[oldlock]

Hi Guys

I'd appreciate if someone with experience of tormach / g-code could cast their eye over this.

I have done drilling operations before with no issues but this has me stumped.

Scenario - step 4 of a program (I'm having to run them individually as the ATC is offline).

1 to 3 work fine, All tools are correctly measured and offset.

Then this simple drilling operation is run. In this case the drill is driven deep beside the work for no reason I can see. Then dragged into the side of the work (snap) and across to the start point of the hole. The chuck then raises and the program works as I would expect it to. Then it slams back down far too deep into the work.

The code was created in Fusion 360 and the simulation runs fine. The post processsor has not changed. The machine has been updated to 2.7.3 but I rolled it back to 2.7.2 and it still does the same thing.

I"d appreciate any insights !

[Clive S]

According to this article

The G98 and G99 G Codes
The G98 and G99 G Codes
Here is this program explained line by line

Z15.0 M08;

First, we bring the drill down to 15mm above the surface of the material and turn on the coolant with M08

G82 G99 Z-4.0 R1.0 P500 F50.0;

This line sets our counterbore canned cycle by using G82 and sets the movement to our hole with G99, this tells the machine that once the first hole is drilled to retract to the R1.0 value and not the Z15.0 set by the line above.
The Z-4.0 is the depth of the counterbore
The P500 value is the dwell time that is set to 500 milliseconds that will take place once the drill has reached the bottom of the hole.
F is our feed rate in mm/min.

X20.0;

This is the distance from the first hole to the second along the X axis, it is taken as an incremental move and can include a Y movement and an optional Z depth if the depth of the hole differs from the first. The G99 code is still active from the line above so the drill will retract to 1.0mm above the surface as defined by the R value.

G98 X40.0;

This line drills our third hole 40mm in the plus direction along the X axis. It retracts to Z15.0 above the surface of the part after drilling the previous hole. The G98 code tells the control that we wish to ignore the retract value of 1mm that we defined by R in our canned cycle line and to return to the Z15.0 distance. Safely above our clamp.

G99 X20.0;

The final hole is drilled 20mm in X from the last hole, the G99 code tells the machine to retract back to the R position and not the Z position.

G80;

The G80 command is the G Code we use to tell the control that the canned cycle has ended.

It is common to make the mistake of putting the G98/G99 on the wrong line. An easy way to remember it is that we add it to the hole position after the obstacle and not on the hole position before.

[soofle616]

Nothing is jumping out at me. Are you sure your tool length is properly set? Are you using the right work offset? Can you share the entire program instead of just the drill op?

[mactec54]

Hi Guys

I'd appreciate if someone with experience of tormach / g-code could cast their eye over this.

I have done drilling operations before with no issues but this has me stumped.

Scenario - step 4 of a program (I'm having to run them individually as the ATC is offline).

1 to 3 work fine, All tools are correctly measured and offset.

Then this simple drilling operation is run. In this case the drill is driven deep beside the work for no reason I can see. Then dragged into the side of the work (snap) and across to the start point of the hole. The chuck then raises and the program works as I would expect it to. Then it slams back down far too deep into the work.

The code was created in Fusion 360 and the simulation runs fine. The post processsor has not changed. The machine has been updated to 2.7.3 but I rolled it back to 2.7.2 and it still does the same thing.

I"d appreciate any insights !

What's the G30 for is this your control requirement???

Header has code that can cancel your tool offsets

G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49

This is all you need in the header

G90 G17G40G80

G90 is only needed in the header if you don't have it in your program
G49 can cancel your tool offset in some controls

Your post processor is of poor design

Really need to see the whole program to see where the real problem is

[metalmayhem]

What's the G30 for is this your control requirement???

Header has code that can cancel your tool offsets

G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49

This is all you need in the header

G90 G17G40G80

G90 is only needed in the header if you don't have it in your program
G49 can cancel your tool offset in some controls

Your post processor is of poor design

Really need to see the whole program to see where the real problem is

the processor is a turd . g30 is return home which is handy when hand bombing tools . A G64P#### is also important to have in the header but not necessary in this case

[mactec54]

the processor is a turd . g30 is return home which is handy when hand bombing tools . A G64P#### is also important to have in the header but not necessary in this case

Yes that is obvious, what is the G64P#### used for that you would want it in the header

G30 why would you want your machine to return to home at the start of a program is this what they have you do with PP control or just a goofy Post processor

[metalmayhem]

you can go with a g53 or just return home g30 , nothing goofy about it if a tool change may be needed . it doesn't necessarily have to been in the header but it doesn't hurt anything either
G64 is toolpath control the p value is a tolerance , I punch g64p.001 into all my headers . I've had pathpilot do some funky stuff without the tolerance added

[mactec54]

you can go with a g53 or just return home g30 , nothing goofy about it if a tool change may be needed . it doesn't necessarily have to been in the header but it doesn't hurt anything either
G64 is toolpath control the p value is a tolerance , I punch g64p.001 into all my headers . I've had pathpilot do some funky stuff without the tolerance added

Neither a G53 or a G30 is required at the start of any program

You don't need a G30 because you are going to do a Tool Change, as soon as a Tool is called T26 in his case the Z axis will move to the tool change position

[metalmayhem]

as soon as a Tool is called T26 in his case the Z axis will move to the tool change position

with atc yes , without atc no

[jwatte]

with atc yes , without atc no

In PathPilot, any M06 (too change) macro will move the spindle to the G30 height, even if you don't have the ATC.

