Re: G28.1 problems THC300 setup Mach3

Yahoo posts
1

Yes im using the latest version of Mach3,I think my problem is with
the g28.1 routine which is a reference home command,i don’t see how
this would ever work for someone!From what i got from it,is that it
moves a axis toward the ref switch,and sets the machine cords to o.oo
so if i set my z axis up so it homes toward the table(which is wrong)
this will go down and touch off the plate and then next line of code
set 0.00 it would kinda work ,but now the machine mech limits are
ref off of the plate surface and not the physical min and max
travels of the that axis.This way seems all wrong and the g31 probe
comand should be the way to go,but i will have to find the right
post processor for sheetcam to add the right m03,m05 to the code in
the right place,and change the m03 in thc300 folder for the code
from bob cambells pdf,but there is the problem i can’t find that m03
file anywhere ,can anyone help me on this,I got a headache from this
one,looking at the code in the pdf its all wrong and looks like it
won’t work there is (wendif),
I would think i’m not the only person running the THC300 kit and the
THC300 setup files,But bob’s Websits is missing the m03 file for
everything to work,and the sheetcam post processor also to work
along with the m03.

Any help would be nice.

Thanks Erik


— In sheetcam@yahoogroups.com, Ray Hager <rayhager7@…> wrote:

This sounds similar to a problem I was having with Mach3. You

didn’t say what CNC program you are using but when I first tried to
get this to work using Sheetcam and Mach3 it was acting like
something was backwards.

To get it to work correcty I had to change Config/Homing/Limits

(Mach3) and check ‘Home Neg’.

Hope this helps,
Ray

Erik <pfauto@…> wrote:

Hi all,
Here is my problem i’m having with the sheetcam post processor or

the

g28.1 code in general,When the machine is running through the code

and

it gets to the g28.1 z.12,the machine rapids down to the .500

above

the surface from previous code then moves down to .120 then tryies

to

move up to the z home switch, which is 8.00 all the way up at the

top

of the z axis, i think it should be trying to find the top of the
plate by moving more negitive and then set this at 0.0 then move

to

cut height and on from there.Where am i going wrong on this,or

what

setting do i have wrong.Also i have to shut off softlimits to even

get

this far with soft max set at 8.00 and -1.00 for z min and have

tryied

z min 0.0 both still don’t work.

Thanks in advance Erik






[Non-text portions of this message have been removed]

2

I have to admit I also think probe is better than home. Home should be
for the machine’s physical limits, not the position of the work.
Probably very few people bother to use soft-limits. Without soft-limits
it doesn’t really matter where the Z home is. ISTR that the earlier THC
posts did use probe but there were reliability problems. It may well be
that the problems have now been solved with the later versions of Mach.

You should either use a Mach M03 macro to do the probe and use a non-THC
post or let SheetCam take care of all of the work. Trying to mix the two
is likely to cause more problems than it solves.

Erik, if you work out the correct G-code sequence for a probe-zero
cycle, I’ll write a post that will generate it for you. I can’t test the
code myself as I don’t have THC. In fact my plasma isn’t even working at
the moment…

Les


Erik wrote:

Yes im using the latest version of Mach3,I think my problem is with
the g28.1 routine which is a reference home command,i don’t see how
this would ever work for someone!From what i got from it,is that it
moves a axis toward the ref switch,and sets the machine cords to o.oo
so if i set my z axis up so it homes toward the table(which is wrong)
this will go down and touch off the plate and then next line of code
set 0.00 it would kinda work ,but now the machine mech limits are
ref off of the plate surface and not the physical min and max
travels of the that axis.This way seems all wrong and the g31 probe
comand should be the way to go,but i will have to find the right
post processor for sheetcam to add the right m03,m05 to the code in
the right place,and change the m03 in thc300 folder for the code
from bob cambells pdf,but there is the problem i can’t find that m03
file anywhere ,can anyone help me on this,I got a headache from this
one,looking at the code in the pdf its all wrong and looks like it
won’t work there is (wendif),
I would think i’m not the only person running the THC300 kit and the
THC300 setup files,But bob’s Websits is missing the m03 file for
everything to work,and the sheetcam post processor also to work
along with the m03.

Any help would be nice.

