G84 does not seem to work for me.

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

G84 does not seem to work for me.

Postby Derek » Tue Jun 20, 2017 11:39 am

This works:
Code: Select all
S150
M03
N9 G00 Z0.3500
N10 X0.0000 Y0.0000
N11  X0.0000 Y0.0000
N12G33.1 Z-0.5 K.0461
N13M03
N15 G00 Z0.3500
N16 M05
N17 M30


This does not:
Code: Select all
S150
M03
N9 G00 Z0.3500
N10 X0.0000 Y0.0000
N11  X0.0000 Y0.0000
N12G84 Z-0.5 K.0461
N14G80
N15 G00 Z0.3500
N16 M05
N17 M30


The spindle turns on and it positions but just sits there like it's waiting for the index signal.
Thanks
Derek
Derek
 
Posts: 196
Joined: Mon Sep 05, 2016 9:57 am

Re: G84 does not seem to work for me.

Postby dezsoe » Tue Jun 20, 2017 12:58 pm

Set also P parameter to 1. If P is 0 (or not given) it means left handed tapping (G33.2).
dezsoe
 
Posts: 216
Joined: Sun Mar 12, 2017 4:41 pm
Location: Csörög, Hungary

Re: G84 does not seem to work for me.

Postby dezsoe » Tue Jun 20, 2017 1:17 pm

Also, you can shorten you code, because G84 has X and Y coordinates, so you can use:

Code: Select all
S150
M03
G00 Z0.3500
G84 X0.0000 Y0.0000 Z-0.5 K.0461
G80
G00 Z0.3500
M05
M30
dezsoe
 
Posts: 216
Joined: Sun Mar 12, 2017 4:41 pm
Location: Csörög, Hungary

Re: G84 does not seem to work for me.

Postby Derek » Tue Jun 20, 2017 1:38 pm

That fixed it.

Is this a known G84 or one that you created for UCCNC. I tried a few different post processors and couldn't come up with one that produced a G84 that uses K as the pitch. I can edit my post for UCCNC but it would be easier if it was based on a known convention.

Also wouldn't it make more sense since the overwhelming majority of threads are right hand to have no P default to right hand tap. Seems counter intuitive.

Thanks
Derek
Derek
 
Posts: 196
Joined: Mon Sep 05, 2016 9:57 am

Re: G84 does not seem to work for me.

Postby cncdrive » Tue Jun 20, 2017 2:06 pm

Hi Derek,

Yes, we've unfortunately made the P parameter in reverse as how we wanted to make it.
I mean we wanted to make it that if P missing then it is right hand tap and when P is defined then left hand, but accidentally made it reversed.
Will reverse this.
Also P parameter for direction now does not seems to be the best idea, because it means a dwell e.g. on the Fanucs, so I will change the P to H parameter and will reverse the direction.

On many controls there is no K parameter, because the feedrate and spindle speed sets the pitch, but I think it is better to have a definable pitch parameter otherwise the user always have to figure the pitch...
cncdrive
Site Admin
 
Posts: 1365
Joined: Tue Aug 12, 2014 11:17 pm

Re: G84 does not seem to work for me.

Postby dezsoe » Tue Jun 20, 2017 2:11 pm

G84 exists in some g-code dialects, but with various meaning of parameters. In UCCNC G33.x uses also K parameter, so it came here too. :)
dezsoe
 
Posts: 216
Joined: Sun Mar 12, 2017 4:41 pm
Location: Csörög, Hungary

Re: G84 does not seem to work for me.

Postby Vmax549 » Thu Jun 22, 2017 4:34 pm

Normally with G84/74 teh pitch is set in G95 mode Unit per rev as that gives you the pitch directly. OR it could be done from RPM/Feedrate.

i have never seen a seperate parameter for Feed with G84 (K).

Just a thought. (;-) TP
Vmax549
 
Posts: 515
Joined: Sun Nov 22, 2015 3:25 am
Location: USA


Return to Report a bug

Who is online

Users browsing this forum: No registered users and 2 guests

cron