[RussMachine]

Well Hell!
I was running the old trusty (mostly) 770 today, and my G84 Tapping cycle glitched-out on me.
I thought PATHPILOT was supposed to fix the G84 gremlins?
(G84 X0. Y0. Z-.5 R.2 F50. P1.)

The spindle started, fed down to -.5 … Then stopped.
No spindle reverse, no feeding up... Nothing!

UH OH !!!!!! Luckily I was dry-running the program, without a part in the vise.
I had to reset the program, turn the spindle on manually (To make sure the spindle wasn't dead), and try again.

Nope!! died again...
So, I had to go back to the old MACH3 style, long-hand programming with the feed in, pause, reverse, feed out, etc.
Long-hand program worked like a charm.

Maybe it's something to notify TORMACH about?

[mactec54]

Well Hell!
I was running the old trusty (mostly) 770 today, and my G84 Tapping cycle glitched-out on me.
I thought PATHPILOT was supposed to fix the G84 gremlins?
(G84 X0. Y0. Z-.5 R.2 F50. P1.)

The spindle started, fed down to -.5 … Then stopped.
No spindle reverse, no feeding up... Nothing!

UH OH !!!!!! Luckily I was dry-running the program, without a part in the vise.
I had to reset the program, turn the spindle on manually (To make sure the spindle wasn't dead), and try again.

Nope!! died again...
So, I had to go back to the old MACH3 style, long-hand programming with the feed in, pause, reverse, feed out, etc.
Long-hand program worked like a charm.

Maybe it's something to notify TORMACH about?

It would help if you gave it a retract either G99 or a G98, it does not know what to do without this code

Add a G99 G84 this is normal for a G84 threading cycle, it can be a G99 or a G98 depending on how you want it to retract G99 will look at the R.2 and retract .2 above the part G98 will retract to the set Z height above the part

[rowbare]

I was curious and I checked the documentation. (7.4.6 Tapping Cycle – G84 in the Series 3 manual). It says the same thing as Mactec. The Mach canned cycle probably had a shortcut for it..

bob

[RussMachine]

Really?
Oops, I forgot the G98.
So it won't read the G98 from the previous canned drilling cycle?
hhmmmmm…

I'll have to try it again with the G98 in there, and see if that fixes it.
Thanks!!

[mactec54]

Really?
Oops, I forgot the G98.
So it won't read the G98 from the previous canned drilling cycle?
hhmmmmm…

I'll have to try it again with the G98 in there, and see if that fixes it.
Thanks!!

Without having a G98 or a G99 it does not know what to do it is waiting for a retract command

Every canned cycle is It's own line of code nothing in other canned cycles will carry to another canned cycle it is modal so needs to be canceled

You also have to cancel the canned cycle once completed

A G80 after the canned cycle is complete is normally used as this then cancels the canned cycle which is using a G91 for it's operation G80 cancels the G91 and your next move would be G90 absolute move, if the rest of your program is G91 most likely not then you don't need the G80, you can also just use a G90 G1 or G0 for the next moves after the canned cycle

[metalmayhem]

g98 g99 are both modal commands . It's good practice to always add them to the drilling or tapping cycles but it's not absolutely necessary . A lot of controls like fanuc default to g98 on start up . Pathpilot defaults to g99 on start up

[mactec54]

g98 g99 are both modal commands . It's good practice to always add them to the drilling or tapping cycles but it's not absolutely necessary . A lot of controls like fanuc default to g98 on start up . Pathpilot defaults to g99 on start up

Yes both are modal and have to be canceled either by the control default or the next line after the canned cycle is completed

It is always necessary to have either a G98 or G99 for canned cycles unless the controls being used have it built in as there default, it is always good practice to use it as it takes nothing away from the way it runs and you can have more control of what way it works

If Pathpilot has a default G99 then his tapping cycle should of worked and it did not

[metalmayhem]

If Pathpilot has a default G99 then his tapping cycle should of worked and it did not

g98 or g99 likely aren't the problem . I don't know if you tried it on your pp control but for curiosity sake I tried it without adding a g98 or g99 to the cycle and it worked perfectly fine in pathpilots simulation mode . I'm not aware of anything that cancels these modal commands once they are called , other than one being called and cancelling out the other .

[mactec54]

g98 or g99 likely aren't the problem . I don't know if you tried it on your pp control but for curiosity sake I tried it without adding a g98 or g99 to the cycle and it worked perfectly fine in pathpilots simulation mode . I'm not aware of anything that cancels these modal commands once they are called , other than one being called and cancelling out the other .

G80 cancels any canned cycle or a G90 in the next line after a canned cycle has finished

It would be good to here from RussMachine as to what worked

[metalmayhem]

yes g80 does cancel a drill cycle , it doesn't cancel g98 g99 which are codes of their own

[mountaindew]

I was told for best results to always use long hand code format option in cam software. In Sprutcam's case the difference is considerable. Many options for drilling, tapping, reaming, boring... do not translate into good canned cycle code.

