[widget_maker]

I'm not a machinist, just a hobbiest trying to learn the solidworks/hsmxpress/post flow on my Tormach. So far, so good. I have milled pockets, islands, contours etc. Today, I thought I would add some drilling cycles to my testpart, a simple 1/4" hole, then a couple of 1/4" holes with a 1/2" drill used as a countersink.

When I loaded the program I got a G code error pointing to the first of the new cycles, it appeared to be pointing at the G80 line although I'm not sure how accurately the error lines are identified. I cut and pasted the first drilling cycle below. Any ideas if it's me or the post program?

I don't really know what ending a "canned cycle" means.
thanks!

(================================================= ======)
(Drill1)
()
(Z Range MIN: -0.04, MAX: 0.6)
(================================================= ======)

N17005 M05
N17010 M09
N17015 M998
N17020 T16 M06
N17025 S1000 M03
N17030 X3.3 Y-1.3
N17035 G43 Z0.6 H16
N17040 G17
N17045 G00 Z0.2
N17050 G98 G81 X3.3 Y-1.3 Z-0.34 R-0.14 F40.
N17055 G80
N17060 Z0.6

[RussMachine]

G80 cancels all canned cycles.
A "Canned Cycle" is basically a little routine to do the same thing (cycle) at different locations.
Like drilling, tapping, turning on a lathe, threading on a lathe, etc.
Your drilling canned cycle is on line 17050 (N17050) with G98 (Return to initial Z reference) , G81 (Drill) , Z (Depth), R-.140 (drilling start point) , and F40 (Feedrate)
It will drill ONE hole at this X,Y location.
If you want to drill more holes, you need to delete that G80 on the next line, since it cancels your drilling cycle.
Then add X,Y locations on individual lines, until finished.
THEN put in a G80 to cancel the drilling cycle.
Also.. the R-.14 makes me nervous.
Are you starting the drilling cycle .140 BELOW the top of your part, as in a counterbore?
I hope this helps. It's kinda hard to explain without typing a whole page.

[Philbobb]

Any details on the error, specific verbage?

Your feed is a little high as well, should be closer to 8 in/min at 1000rpm, assuming 6061.

[widget_maker]

Yes, please ignore feeds and speeds, they are defaults - this is simply a test case to discover problems like I'm having.

I made an even simpler test case with a single hole drilled. Not countersunk or anything, a simple through hole.

Here's the error:

Attachment 271482

And here's the gcode created from hsmxpress and the post mentioned in an earlier thread here.

%
O
N10 G90 G94 G17
N15 G20
( )


(@ToolTable)
(T1, 1/4, Max Depth: -0.8651)


(Operation List
( 00:00:00, Drill1, 1/4, ZRange: MIN: -0.8651, MAX: 0.6 )
( 00:00:00 Total Time )



(================================================= ======)
(Drill1)
()
(Z Range MIN: -0.8651, MAX: 0.6)
(================================================= ======)

N25 M05
N30 M998
N35 T1 M06
N40 S1000 M03
N45 G54
N50 G00 X-0.2865 Y0.
N55 G43 Z0.6 H01
N60 G17
N65 G00 Z0.2
N70 G98 G73 X-0.2865 Y0. Z-0.8651 R-0.34 Q0.0625 F40.
N75 G80
N80 Z0.6
N90 M05
N95 M998
N100 T1(LOAD FIRST TOOL)
N105 M30
%

[widget_maker]

On pathpilot, the "edit gcode" feature shows line 36 as being the N90 M05 line. Not sure if it's relevant since the error says "near line 36"

[widget_maker]

This is the code created by the "generic Tormach post" on hsmxpress. It works on the machine!
Trouble is, this post fails for general machining giving "radius too small" errors at certain points.

%
(DRILL1)
(T1 D=0.25 CR=0. TAPER=118DEG - ZMIN=-0.8651 - DRILL)
N10 G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
N20 G20
N30 G28 G91 Z0.
N40 G90

(DRILL1)
N50 M998
N60 T1 G43 H1 M6
N70 S1000 M3
N80 G54
N90 G0 X-0.2865 Y0.
N100 M9
N110 G0 Z0.6
N130 G0 Z0.2
N140 G98 G73 X-0.2865 Y0. Z-0.8651 R-0.34 Q0.0625 F40.
N150 G80
N160 G0 Z0.6

N180 M9
N190 G28 G91 Z0.
N200 G28 X0. Y0.
N210 M30

[SCzEngrgGroup]

It's complaining about this line:

N80 Z0.6

This is right after the G80. No motion modal is in effect, so it doesn't know what to do about this. Make it:

N80 G0 Z0.6

and I bet it's happy.

Regards,
Ray L.

[widget_maker]

It's complaining about this line:

N80 Z0.6

This is right after the G80. No motion modal is in effect, so it doesn't know what to do about this. Make it:

N80 G0 Z0.6

and I bet it's happy.

Regards,
Ray L.

I'll try it in a bit....

