course.
Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
Reverses and goes up at 600 RPM.
Without the I3.0 it goes up at 200 RPM.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 9:07 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

There is positioning move XYZ in real program but happened to remove
them then I should make a small test case.

Adding positioning move to test case make no difference. Linuxcnc report
a file interpretation error and do not update display but program seems
to work supposed to.

Nicklas Karlsson


Den 2023-06-23 kl. 16:20, skrev Chris Radek:

I would add positioning moves (positioning all of XYZ) before the
G33.1 because otherwise the tapped hole can be anywhere - the
program is indeterminate.  This sure might mess up any attempt by
your GUI to check the program or generate a preview.

Chris

On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:

I put the lines below into a file:

 ?? M3 S100
 ?? G33.1 Z-30.474 K0.8 I3.000
 ?? M5
 ?? M2

Then I read into Linuxcnc I get error message:

 ?? parse_file interp_error

Removing the line with G33.1 then no error message so it is something
with this row. Program do however execute as expected with G33.1 line
even though there is an error message so no real problem. Also execute
without an error message if run manually in MDI mode. Use origin/master
last commit Mon May 8 16:10:03 2023 +0200
404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar

problem?

Nicklas Karlsson



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/lis

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

If I type python from the command line I get 2.7.13.  If I type python3 I
get python 3.5. 


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu] 
Sent: July 3, 2023 3:46 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Trying 2.9 it did not here. Same problem with master.

Checking out 2.8 and compiling it complain python is not found. If I 
remember correct there have been change of python version. You use 2.8 
or older?


Nicklas Karlsson


Den 2023-06-28 kl. 19:52, skrev John Dammeyer:
> So this morning I whipped up a small g-code program to test the tapping.
I
> started a fresh LinuxCNC so that most of the parameters were default.
> Did  a HOME command and then moved to the logical home position with a G0
X0
> Y0 G0 Z0.
> Then loaded this program.
>
> G17 G20 G40 G90
> G1 X0 Y0 F20
> G1 Z0
> S200 M3
> G33.1 Z-0.7 K0.05 I3.0
> g0 Z0.5
> M5
> M2
> %
>
> The program loaded without errors.
> What's interesting is that this time although the knee went back down at
3x
> the speed after tapping the end result was a "Joint 2 following error"
> Remove the I3.0 and the following error does not happen.  Works with I1.5
> but not I2.0.
>
> Not sure why that is.  It worked the other day, even from the MDI entry
with
> I3.0.  And now it also generates the following error from the MDI.
>
> I'm going to guess either the machine is cold and a bit stiff or there
were
> some other parameters the other day set that prevented the fault.
> In either case, I do not get a fault loading the program.
>
> John
>
>
> -Original Message-
> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
> Sent: June 28, 2023 6:30 AM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
>
> Have used the latest origin/master not more than a few weeks old but
> have not checked against older version. Will do this sooner or later,
> hopefully within a week.
>
>
> Den 2023-06-26 kl. 07:29, skrev John Dammeyer:
>> OK.
>> I'll try that for you.
>> I'm wondering if perhaps spindle acceleration time or some other HAL
>> parameter gets flagged with an incorrect error message.   I've done power
>> tapping from .ngc files without issue but I've not used the 'I'
parameter.
>> John
>>
>> -Original Message-
>> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
>> Sent: June 25, 2023 10:09 PM
>> To: emc-users@lists.sourceforge.net
>> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
>>
>> Run from MDI then there is no error message for me either. Put the same
>> rows in a .ngc file adding M2 and bottom there is an interpreter error
>> message then loading the file and display not updated. Looking at bottom
>> the program is however actually loaded and seems to work OK.
>>
>>
>> Nicklas Karlsson
>>
>>
>> Den 2023-06-26 kl. 01:26, skrev John Dammeyer:
>>> I ran the following commands from the MDI without issue from AXIS 2.8.1
>> with
>>> MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
>>> G1 X0 Y0 F20
>>> G1 Z0
>>> S200 M3
>>> G33.1 Z-0.7 K0.05 I3.0
>>> M5
>>>
>>> Interesting watching the spindle RPM indicator, and you can hear it too
> of
>>> course.
>>> Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
>>> Reverses and goes up at 600 RPM.
>>> Without the I3.0 it goes up at 200 RPM.
>>>
>>> John
>>>
>>>
>>> -Original Message-
>>> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
>>> Sent: June 25, 2023 9:07 AM
>>> To: emc-users@lists.sourceforge.net
>>> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
>>>
>>> There is positioning move XYZ in real program but happened to remove
>>> them then I should make a small test case.
>>>
>>> Adding positioning move to test case make no difference. Linuxcnc report
>>> a file interpretation error and do not update display but program seems
>>> to work supposed to.
>>>
>>> Nicklas Karlsson
>>>
>>>
>>> Den 2023-06-23 kl. 16:20, skrev Chris Radek:
>>>> I would add positioning moves (positioning all of XYZ) before the
>>>> G33.1 because otherwise the tapped hole can be anywhere - the
>>>> program is indeterminate.  This sure might mess up any attempt by
>>>> your GUI to check the program or generate a preview.
>>>>
>>>> Chris
>>>&g