[mactec54]

yes g80 does cancel a drill cycle , it doesn't cancel g98 g99 which are codes of their own

A G80 cancels all canned cycles so if the G98 or G99 are in the canned cycle line like it suppose to be formatted then they will be canceled

[metalmayhem]

when have g98 and g99 become canned cycles ?? They are modal commands and though they are used with canned cycles they are not canned cycles , they are codes of their own and g80 does not cancel these 2 codes out no matter how many times a canned cycle has been canceled . If you don't believe me then try it !! Once these codes are called nothing cancels them other than one canceling out the other , no different that g20 canceling out g21

[mactec54]

when have g98 and g99 become canned cycles ?? They are modal commands and though they are used with canned cycles they are not canned cycles , they are codes of their own and g80 does not cancel these 2 codes out no matter how many times a canned cycle has been canceled . If you don't believe me then try it !! Once these codes are called nothing cancels them other than one canceling out the other , no different that g20 canceling out g21

They have always been part of canned cycles for mills lathes use it in a different way G98 for feedrate per minute G99 feedrate per revolution

Here is a video for you note the Haas control defaults to a G98 so does not need to write it in his drilling cycle program, note the G80 at the end of his program this cancels the Canned cycle but no it is not canceling the G98 because that is a default code in the Haas control, what it is canceling is the incremental part of the canned cycle

Note not all controls have G98 or a G99 as a default so those that don't which is most, have to be added to a canned cycle so that it will function correctly or how you want it to work

https://www.youtube.com/watch?v=YbbZJ7H0NUw

[metalmayhem]

Canned cycles use these reference commands , there is no arguing that and that not my point . As I said to begin with , it is always good practice to always add them to the drill cycles , but it isn't an absolute necessity to call them every drill cycle . These reference commands are modal (key point ) which ever one is called .The drill cycles will work without re-adding a g98-99 as long as the command is already in mode

hass as with many mills start up with a default g98 which is the safer choice to start with . Once g99 is called it will stay modal until g98 is called again . I don't remember and never paid attention to whether or not hass defaults back to g98 after the program has completed , or when the machine has been reset (probably does) , but it's only a parameter setting which would determine that . I know the hass mills I worked on would always default back to g54 under those conditions (I hated that)

right now we are talking about pathpilot control , and mine default to g99 on power up . I can run a drill cycle without adding a g98-99 to the drill cycle and it works perfectly fine . Would I hand code a drill cycle under normal conditions without adding one or the other , no ! I've been trained to do things a certain way and I have never swayed away from it

[mactec54]

Canned cycles use these reference commands , there is no arguing that and that not my point . As I said to begin with , it is always good practice to always add them to the drill cycles , but it isn't an absolute necessity to call them every drill cycle . These reference commands are modal (key point ) which ever one is called .The drill cycles will work without re-adding a g98-99 as long as the command is already in mode

hass as with many mills start up with a default g98 which is the safer choice to start with . Once g99 is called it will stay modal until g98 is called again . I don't remember and never paid attention to whether or not hass defaults back to g98 after the program has completed , or when the machine has been reset (probably does) , but it's only a parameter setting which would determine that . I know the hass mills I worked on would always default back to g54 under those conditions (I hated that)

right now we are talking about pathpilot control , and mine default to g99 on power up . I can run a drill cycle without adding a g98-99 to the drill cycle and it works perfectly fine . Would I hand code a drill cycle under normal conditions without adding one or the other , no ! I've been trained to do things a certain way and I have never swayed away from it

It does not matter if the G98 and G99 are modal or not there only function is for canned cycles when used for milling

With a Haas control the canned cycle is canceled with the default G80 so each line of the canned cycle is canceled after it is complete

What is wrong with the Haas control defaulting to G54 this is the industry standard you call in your program for what ever offset you want to use

If your control defaults to G99 that could be a crash waiting to happen, that was a bad choice by the programmers to do that

[metalmayhem]

What is wrong with the Haas control defaulting to G54 this is the industry standard you call in your program for what ever offset you want to use

there is nothing wrong with the hass control defaulting to g54 on start up . but when using a program that uses g55 and having the machine default back to g54 upon a reset or when reaching an m30 is stupid and dangerous in my opinion !! As stated , this would be a parameter setting , but since the boss would have flipped if we messed with the parameters , it stayed that way

I don't recall saying g98-99 are not used for canned cycles so i don't get your point . And I never once said that a g80 doesn't cancel a drill cycle but I have said it will not cancel a g98 . Clearly you lack the understanding of what a modal command is about . There is a reason you don't have to add g1 to every line once it is called , same goes for any other modal command
Like I said , I always program them in and I'm not going t argue the point any further . I physically sat down at my pathpilot controller and hand coded a drill cycle which i did not add a g98 or g99 , it worked fine , why ? , because g99 was defaulted on start up . It is a modal command , it does not get cancelled with a g80 . So you can continue to argue whatever point you are trying to make but it works !

[jwatte]

using a program that uses g55 and having the machine default back to g54 upon a reset or when reaching an m30 is stupid and dangerous in my opinion

I think it's totally understandable to have M30 go back to "machine reset state" but with homing retained. This includes G54. If you assume some other coordinate system in your program, make sure that's part of your safeline or initial setup. Safest is of course to always specify which work offset you're assuming, be it G54, G55, or something else.

[metalmayhem]

Certain reset I can agree with such as g52 shifts or whatnot that could cause potential disaster . But , I don't like it having a work shift change upon a machine reset or m30 . Reason being is that it can lead to issues if a guy needs to rerun sections and skip thru sections of a program for example . I almost had this bite me on the butt when I was new to hass after years of running fanuc and other controls (which didn't do that) . Of course the code can be edited in at those skip points but sometimes we may forget the important things at the time .
I agree that work shift codes should be programmed in as a properly formatted g code program should be . I've programmed and run in jobbing and production shops , so proper format is the rule

[jwatte]

issues if a guy needs to rerun sections

Haven't run a Haas, so I don't know what it does, but PathPilot, when doing "run from here," will apply all the various transforms in order (without doing the actual movements) to always have the right coordinate system.

However, if you edit the file, and cut out lines, or if you restart the controller in between, well, you're on your own :-)