Drilling cycle problem

[Derek]

Drilling cycle is ignoring the R number in the code on initial approach.

When I run this code in 1.1021 it rapids down to .1 then drills from there. When I run it in 1.2021 it starts feeding from the Z clearance height. In this case 2.0" It happens in G83 and I'm pretty sure it's happening in tapping as well.

Code: Select all

N9 G00 Z2.0000
N10 X0.0000 Y0.0000
N11 G81 X0.0000 Y0.0000 Z-0.5 R0.1 F30.
N12G80
N13 G00 Z2.0000

[cncdrive]

Isn't the issue is that G98 is active?
I did not look it up yet, but I think the G98/G99 was not implemented yet in version 1.1021, but in the version 1.2xxx it is.
And G98/G99 controls the return level of the canned cycles.

[Derek]

Yep that was it. I never even knew that existed. Do you know if that is persistent or do I need to do G99 every time I start up UCCNC.

Thanks
Derek

[cncdrive]

Hi Derek,

It's not persistant, just modal, but on startup always the G98 is active,
so if you want to use G99 then you have to execute the G99 code first.
Maybe adding it to the M99998 macro would be a good idea if you mostly working in G99,
or adding it to your CAM post processor to let the CAM software add it to your codes.

[svse]

Hi,

i have the same problem, but G99 is not working for me.
With G98 at the first, the machine moves to safe z after each hole. That is exactly what i need. (With G99 it moves only to R after drilling.)
But at each hole the machine beginns the drilling from safe-z, that needs alot more time. I had used linuxcnc before and there he first makes a rapid movement down to R and then starts drilling.

The GCode for Linuxcnc and UCCNC is the same. What is the normal behaviour of G83 with G98?

Is someone using Mach3? It is the same behaviour as in UCCNC or as in LinuxCNC?
Is there a way to change the G83 in UCCNC?

Thanks alot,

Sven

[cncdrive]

Hi,

Yes, somebody else recently reported the same and it really does not rapids down to R when in G98 mode.
I'm still not 100% sure if it has to rapid down or not, I mean the standards book only mentions how the pullout has to happen, but not how the start.
So, I will try to read after what is the correct implementation is and if it has to rapid down then we will change it.

[cncdrive]

Thank you Terry.
I read after this at a few places, but could not locate any documentation which would describe the initial movement with G98 and defined R parameters, all documents only describes the pullout and the R with G99.
Anyways, I've discussed this question also on the Hungarian hobbycnc forum and the guys there also said that it should rapid to R in G98, so I have now enough input to confidentally change the code.

[svse]

Thumbs up! That are great news, thanks for the support.

Regards, Sven

[Dan911]

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

[cncdrive]

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.