Re: [Emc-users] G33.1 error then g-code file parsed

[Nicklas SB Karlsson]

Trying 2.9 it did not here. Same problem with master.

Checking out 2.8 and compiling it complain python is not found. If I 
remember correct there have been change of python version. You use 2.8 
or older?



Nicklas Karlsson


Den 2023-06-28 kl. 19:52, skrev John Dammeyer:

So this morning I whipped up a small g-code program to test the tapping.  I
started a fresh LinuxCNC so that most of the parameters were default.
Did  a HOME command and then moved to the logical home position with a G0 X0
Y0 G0 Z0.
Then loaded this program.

G17 G20 G40 G90
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
g0 Z0.5
M5
M2
%

The program loaded without errors.
What's interesting is that this time although the knee went back down at 3x
the speed after tapping the end result was a "Joint 2 following error"
Remove the I3.0 and the following error does not happen.  Works with I1.5
but not I2.0.

Not sure why that is.  It worked the other day, even from the MDI entry with
I3.0.  And now it also generates the following error from the MDI.

I'm going to guess either the machine is cold and a bit stiff or there were
some other parameters the other day set that prevented the fault.
In either case, I do not get a fault loading the program.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 28, 2023 6:30 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Have used the latest origin/master not more than a few weeks old but
have not checked against older version. Will do this sooner or later,
hopefully within a week.


Den 2023-06-26 kl. 07:29, skrev John Dammeyer:

OK.
I'll try that for you.
I'm wondering if perhaps spindle acceleration time or some other HAL
parameter gets flagged with an incorrect error message.   I've done power
tapping from .ngc files without issue but I've not used the 'I' parameter.
John

-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 10:09 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Run from MDI then there is no error message for me either. Put the same
rows in a .ngc file adding M2 and bottom there is an interpreter error
message then loading the file and display not updated. Looking at bottom
the program is however actually loaded and seems to work OK.


Nicklas Karlsson


Den 2023-06-26 kl. 01:26, skrev John Dammeyer:

I ran the following commands from the MDI without issue from AXIS 2.8.1

with

MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
M5

Interesting watching the spindle RPM indicator, and you can hear it too

of

course.
Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
Reverses and goes up at 600 RPM.
Without the I3.0 it goes up at 200 RPM.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 9:07 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

There is positioning move XYZ in real program but happened to remove
them then I should make a small test case.

Adding positioning move to test case make no difference. Linuxcnc report
a file interpretation error and do not update display but program seems
to work supposed to.

