Group: DynoMotion	Message: 14075	From: mmurray70@hotmail.com	Date: 11/15/2016
Subject: Problem with G83 peck drill Cycle

Hi,

Im having a slight problem with G83 drilling cycle. Im using G98 (return to initial plane), but when pecking the tool returns to the initial plane (Z2.0) every peck. It should go to the R plane (0.1) when pecking, and then back up to Z2.0 when moving to the next hole to clear clamps. Here is an example program:

N140 G00 G90 G54 X0. Y0. S2000 M03

N150 G43 G94 H1 Z2.

N160 G98 G83 Z-.5 R.1 Q.1 F15.

N170 X1.

N180 G80

N190 M05

This is alot of extra rapids and wasted time going to initial plane every peck. Is there any way around this? Our Fanuc and Mazak mills at work would run this code as i describe above, going to 0.1 each peck and 2.0 when moving to the next hole.

Ive tried G99 and this goes to to 0.1 for each peck, but does not go to clearance plane between holes and thats asking for trouble for my type of work lol. Is there a way to change this? Thanks.

Group: DynoMotion	Message: 14078	From: Tom Kerekes	Date: 11/16/2016
Subject: Re: Problem with G83 peck drill Cycle

Hi,

I can't find a good reference on the height Z should retract at the end of the G83 cycle.

We could change that but I'm not sure it wouldn't cause problems for existing GCode files.

I suppose it would just slow down some Jobs that don't need to move to the Clamp clearance height.

Of course you could add in an extra Z move in your post processor as a workaround.

Does anyone have an opinion?

Regards
TK

On 11/15/2016 6:26 PM, mmurray70@... [DynoMotion] wrote:

Hi,

Im having a slight problem with G83 drilling cycle. Im using G98 (return to initial plane), but when pecking the tool returns to the initial plane (Z2.0) every peck. It should go to the R plane (0.1) when pecking, and then back up to Z2.0 when moving to the next hole to clear clamps. Here is an example program:

N140 G00 G90 G54 X0. Y0. S2000 M03

N150 G43 G94 H1 Z2.

N160 G98 G83 Z-.5 R.1 Q.1 F15.

N170 X1.

N180 G80

N190 M05

This is alot of extra rapids and wasted time going to initial plane every peck. Is there any way around this? Our Fanuc and Mazak mills at work would run this code as i describe above, going to 0.1 each peck and 2.0 when moving to the next hole.

Ive tried G99 and this goes to to 0.1 for each peck, but does not go to clearance plane between holes and thats asking for trouble for my type of work lol. Is there a way to change this? Thanks.

Group: DynoMotion	Message: 14079	From: engnerdan	Date: 11/16/2016
Subject: Re: Problem with G83 peck drill Cycle

I just ran a simulation with this code, as it was post processed from HSM express, and it shows it coming to the clearance plane until drilling is done and then going to the initial plane so that is how I would have expected it to work. But my initial plane is only 0.4" different than the clearance plane so I may have never noticed it not doing it on my machine.

But while on the topic of peck drilling cycles I have got the KFLOP to mess up a bit with this exact code. I was using feedhold many times during the first hole location (to clear chips) and at one point it is like the KFLOP forgot where it was in the cycle and restarted from the beginning. I think I might even have video of it doing this somewhere.

-Dan

Group: DynoMotion	Message: 14081	From: Moray Cuthill	Date: 11/16/2016
Subject: Re: Problem with G83 peck drill Cycle

I've just searched, and the Hass G-code guide shows it as going back to the initial plane, with the only exception being on the first peck where it rapids to the R - https://diy.haascnc.com/g-codes-mills

Unless you've changed a setting in the controller.

The other links I've checked (Tormach, cnccookbook) are pretty ambiguous in their descriptions.

I've only ever used G83 on my lathe, where clearance between holes isn't a problem.

However, was the problem with the G83 and G18/lack of Y ever solved?

I've copied and pasted my last post on the problem from April below, although ignore my comment about G73 as it seems to vary between controllers.

Hi Tom,

I can add G43s easily enough.