Should I EXPECT to have to manually edit a post output? Is that standard or should I expect better?

[SCzEngrgGroup]

I'll try it in a bit....

Should I EXPECT to have to manually edit a post output? Is that standard or should I expect better?

You should absolutely expect better. I never edit the code I get out of HSMXpress.

Regards,
Ray L.

[widget_maker]

You should absolutely expect better. I never edit the code I get out of HSMXpress.

Regards,
Ray L.

You were right, your modification worked. So, I have several posts available on the web all seem to have issues one way or the other.

By the way Ray, I found YOUR post and it "compiled" just fine (by compiled I mean Pathpilot never through up an error message when it was loaded- wrong terminology I'm sure) but unfortunately, it looked set up for a tool changer and ignored my manual tool numbers in the program. For example, my first tool was tool #11, and your program asked for tool 1 (of course tool 1 offset is set too etc).

What is confusing is that others have used these post programs and have had no issues...........

[SCzEngrgGroup]

I uploaded a copy of my HSMXpress post some time ago because others asked for it. What I have is setup for my use, not for a Tormach, and it does some things, like re-numbering the tools, that others might not like. But, there are several people here who are using it, suitably modified for their Tormachs. Make a post asking for it, and I'm sure someone will pass it along. The changes to make it work with a Tormach should be pretty trivial.

Regards,
Ray L.

[dneisler]

widget_maker,
If I recall you are trying to use the HSMexpress post I modified, if so it started as Rays. I use it every day with no issues, thought, I have not tried it on PathPilot yet. I have no issues with it on Mach 3.

I have PP installed on a second hard drive but I have not had a chance to do any testing as i been to busy with production jobs.
If you need any assistance with the post I modified, feel free to PM me.

[vmax549]

Just remember that the Path Pilot(LiuxCNC) and the OLD Mach3 talk 2 different versions of Gcode. Close but NOT the same thing. The G80 is ONLY suppose to cancel the Canned cycles. It should NOT cancel ALL modality of the System.( LinuxCNC bug)

Mach3 will run that code as is.

This IS something yous guys will have to learn to deal with UNTIL PathPilot Specific POST are made available. I am SURE it will not be long until they are.

Just a thought, (;-) TP

[SCzEngrgGroup]

Just remember that the Path Pilot(LiuxCNC) and the OLD Mach3 talk 2 different versions of Gcode. Close but NOT the same thing. The G80 is ONLY suppose to cancel the Canned cycles. It should NOT cancel ALL modality of the System.( LinuxCNC bug)

Mach3 will run that code as is.

This IS something yous guys will have to learn to deal with UNTIL PathPilot Specific POST are made available. I am SURE it will not be long until they are.

Just a thought, (;-) TP

Fixing that in the HSMXpress post is trivial - it's a one-line change.

Regards,
Ray L.

[vmax549]

What you really NEED to know is exactly what Modal values does the G80 turn off in PP SO they can be turned back ON via Gcode.

Just a thought, (;-) TP

[SCzEngrgGroup]

What you really NEED to know is exactly what Modal values does the G80 turn off in PP SO they can be turned back ON via Gcode.

Just a thought, (;-) TP

It's all in the LinucCNC documentation:

G80 - cancel canned cycle modal motion. G80 is part of modal group 1, so programming any other G code from modal group 1 will also cancel the canned cycle.

It is an error if:

Axis words are programmed when G80 is active.

Modal group 1 contains: G0, G1, G2, G3, G33, G38.x, G73, G76, G80, G81, G82, G83, G84, G85, G86, G87, G88, G89

The post KNOWS which modal(s) are in effect when the canned cycles is executed, so it can easily restore them.

Regards,
Ray L.

[Steve Seebold]

Well, I have seen and read the examples of a drilling program that have been posted by folks using Path Pilot, and after what I have seen, "I DON'T WANT IT".

I hope Tormach's plan is is to offer both operating systems. If they switch to Path Pilot exclusively, I will become a Haas customer once again

[widget_maker]

But isn't the program a function of the post processor, and not PAth pilot? The posts I have tried have all been available ebfore Path Pilot existed, none are specific for it.

[SCzEngrgGroup]

But isn't the program a function of the post processor, and not PAth pilot? The posts I have tried have all been available ebfore Path Pilot existed, none are specific for it.

The program is, but the fact that PathPilot, and LinuxCNC, are implemented such that G80 invalidates ALL Group 1 modals is part of PathPilot. That said. Who cares? Make a one-line change to the POST, and it'll never be a problem. EVERY g-code interpreter has features like this that are different from others. It's really not a big deal.

Regards,
Ray L.

[SCzEngrgGroup]

I hope Tormach's plan is is to offer both operating systems. If they switch to Path Pilot exclusively, I will become a Haas customer once again

Better get ready to put your money where your mouth is. Tormach has made it crystal clear that Mach3 will be "end-of-lifed" very soon (once PathPilot is out of "beta"), and they will support only PathPilot going forward.

Regards,
Ray L.