Nicklas Karlsson


Den 2023-06-23 kl. 16:20, skrev Chris Radek:

I would add positioning moves (positioning all of XYZ) before the
G33.1 because otherwise the tapped hole can be anywhere - the
program is indeterminate.  This sure might mess up any attempt by
your GUI to check the program or generate a preview.

Chris

On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:

I put the lines below into a file:

 ?? M3 S100
 ?? G33.1 Z-30.474 K0.8 I3.000
 ?? M5
 ?? M2

Then I read into Linuxcnc I get error message:

 ?? parse_file interp_error

Removing the line with G33.1 then no error message so it is something
with this row. Program do however execute as expected with G33.1 line
even though there is an error message so no real problem. Also execute
without an error message if run manually in MDI mode. Use origin/master
last commit Mon May 8 16:10:03 2023 +0200
404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar

problem?

Nicklas Karlsson



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

So this morning I whipped up a small g-code program to test the tapping.  I
started a fresh LinuxCNC so that most of the parameters were default.
Did  a HOME command and then moved to the logical home position with a G0 X0
Y0 G0 Z0.
Then loaded this program.

G17 G20 G40 G90
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
g0 Z0.5
M5
M2
%

The program loaded without errors.
What's interesting is that this time although the knee went back down at 3x
the speed after tapping the end result was a "Joint 2 following error"
Remove the I3.0 and the following error does not happen.  Works with I1.5
but not I2.0.

Not sure why that is.  It worked the other day, even from the MDI entry with
I3.0.  And now it also generates the following error from the MDI.

I'm going to guess either the machine is cold and a bit stiff or there were
some other parameters the other day set that prevented the fault.
In either case, I do not get a fault loading the program.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu] 
Sent: June 28, 2023 6:30 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Have used the latest origin/master not more than a few weeks old but 
have not checked against older version. Will do this sooner or later, 
hopefully within a week.


Den 2023-06-26 kl. 07:29, skrev John Dammeyer:
> OK.
> I'll try that for you.
> I'm wondering if perhaps spindle acceleration time or some other HAL
> parameter gets flagged with an incorrect error message.   I've done power
> tapping from .ngc files without issue but I've not used the 'I' parameter.
> John
>
> -Original Message-
> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
> Sent: June 25, 2023 10:09 PM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
>
> Run from MDI then there is no error message for me either. Put the same
> rows in a .ngc file adding M2 and bottom there is an interpreter error
> message then loading the file and display not updated. Looking at bottom
> the program is however actually loaded and seems to work OK.
>
>
> Nicklas Karlsson
>
>
> Den 2023-06-26 kl. 01:26, skrev John Dammeyer:
>> I ran the following commands from the MDI without issue from AXIS 2.8.1
> with
>> MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
>> G1 X0 Y0 F20
>> G1 Z0
>> S200 M3
>> G33.1 Z-0.7 K0.05 I3.0
>> M5
>>
>> Interesting watching the spindle RPM indicator, and you can hear it too
of
>> course.
>> Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
>> Reverses and goes up at 600 RPM.
>> Without the I3.0 it goes up at 200 RPM.
>>
>> John
>>
>>
>> -Original Message-
>> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
>> Sent: June 25, 2023 9:07 AM
>> To: emc-users@lists.sourceforge.net
>> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
>>
>> There is positioning move XYZ in real program but happened to remove
>> them then I should make a small test case.
>>
>> Adding positioning move to test case make no difference. Linuxcnc report
>> a file interpretation error and do not update display but program seems
>> to work supposed to.
>>
>> Nicklas Karlsson
>>
>>
>> Den 2023-06-23 kl. 16:20, skrev Chris Radek:
>>> I would add positioning moves (positioning all of XYZ) before the
>>> G33.1 because otherwise the tapped hole can be anywhere - the
>>> program is indeterminate.  This sure might mess up any attempt by
>>> your GUI to check the program or generate a preview.
>>>
>>> Chris
>>>
>>> On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:
>>>> I put the lines below into a file:
>>>>
>>>> ?? M3 S100
>>>> ?? G33.1 Z-30.474 K0.8 I3.000
>>>> ?? M5
>>>> ?? M2
>>>>
>>>> Then I read into Linuxcnc I get error message:
>>>>
>>>> ?? parse_file interp_error
>>>>
>>>> Removing the line with G33.1 then no error message so it is something
>>>> with this row. Program do however execute as expected with G33.1 line
>>>> even though there is an error message so no real problem. Also execute
>>>> without an error message if run manually in MDI mode. Use origin/master
>>>> last commit Mon May 8 16:10:03 2023 +0200
>>>> 404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar
>> problem?
>>>> Nicklas Karlsson
>>>>
>>>>
>>>>
>>>> _

