Drilling cycle problem

If you think you've found a bug post it here.

Re: Drilling cycle problem

Postby Dan911 » Mon Nov 13, 2017 10:17 pm

Ok...Happy to see/find I'm not the only1 that found this to be a problem. It seems that G98 was partially fixed, the first hole of cycle works correctly but every hole in that cycle after starts at initial plane drill or peck. Only tested g73, G81,G82,G83.

Dan
Dan911
 
Posts: 354
Joined: Mon Oct 31, 2016 1:22 am
Location: USA

Re: Drilling cycle problem

Postby cncdrive » Tue Nov 14, 2017 12:09 am

The issue described in this thread was already fixed in version 1.2038.
I quickly tested G83 with G98 with 1.2047 and it works fine at me.
I did not see your code but I guess you did not define the R plane on the second and etc. codes and the R value is not modal and if not defined then the only defined retract to value is the inital plane, so the software will start the peck drilling and the retract to the initial plane anyways.
If not this is the case then please post your code to let me test it, because what codes I tested with works fine.

The G83 code definition from the manual:

Peck drilling cycle with full backoff distance: G83
To execute a pecl drilling cycle with a full back off distance, program G83 X... Y... Z... Q... R... ,
where the X, Y and the R parameters are optional and the Q parameter is modal.
The G83 code is very similar to the G73, the only difference is that at each peck increments the
controller returns to the R plane if the R plane was programmed or to the initial plane if the R
parameter was not set. The purpose of this command is the same as of the G73, but because of the
full retract at each increments can break spiral chips better.
cncdrive
Site Admin
 
Posts: 1940
Joined: Tue Aug 12, 2014 11:17 pm

Re: Drilling cycle problem

Postby Dan911 » Tue Nov 14, 2017 12:47 am

[codeO0000 (PECKTEST)

G20 G40 G80 G17

N1 (DRILL - 1-4 IN DIA)
G00 G90 G43 X0.7 Y11.3
T1 M6
Z1.
S8000 M3
M9
G98 G83 Z-0.5 R0.5 Q.125 F5 M9
X6. Y11.3
X11.3 Y11.3
X11.3 Y6.
X11.3 Y0.7
X6. Y0.7
X0.7 Y0.7
X0.7 Y6.
G80
G90 Z1 M6
M30][/code]

If the R value is not modal in UCCNC than that explains where the problem is. From what I understood and experienced with canned cycles is the only time a new R value is needed in a running canned cycle is if it needed to be changed. I know for sure this is how it works in Mach3 and Tormach, any other info I found online explains it this way also.

Dan
Dan911
 
Posts: 354
Joined: Mon Oct 31, 2016 1:22 am
Location: USA

Re: Drilling cycle problem

Postby cncdrive » Tue Nov 14, 2017 1:03 am

I could not locate any documentations (Mach3 or LinuxCNC and NIST) which states that R has to be modal.
I also tried to test Mach3 now with some simple G83 codes to see at which point does it rapids to and retracts to, but it seems there is somekind of bug (maybe in the version I have installed) that it always runs the wrong feedrate, not the programmed one, but it runs with the default 6 feedrate and it's late night at me so I don't have time now to figure it out why is this or to reinstall mach3 to see if it makes any difference.

So, maybe you have a link to the manuals/online info you mentioned where it is stated the R is modal?
I'm not interested in forum discussions about this, because those can be missleading, but some control manuals where this is stated and written that R should be modal, because yet I'm not aware that it should be modal, I did not see it written anywhere so far. I did not use canned cycles in practise though, so I'm easily convincable, but it would be good to see if it really has to work like that?!
cncdrive
Site Admin
 
Posts: 1940
Joined: Tue Aug 12, 2014 11:17 pm

Re: Drilling cycle problem

Postby Dan911 » Tue Nov 14, 2017 1:47 am

cncdrive wrote:I could not locate any documentations (Mach3 or LinuxCNC and NIST) which states that R has to be modal.
I also tried to test Mach3 now with some simple G83 codes to see at which point does it rapids to and retracts to, but it seems there is somekind of bug (maybe in the version I have installed) that it always runs the wrong feedrate, not the programmed one, but it runs with the default 6 feedrate and it's late night at me so I don't have time now to figure it out why is this or to reinstall mach3 to see if it makes any difference.