I've just been and done some testing with G83s and have found the issue.
If you declare a G18 (Select X-Z plane), then the G83 rapids to depth, but not only that, it doesn't retract before the next move. I've attached a screen grab showing the moves. If you then run a code snippet such as the following (after the code shown in that screen grab)-
G90 G21
G00 G53 X0 Z0
(T101M6)
M6 T114
G43H114
G0 X0 Z2
(G1 Z1)
G83 X0 Y0 Z-32.0 R2 Q3 F100
G0 G53 X0 Z0
M30
the first time it runs, it also rapids to depth, then on subsequent re-runs, works as intended, until you then add a G18. However testing with only that snippet, the issue disappears as soon as the G18 is removed.
The G18s in my files all came from Mach3 files, as I've just been editing my old Mach3 files by changing the M6/tool change blocks to suit KMotionCNC. Now I know the problem, I'll just remove the G18s.

I'm guessing there's an issue with the G18 then having/needing Y declared in the G83. I won't go as far as saying it's a bug, as technically a G83 is a milling cycle, with the lathe equivalent being a G73, but it's something that should perhaps be highlighted somehow?

Thanks,
Moray

On Wed, Nov 16, 2016 at 8:16 PM, engnerdan@... [DynoMotion] <DynoMotion@yahoogroups.com> wrote:

I just ran a simulation with this code, as it was post processed from HSM express, and it shows it coming to the clearance plane until drilling is done and then going to the initial plane so that is how I would have expected it to work. But my initial plane is only 0.4" different than the clearance plane so I may have never noticed it not doing it on my machine.

But while on the topic of peck drilling cycles I have got the KFLOP to mess up a bit with this exact code. I was using feedhold many times during the first hole location (to clear chips) and at one point it is like the KFLOP forgot where it was in the cycle and restarted from the beginning. I think I might even have video of it doing this somewhere.

-Dan

Group: DynoMotion	Message: 14083	From: mmurray70@hotmail.com	Date: 11/16/2016
Subject: Re: Problem with G83 peck drill Cycle

It looks like Hass has a parameter 52 that adds extra distance to each peck retract above the R plane to clear chips. I dont think we need to get that complicated.

The sequence when using G98, should be: Rapid to X/Y of first hole, Rapid to R plane, peck drill hole returning to R plane each time to clear chips, rapid to Initial/clearance plane when done drilling a hole, move to next X/Y position and repeat until done.

At the end of a cycle and all holes are drilled it should return to initial/clearance plane. I just verified this in cam. If i post out a drilling operation and then a milling operation right after with the same tool, and same clearance plane of 2.0, it does not output a Z move to clearance plane for the milling operation. It expects the drilling operation to have returned the tool to Z2.0. If i post out the two operations with different clearance planes there is a Z move to the new clearance plane.

Group: DynoMotion	Message: 14084	From: Tom Kerekes	Date: 11/16/2016
Subject: Re: Problem with G83 peck drill Cycle

It sounds like it is reasonable to make that change.

Here is a patch for Version 4.34e that should have that behavior.

http://dynomotion.com/Software/Patch/AddFanucStyleCompEntryMove_V434e/GCodeInterpreter.dll

Copy it to the C:\KMotion434e\KMotion\Release directory.

Please let us know if there are any issues.

Regards

On 11/16/2016 5:52 PM, mmurray70@... [DynoMotion] wrote:

It looks like Hass has a parameter 52 that adds extra distance to each peck retract above the R plane to clear chips. I dont think we need to get that complicated.

The sequence when using G98, should be: Rapid to X/Y of first hole, Rapid to R plane, peck drill hole returning to R plane each time to clear chips, rapid to Initial/clearance plane when done drilling a hole, move to next X/Y position and repeat until done.

At the end of a cycle and all holes are drilled it should return to initial/clearance plane. I just verified this in cam. If i post out a drilling operation and then a milling operation right after with the same tool, and same clearance plane of 2.0, it does not output a Z move to clearance plane for the milling operation. It expects the drilling operation to have returned the tool to Z2.0. If i post out the two operations with different clearance planes there is a Z move to the new clearance plane.

Group: DynoMotion	Message: 14086	From: mmurray70@hotmail.com	Date: 11/16/2016
Subject: Re: Problem with G83 peck drill Cycle

Thanks Tom, I will try this on friday. Im still using 4.33, is there anything to watch out for when changing to 4.34? I was hesitant to install it since it wasnt the lastest version on the Dynomotion website.

Group: DynoMotion	Message: 14090	From: Tom Kerekes	Date: 11/17/2016
Subject: Re: Problem with G83 peck drill Cycle

Oops sorry, this file changed also:

http://dynomotion.com/Software/Patch/AddFanucStyleCompEntryMove_V434e/KMotionCNC.exe

I assume you meant to say V4.34e. I'm not aware of any problems in V4.34e.