Re: [Emc-users] G33.1 error then g-code file parsed

[Nicklas SB Karlsson]

Have used the latest origin/master not more than a few weeks old but 
have not checked against older version. Will do this sooner or later, 
hopefully within a week.



Den 2023-06-26 kl. 07:29, skrev John Dammeyer:

OK.
I'll try that for you.
I'm wondering if perhaps spindle acceleration time or some other HAL
parameter gets flagged with an incorrect error message.   I've done power
tapping from .ngc files without issue but I've not used the 'I' parameter.
John

-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 10:09 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Run from MDI then there is no error message for me either. Put the same
rows in a .ngc file adding M2 and bottom there is an interpreter error
message then loading the file and display not updated. Looking at bottom
the program is however actually loaded and seems to work OK.


Nicklas Karlsson


Den 2023-06-26 kl. 01:26, skrev John Dammeyer:

I ran the following commands from the MDI without issue from AXIS 2.8.1

with

MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
M5

Interesting watching the spindle RPM indicator, and you can hear it too of
course.
Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
Reverses and goes up at 600 RPM.
Without the I3.0 it goes up at 200 RPM.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 9:07 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

There is positioning move XYZ in real program but happened to remove
them then I should make a small test case.

Adding positioning move to test case make no difference. Linuxcnc report
a file interpretation error and do not update display but program seems
to work supposed to.

Nicklas Karlsson


Den 2023-06-23 kl. 16:20, skrev Chris Radek:

I would add positioning moves (positioning all of XYZ) before the
G33.1 because otherwise the tapped hole can be anywhere - the
program is indeterminate.  This sure might mess up any attempt by
your GUI to check the program or generate a preview.

Chris

On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:

I put the lines below into a file:

?? M3 S100
?? G33.1 Z-30.474 K0.8 I3.000
?? M5
?? M2

Then I read into Linuxcnc I get error message:

?? parse_file interp_error

Removing the line with G33.1 then no error message so it is something
with this row. Program do however execute as expected with G33.1 line
even though there is an error message so no real problem. Also execute
without an error message if run manually in MDI mode. Use origin/master
last commit Mon May 8 16:10:03 2023 +0200
404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar

problem?

Nicklas Karlsson



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

OK.
I'll try that for you.  
I'm wondering if perhaps spindle acceleration time or some other HAL
parameter gets flagged with an incorrect error message.   I've done power
tapping from .ngc files without issue but I've not used the 'I' parameter.
John

-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu] 
Sent: June 25, 2023 10:09 PM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

Run from MDI then there is no error message for me either. Put the same 
rows in a .ngc file adding M2 and bottom there is an interpreter error 
message then loading the file and display not updated. Looking at bottom 
the program is however actually loaded and seems to work OK.