So, maybe you have a link to the manuals/online info you mentioned where it is stated the R is modal?
I'm not interested in forum discussions about this, because those can be missleading, but some control manuals where this is stated and written that R should be modal, because yet I'm not aware that it should be modal, I did not see it written anywhere so far. I did not use canned cycles in practise though, so I'm easily convincable, but it would be good to see if it really has to work like that?!



I've done many canned cycles with Mach3 and I can a sure you R in Modal.

Here's a quick link from cnccookbook, scroll down to "Multiple Holes Until G80 Cancels the Cycle"

https://www.cnccookbook.com/g81-g73-g83 ... ned-cycle/


Dan
Dan911
 
Posts: 354
Joined: Mon Oct 31, 2016 1:22 am
Location: USA

Re: Drilling cycle problem

Postby cncdrive » Tue Nov 14, 2017 11:38 am

That document only says (what I see) that the canned cycle is modal which is fine and it is already like that in the UCCNC. G81, 82, 83 etc are in the mode 1, they are modal.
The doc does not say the parameters like R is modal. And what the document says that you can command just coordinates to go to another location to make another canned cycle is true with the UCCNC also, because the G81 etc are modal. Except G73, that is not modal, but as I saw so far it is not part of mode 1 in any other controls, so is why it is also not modal in the UCCNC.
So, this is my problem is that if a parameter like the R has to be modal or not is not documented in any documents I saw so far.

My further thoughts on this is that if R is modal is advantage on one side that R does not have to be always programmed,
but has a disadvantage also that what if you forget about R was already coded and that R was lower than the initial plane and G99 active,
so you code a canned cycle and the tool does not retract back enough and breaks your tool.
So is why I would really like to see how this has to work by the standards, because I see a good and bad side also in both and in the NIST book there is no mention of how this should work and I also could not locate any documentation which would state that R has to be modal or not.
cncdrive
Site Admin
 
Posts: 1940
Joined: Tue Aug 12, 2014 11:17 pm

Re: Drilling cycle problem

Postby Dan911 » Tue Nov 14, 2017 12:18 pm

cncdrive wrote:My further thoughts on this is that if R is modal is advantage on one side that R does not have to be always programmed,
but has a disadvantage also that what if you forget about R was already coded and that R was lower than the initial plane and G99 active,


How I understood it is that the canned cycle values are modal until the G80 cancels it. For whatever it's worth Mach3 works this way.

Thanks,
Dan
Dan911
 
Posts: 354
Joined: Mon Oct 31, 2016 1:22 am
Location: USA

Re: Drilling cycle problem

Postby Dan911 » Tue Nov 14, 2017 12:26 pm

This is from the Tormach site link below.... "G81 to G89 G-Code Canned Cycles Background"

For canned cycles, we will call a number "sticky" if, when the same cycle is used on several lines of code in a row, the number must be used the first time, but is optional on the rest of the lines. Sticky numbers keep their value on the rest of the lines if they are not explicitly programmed to be different. The R number is always sticky.

https://www.tormach.com/g81_g89_backgro ... lYQAvD_BwE
Dan911
 
Posts: 354
Joined: Mon Oct 31, 2016 1:22 am
Location: USA

Re: Drilling cycle problem

Postby dezsoe » Tue Nov 14, 2017 1:25 pm

LOL, copy/paste forever! Open The NIST RS274/NGC Interpreter - Version 3 and search for "sticky". :)
dezsoe
 
Posts: 455
Joined: Sun Mar 12, 2017 4:41 pm
Location: Csörög, Hungary

Re: Drilling cycle problem

Postby Dan911 » Tue Nov 14, 2017 1:59 pm

LOL...What???

Balazs asked me to post links of other controllers and that's what I did. Mach3 and Tormach canned cycles work this way and I suspect mostly others.

I don't know what's right or wrong but can only post what I experienced. I certainly see his reasoning for not making a change YET.

Dan
Dan911
 
Posts: 354
Joined: Mon Oct 31, 2016 1:22 am
Location: USA

PreviousNext

Return to Report a bug

Who is online

Users browsing this forum: No registered users and 3 guests