Regards

On 11/16/2016 7:37 PM, mmurray70@... [DynoMotion] wrote:

Thanks Tom, I will try this on friday. Im still using 4.33, is there anything to watch out for when changing to 4.34? I was hesitant to install it since it wasnt the lastest version on the Dynomotion website.

Group: DynoMotion	Message: 14103	From: mmurray70@hotmail.com	Date: 11/18/2016
Subject: Re: Problem with G83 peck drill Cycle

Hi Tom,

Sorry but I wasn't able to test the changes you made today. I tried upgrading to 4.34e but it dont seem like its going to work on my old XP laptop. In search of a windows 7 machine now. I will let you know how it works when i find a newer computer. Thanks.

Mark

Group: DynoMotion	Message: 14116	From: mmurray70@hotmail.com	Date: 11/19/2016
Subject: Re: Problem with G83 peck drill Cycle

Hi,

I got a Windows 7 computer today and got everything up and running with 4.34e and i replaced both of those files, but it does the same rapid to initial/clearance plane each peck the same as before. No sure what went wrong. I double checked both the files are replaced with the new ones dated from a couple days ago. Any other suggestions? Thanks.

Mark

Group: DynoMotion	Message: 14118	From: TKSOFT	Date: 11/19/2016
Subject: Re: Problem with G83 peck drill Cycle

Hi Mark,

Did you try with G98 or G99?

Regards
TK

On 2016-11-19 14:30, mmurray70@... [DynoMotion] wrote:
> Hi,
>
> I got a Windows 7 computer today and got everything up and running
> with 4.34e and i replaced both of those files, but it does the same
> rapid to initial/clearance plane each peck the same as before. No sure
> what went wrong. I double checked both the files are replaced with the
> new ones dated from a couple days ago. Any other suggestions? Thanks.
>
> Mark
>

Group: DynoMotion	Message: 14119	From: mmurray70@hotmail.com	Date: 11/19/2016
Subject: Re: Problem with G83 peck drill Cycle

Hi Tom,

I tried with G98 and there is no change, I just tried again with G99 and it is changed. But this is not exactly right. G98 is the code used for this motion. G99 should just use the R plane for everything as far as i know. So current G99 motion, should be G98. And i believe G99 should just go to R plane each time for pecks and moving between holes, although honestly i dont ever use G99.

One more slight issue too. Using G99 with this patch (which should be G98) it is going to the R plane when pecking which is great, and going to initial plane between holes which is also great. But after going to the inital plane when finished the first hole, it should move X/Y to next hole and then move Z to R plane to start next hole. Its actually moving X/Y/Z all in one move to the next hole, moving on an angle. Hopefully these are easy fixes. Thanks again!

Mark

Group: DynoMotion	Message: 14125	From: Tom Kerekes	Date: 11/19/2016
Subject: Re: Problem with G83 peck drill Cycle

Hi Mark,

I think I understand now. Here is a Video demo of the latest result:

https://youtu.be/rnzRSWcLMJ8

Please download the files again and see if it now behaves as you expect

Regards

On 11/19/2016 6:02 PM, mmurray70@... [DynoMotion] wrote:

Hi Tom,

I tried with G98 and there is no change, I just tried again with G99 and it is changed. But this is not exactly right. G98 is the code used for this motion. G99 should just use the R plane for everything as far as i know. So current G99 motion, should be G98. And i believe G99 should just go to R plane each time for pecks and moving between holes, although honestly i dont ever use G99.

One more slight issue too. Using G99 with this patch (which should be G98) it is going to the R plane when pecking which is great, and going to initial plane between holes which is also great. But after going to the inital plane when finished the first hole, it should move X/Y to next hole and then move Z to R plane to start next hole. Its actually moving X/Y/Z all in one move to the next hole, moving on an angle. Hopefully these are easy fixes. Thanks again!

Mark

Group: DynoMotion	Message: 14127	From: mmurray70@hotmail.com	Date: 11/20/2016
Subject: Re: Problem with G83 peck drill Cycle

Hi Tom,

I just tried it with the new files and G83 with G98 is now working perfectly. Didnt test G99 but looks to be right in your video. Thanks again for the great support!

Mark