Nicklas Karlsson


Den 2023-06-26 kl. 01:26, skrev John Dammeyer:
> I ran the following commands from the MDI without issue from AXIS 2.8.1
with
> MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
> G1 X0 Y0 F20
> G1 Z0
> S200 M3
> G33.1 Z-0.7 K0.05 I3.0
> M5
>
> Interesting watching the spindle RPM indicator, and you can hear it too of
> course.
> Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
> Reverses and goes up at 600 RPM.
> Without the I3.0 it goes up at 200 RPM.
>
> John
>
>
> -Original Message-
> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
> Sent: June 25, 2023 9:07 AM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] G33.1 error then g-code file parsed
>
> There is positioning move XYZ in real program but happened to remove
> them then I should make a small test case.
>
> Adding positioning move to test case make no difference. Linuxcnc report
> a file interpretation error and do not update display but program seems
> to work supposed to.
>
> Nicklas Karlsson
>
>
> Den 2023-06-23 kl. 16:20, skrev Chris Radek:
>> I would add positioning moves (positioning all of XYZ) before the
>> G33.1 because otherwise the tapped hole can be anywhere - the
>> program is indeterminate.  This sure might mess up any attempt by
>> your GUI to check the program or generate a preview.
>>
>> Chris
>>
>> On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:
>>> I put the lines below into a file:
>>>
>>>?? M3 S100
>>>?? G33.1 Z-30.474 K0.8 I3.000
>>>?? M5
>>>?? M2
>>>
>>> Then I read into Linuxcnc I get error message:
>>>
>>>?? parse_file interp_error
>>>
>>> Removing the line with G33.1 then no error message so it is something
>>> with this row. Program do however execute as expected with G33.1 line
>>> even though there is an error message so no real problem. Also execute
>>> without an error message if run manually in MDI mode. Use origin/master
>>> last commit Mon May 8 16:10:03 2023 +0200
>>> 404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar
> problem?
>>>
>>> Nicklas Karlsson
>>>
>>>
>>>
>>> ___
>>> Emc-users mailing list
>>> Emc-users@lists.sourceforge.net
>>> https://lists.sourceforge.net/lists/listinfo/emc-users
>>>
>> ___
>> Emc-users mailing list
>> Emc-users@lists.sourceforge.net
>> https://lists.sourceforge.net/lists/listinfo/emc-users
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[Nicklas SB Karlsson]

Run from MDI then there is no error message for me either. Put the same 
rows in a .ngc file adding M2 and bottom there is an interpreter error 
message then loading the file and display not updated. Looking at bottom 
the program is however actually loaded and seems to work OK.



Nicklas Karlsson


Den 2023-06-26 kl. 01:26, skrev John Dammeyer:

I ran the following commands from the MDI without issue from AXIS 2.8.1 with
MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
M5

Interesting watching the spindle RPM indicator, and you can hear it too of
course.
Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
Reverses and goes up at 600 RPM.
Without the I3.0 it goes up at 200 RPM.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 25, 2023 9:07 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

There is positioning move XYZ in real program but happened to remove
them then I should make a small test case.

Adding positioning move to test case make no difference. Linuxcnc report
a file interpretation error and do not update display but program seems
to work supposed to.

Nicklas Karlsson


Den 2023-06-23 kl. 16:20, skrev Chris Radek:

I would add positioning moves (positioning all of XYZ) before the
G33.1 because otherwise the tapped hole can be anywhere - the
program is indeterminate.  This sure might mess up any attempt by
your GUI to check the program or generate a preview.

Chris

On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:

I put the lines below into a file:

   ?? M3 S100
   ?? G33.1 Z-30.474 K0.8 I3.000
   ?? M5
   ?? M2

Then I read into Linuxcnc I get error message:

   ?? parse_file interp_error

Removing the line with G33.1 then no error message so it is something
with this row. Program do however execute as expected with G33.1 line
even though there is an error message so no real problem. Also execute
without an error message if run manually in MDI mode. Use origin/master
last commit Mon May 8 16:10:03 2023 +0200
404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar

problem?


