Drilling cycle problem

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

Drilling cycle problem

Postby Derek » Sat Sep 24, 2016 3:29 pm

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
Derek
 
Posts: 207
Joined: Mon Sep 05, 2016 9:57 am

Re: Drilling cycle problem

Postby cncdrive » Sat Sep 24, 2016 3:57 pm

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.
cncdrive
Site Admin
 
Posts: 1480
Joined: Tue Aug 12, 2014 11:17 pm

Re: Drilling cycle problem

Postby Derek » Sat Sep 24, 2016 4:24 pm

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
Derek
 
Posts: 207
Joined: Mon Sep 05, 2016 9:57 am

Re: Drilling cycle problem

Postby cncdrive » Sat Sep 24, 2016 4:58 pm

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.
cncdrive
Site Admin
 
Posts: 1480
Joined: Tue Aug 12, 2014 11:17 pm

Re: Drilling cycle problem

Postby svse » Sun Apr 23, 2017 11:02 am

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
svse
 
Posts: 11
Joined: Fri Jan 20, 2017 9:33 am

Re: Drilling cycle problem

Postby cncdrive » Mon Apr 24, 2017 12:45 pm

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
Site Admin
 
Posts: 1480
Joined: Tue Aug 12, 2014 11:17 pm

Re: Drilling cycle problem

Postby Vmax549 » Mon Apr 24, 2017 6:01 pm

It SHOULD rapid down to teh R level at teh start of the cycle.

(;-) TP
Vmax549
 
Posts: 599
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: Drilling cycle problem

Postby cncdrive » Tue May 02, 2017 12:43 pm

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. :)
cncdrive
Site Admin
 
Posts: 1480
Joined: Tue Aug 12, 2014 11:17 pm

Re: Drilling cycle problem

Postby svse » Tue May 02, 2017 2:22 pm

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

Regards, Sven
svse
 
Posts: 11
Joined: Fri Jan 20, 2017 9:33 am

Re: Drilling cycle problem

Postby Vmax549 » Tue May 02, 2017 3:12 pm

hi Balazs, IF you read up on the LAST NSTS release it shows in a round about way that it should rapid to teh R level first then start teh downfeed. Each line if teh R is changed it should rapid to teh new R level before it starts that line of motion. That way each Hole could have a different R level for clearances.

Just a thought, (;-) TP
Vmax549
 
Posts: 599
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Next

Return to Report a bug

Who is online

Users browsing this forum: No registered users and 2 guests