[metalmayhem]

In PathPilot, any M06 (too change) macro will move the spindle to the G30 height, even if you don't have the ATC.

I haven't done anything to the macro and none of mine move to g30 on an m06 call , which is why I have my cam post a g30

[metalmayhem]

something I missed with that code was g30 is alone which is goofy
I automatically think g30z0

[machinehop5]

...is it just me or is this normal format of a program that F360 produces? Why would they put the G43 H26 on the same Line as the TC and before calling the Workoffsets? Also, should have G49 H0D0 at the end of each Tool. Very sloppy programming looks like to me.

%
(1005)
(Machine)
( vendor Autodesk)
( description Generic 3-axis)
(T26 D=5. CR=0. TAPER=118deg - ZMIN=-15.5 - drill)
G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
G21 (Metric)
G30

N10(Drill5 3)
T26 G43 H26 M6
S5000 M3 M8
G54
G0 X17.214 Y27.
G0 Z15.
G0 Z5.
G98 G81 X17.214 Y27. Z-15.5 R2.5 F1000.
X-17.1
G80
G0 Z15.
M5 M9

G30
M30
%

[metalmayhem]

...is it just me or is this normal format of a program that F360 produces? Why would they put the G43 H26 on the same Line as the TC and before calling the Workoffsets? Also, should have G49 H0D0 at the end of each Tool. Very sloppy programming looks like to me.

%
(1005)
(Machine)
( vendor Autodesk)
( description Generic 3-axis)
(T26 D=5. CR=0. TAPER=118deg - ZMIN=-15.5 - drill)
G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
G21 (Metric)
G30

N10(Drill5 3)
T26 G43 H26 M6
S5000 M3 M8
G54
G0 X17.214 Y27.
G0 Z15.
G0 Z5.
G98 G81 X17.214 Y27. Z-15.5 R2.5 F1000.
X-17.1
G80
G0 Z15.
M5 M9

G30
M30
%

it's a pretty bad format , plus it's poor to have 2 m codes on the same line

[kstrauss]

...is it just me or is this normal format of a program that F360 produces? Why would they put the G43 H26 on the same Line as the TC and before calling the Workoffsets? Also, should have G49 H0D0 at the end of each Tool.

I'm certainly not a gcode expert but I don't understand your criticisms. The H26 is redundant but what is the problem with putting the G43 on the same line as the tool change? Keeping them together is, in my opinion, just good programming style. Why is it required (or even desirable for that matter) to include a G49? Won't the G43 on the next tool change change the offset?

[machinehop5]

[QUOTE=kstrauss;2449352]

The H26 is redundant but what is the problem with putting the G43 on the same line as the tool change?

no problem if, the machine can handle the Code on the same Line.

Why is it required (or even desirable for that matter) to include a G49?

good practice safe block G49H0D0.

Won't the G43 on the next tool change change the offset?

yes, but what happens if the Operator does something in between Tool changes in MDI and does not realize a Tool Comp is active still.

Murphy's Law

[kstrauss]

I hesitate to mention that this message board is solely devoted to Tormach controllers so whether a another controller works differently (or fails to handle a particular command) is irrelevant. In that vein, the operator cannot issue MDI commands "between tool changes".

In my opinion values should not be given in two places for the same thing -- that only results in errors. Hence, NEVER use H? to specify the default tool used by G43.

[mactec54]

...is it just me or is this normal format of a program that F360 produces? Why would they put the G43 H26 on the same Line as the TC and before calling the Workoffsets? Also, should have G49 H0D0 at the end of each Tool. Very sloppy programming looks like to me.

%
(1005)
(Machine)
( vendor Autodesk)
( description Generic 3-axis)
(T26 D=5. CR=0. TAPER=118deg - ZMIN=-15.5 - drill)
G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
G21 (Metric)
G30

N10(Drill5 3)
T26 G43 H26 M6
S5000 M3 M8
G54
G0 X17.214 Y27.
G0 Z15.
G0 Z5.
G98 G81 X17.214 Y27. Z-15.5 R2.5 F1000.
X-17.1
G80
G0 Z15.
M5 M9

G30
M30
%

Because these guys that wrote this post processors are programmer's and have no machine experience or what is a correct G-Code format should look like

[kstrauss]

Because these guys that wrote this post processors are programmer's and have no machine experience or what is a correct G-Code format should look like

Is there a style guide for gcode? Where do I find it?

[mactec54]

Is there a style guide for gcode? Where do I find it?

The best Style Format is standard Fanuc there are variations of this format for slight changes, that different manufactures use in there controls But the basic's are the same, this is very much industry standard that all controls use

For hobby guys anything that works for them is what they use, then when a crash happens they don't know what to do be cause it looks right to them, keep it simple Here is a simple format that will work on most machines, you just add or change this format which is simple and easy to see where you can make a change to how ever you want it to work for you

Keep it simple is best as it is easy to see if you have a problem some where

%
( O1503 Drill Mag Block )
G17G40G80
( could put your G30 Here if you needed it Tormach only or anyone using PP Can use a G0Z---- also )
T4M6
M8
G54
S2250M3
G90G0X1.75Y-.384
G43Z.1H4
G83G98X1.75Y-.384Z-.4276R.1Q.03F8.
X1.375Y-.216
X1.Y-.384
X.625Y-.216
X.25Y-.384
G80G0Z3. ( Canned cycle Canceled Z moves up 3 inches )
M9
M5
G53Y0. ( This can be used with X as well and any number where you want your table to move too when your job is complete )
M30
%