Nicklas Karlsson



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

I ran the following commands from the MDI without issue from AXIS 2.8.1 with
MESA 7i92H controlling an AC Servo motor (step/dir) for the spindle.
G1 X0 Y0 F20
G1 Z0
S200 M3
G33.1 Z-0.7 K0.05 I3.0
M5

Interesting watching the spindle RPM indicator, and you can hear it too of
course.
Goes down to tap the 0.05" pitch (20TPI thread) at 200RPM
Reverses and goes up at 600 RPM.
Without the I3.0 it goes up at 200 RPM.

John


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu] 
Sent: June 25, 2023 9:07 AM
To: emc-users@lists.sourceforge.net
Subject: Re: [Emc-users] G33.1 error then g-code file parsed

There is positioning move XYZ in real program but happened to remove 
them then I should make a small test case.

Adding positioning move to test case make no difference. Linuxcnc report 
a file interpretation error and do not update display but program seems 
to work supposed to.

Nicklas Karlsson


Den 2023-06-23 kl. 16:20, skrev Chris Radek:
> I would add positioning moves (positioning all of XYZ) before the
> G33.1 because otherwise the tapped hole can be anywhere - the
> program is indeterminate.  This sure might mess up any attempt by
> your GUI to check the program or generate a preview.
>
> Chris
>
> On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:
>> I put the lines below into a file:
>>
>>   ?? M3 S100
>>   ?? G33.1 Z-30.474 K0.8 I3.000
>>   ?? M5
>>   ?? M2
>>
>> Then I read into Linuxcnc I get error message:
>>
>>   ?? parse_file interp_error
>>
>> Removing the line with G33.1 then no error message so it is something
>> with this row. Program do however execute as expected with G33.1 line
>> even though there is an error message so no real problem. Also execute
>> without an error message if run manually in MDI mode. Use origin/master
>> last commit Mon May 8 16:10:03 2023 +0200
>> 404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar
problem?
>>
>>
>> Nicklas Karlsson
>>
>>
>>
>> ___
>> Emc-users mailing list
>> Emc-users@lists.sourceforge.net
>> https://lists.sourceforge.net/lists/listinfo/emc-users
>>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[Nicklas SB Karlsson]

There is positioning move XYZ in real program but happened to remove 
them then I should make a small test case.


Adding positioning move to test case make no difference. Linuxcnc report 
a file interpretation error and do not update display but program seems 
to work supposed to.


Nicklas Karlsson


Den 2023-06-23 kl. 16:20, skrev Chris Radek:

I would add positioning moves (positioning all of XYZ) before the
G33.1 because otherwise the tapped hole can be anywhere - the
program is indeterminate.  This sure might mess up any attempt by
your GUI to check the program or generate a preview.

Chris

On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:

I put the lines below into a file:

  ?? M3 S100
  ?? G33.1 Z-30.474 K0.8 I3.000
  ?? M5
  ?? M2

Then I read into Linuxcnc I get error message:

  ?? parse_file interp_error

Removing the line with G33.1 then no error message so it is something
with this row. Program do however execute as expected with G33.1 line
even though there is an error message so no real problem. Also execute
without an error message if run manually in MDI mode. Use origin/master
last commit Mon May 8 16:10:03 2023 +0200
404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar problem?


Nicklas Karlsson



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[Chris Radek]

I would add positioning moves (positioning all of XYZ) before the
G33.1 because otherwise the tapped hole can be anywhere - the
program is indeterminate.  This sure might mess up any attempt by
your GUI to check the program or generate a preview.

Chris

On Wed, Jun 14, 2023 at 09:14:20PM +0200, Nicklas SB Karlsson wrote:
> I put the lines below into a file:
> 
>  ?? M3 S100
>  ?? G33.1 Z-30.474 K0.8 I3.000
>  ?? M5
>  ?? M2
> 
> Then I read into Linuxcnc I get error message:
> 
>  ?? parse_file interp_error
> 
> Removing the line with G33.1 then no error message so it is something 
> with this row. Program do however execute as expected with G33.1 line 
> even though there is an error message so no real problem. Also execute 
> without an error message if run manually in MDI mode. Use origin/master 
> last commit Mon May 8 16:10:03 2023 +0200 
> 404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar problem?
> 
> 
> Nicklas Karlsson
> 
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
> 


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[Nicklas SB Karlsson]

Without I3.00 make no difference.

Then there is G33.1 in the file error message "parse_file interp_error" 
is shown and display is not updated.


Looking more closely at the bottom G-code is however actually loaded and 
seems to execute correct including the G33.1 rigid tapping cycle even 
though there is error message and display not updated.



Nicklas Karlsson



Den 2023-06-14 kl. 21:36, skrev Sam Sokolik:

Could you try it without I3.000?

On Wed, Jun 14, 2023 at 2:31 PM John Dammeyer 
wrote:


Does your spindle have an encoder and the spindle at speed?


https://forum.linuxcnc.org/38-general-linuxcnc-questions/43124-g33-1-rigid-tapping


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
Sent: June 14, 2023 12:14 PM
To: emc-users@lists.sourceforge.net
Subject: [Emc-users] G33.1 error then g-code file parsed

I put the lines below into a file:

  � M3 S100
  � G33.1 Z-30.474 K0.8 I3.000
  � M5
  � M2

Then I read into Linuxcnc I get error message:

  � parse_file interp_error

Removing the line with G33.1 then no error message so it is something
with this row. Program do however execute as expected with G33.1 line
even though there is an error message so no real problem. Also execute
without an error message if run manually in MDI mode. Use origin/master
last commit Mon May 8 16:10:03 2023 +0200
404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar problem?


Nicklas Karlsson



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[Sam Sokolik]

Could you try it without I3.000?

On Wed, Jun 14, 2023 at 2:31 PM John Dammeyer 
wrote:

> Does your spindle have an encoder and the spindle at speed?
>
>
> https://forum.linuxcnc.org/38-general-linuxcnc-questions/43124-g33-1-rigid-tapping
>
>
> -Original Message-
> From: Nicklas SB Karlsson [mailto:n...@nksb.eu]
> Sent: June 14, 2023 12:14 PM
> To: emc-users@lists.sourceforge.net
> Subject: [Emc-users] G33.1 error then g-code file parsed
>
> I put the lines below into a file:
>
>  � M3 S100
>  � G33.1 Z-30.474 K0.8 I3.000
>  � M5
>  � M2
>
> Then I read into Linuxcnc I get error message:
>
>  � parse_file interp_error
>
> Removing the line with G33.1 then no error message so it is something
> with this row. Program do however execute as expected with G33.1 line
> even though there is an error message so no real problem. Also execute
> without an error message if run manually in MDI mode. Use origin/master
> last commit Mon May 8 16:10:03 2023 +0200
> 404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar problem?
>
>
> Nicklas Karlsson
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] G33.1 error then g-code file parsed

[John Dammeyer]

Does your spindle have an encoder and the spindle at speed?

https://forum.linuxcnc.org/38-general-linuxcnc-questions/43124-g33-1-rigid-tapping


-Original Message-
From: Nicklas SB Karlsson [mailto:n...@nksb.eu] 
Sent: June 14, 2023 12:14 PM
To: emc-users@lists.sourceforge.net
Subject: [Emc-users] G33.1 error then g-code file parsed

I put the lines below into a file:

 � M3 S100
 � G33.1 Z-30.474 K0.8 I3.000
 � M5
 � M2

Then I read into Linuxcnc I get error message:

 � parse_file interp_error

Removing the line with G33.1 then no error message so it is something 
with this row. Program do however execute as expected with G33.1 line 
even though there is an error message so no real problem. Also execute 
without an error message if run manually in MDI mode. Use origin/master 
last commit Mon May 8 16:10:03 2023 +0200 
404aa407f136ce91a3e6bf911c7bda54011a74e9 Anybody else had similar problem?


Nicklas Karlsson



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users