Thanks Erik

3

Erik,
Are you using a floating head to hold the torch on the Z axis ?
The THC post is written to work with one.
If so; then have it home toward the table. It will hit the work and the head will ride up and hit the switch . The post will make the calculations to using the pierce height and the switch travel to move the torch tip the the proper pierce height.
I have some photos I can send you when I get back to my office of a floating head if they would be of help.
Jim

Erik <pfauto@comcast.net> wrote:
Yes im using the latest version of Mach3,I think my problem is with
the g28.1 routine which is a reference home command,i don’t see how
this would ever work for someone!From what i got from it,is that it
moves a axis toward the ref switch,and sets the machine cords to o.oo
so if i set my z axis up so it homes toward the table(which is wrong)
this will go down and touch off the plate and then next line of code
set 0.00 it would kinda work ,but now the machine mech limits are
ref off of the plate surface and not the physical min and max
travels of the that axis.This way seems all wrong and the g31 probe
comand should be the way to go,but i will have to find the right
post processor for sheetcam to add the right m03,m05 to the code in
the right place,and change the m03 in thc300 folder for the code
from bob cambells pdf,but there is the problem i can’t find that m03
file anywhere ,can anyone help me on this,I got a headache from this
one,looking at the code in the pdf its all wrong and looks like it
won’t work there is (wendif),
I would think i’m not the only person running the THC300 kit and the
THC300 setup files,But bob’s Websits is missing the m03 file for
everything to work,and the sheetcam post processor also to work
along with the m03.

Any help would be nice.

Thanks Erik


— In sheetcam@yahoogroups.com, Ray Hager wrote:

This sounds similar to a problem I was having with Mach3. You

didn’t say what CNC program you are using but when I first tried to
get this to work using Sheetcam and Mach3 it was acting like
something was backwards.

To get it to work correcty I had to change Config/Homing/Limits

(Mach3) and check ‘Home Neg’.

Hope this helps,
Ray

Erik

wrote:

Hi all,
Here is my problem i’m having with the sheetcam post processor or

the

g28.1 code in general,When the machine is running through the code

and

it gets to the g28.1 z.12,the machine rapids down to the .500

above

the surface from previous code then moves down to .120 then tryies

to

move up to the z home switch, which is 8.00 all the way up at the

top

of the z axis, i think it should be trying to find the top of the
plate by moving more negitive and then set this at 0.0 then move

to

cut height and on from there.Where am i going wrong on this,or

what

setting do i have wrong.Also i have to shut off softlimits to even

get

this far with soft max set at 8.00 and -1.00 for z min and have

tryied

z min 0.0 both still don’t work.

Thanks in advance Erik






[Non-text portions of this message have been removed]

4

Erik,
Did you get the THC300 touch off issue resolved?
I am home now and can help you work through it.
Thank You
Jim Cullins
----- Original Message -----
From: “Erik” <pfauto@comcast.net>
To: <sheetcam@yahoogroups.com>
Sent: Friday, April 13, 2007 3:44 PM
Subject: [sheetcam] Re: G28.1 problems THC300 setup Mach3


Yes im using the latest version of Mach3,I think my problem is with
the g28.1 routine which is a reference home command,i don’t see how
this would ever work for someone!From what i got from it,is that it
moves a axis toward the ref switch,and sets the machine cords to o.oo
so if i set my z axis up so it homes toward the table(which is wrong)
this will go down and touch off the plate and then next line of code
set 0.00 it would kinda work ,but now the machine mech limits are
ref off of the plate surface and not the physical min and max
travels of the that axis.This way seems all wrong and the g31 probe
comand should be the way to go,but i will have to find the right
post processor for sheetcam to add the right m03,m05 to the code in
the right place,and change the m03 in thc300 folder for the code
from bob cambells pdf,but there is the problem i can’t find that m03
file anywhere ,can anyone help me on this,I got a headache from this
one,looking at the code in the pdf its all wrong and looks like it
won’t work there is (wendif),
I would think i’m not the only person running the THC300 kit and the
THC300 setup files,But bob’s Websits is missing the m03 file for
everything to work,and the sheetcam post processor also to work
along with the m03.

Any help would be nice.

Thanks Erik


— In > sheetcam@yahoogroups.com> , Ray Hager <rayhager7@…> wrote:

This sounds similar to a problem I was having with Mach3. You

didn’t say what CNC program you are using but when I first tried to
get this to work using Sheetcam and Mach3 it was acting like
something was backwards.

To get it to work correcty I had to change Config/Homing/Limits

(Mach3) and check ‘Home Neg’.

Hope this helps,
Ray

Erik <pfauto@…> wrote:

Hi all,
Here is my problem i’m having with the sheetcam post processor or

the

g28.1 code in general,When the machine is running through the code

and

it gets to the g28.1 z.12,the machine rapids down to the .500

above

the surface from previous code then moves down to .120 then tryies

to

move up to the z home switch, which is 8.00 all the way up at the

top

of the z axis, i think it should be trying to find the top of the
plate by moving more negitive and then set this at 0.0 then move

to

cut height and on from there.Where am i going wrong on this,or

what

setting do i have wrong.Also i have to shut off softlimits to even

get

this far with soft max set at 8.00 and -1.00 for z min and have

tryied

z min 0.0 both still don’t work.

Thanks in advance Erik






[Non-text portions of this message have been removed]

5

— In sheetcam@yahoogroups.com, Leslie Newell <lesnewell@…> wrote:

I have to admit I also think probe is better than home. Home

should be

for the machine’s physical limits, not the position of the work.
Probably very few people bother to use soft-limits. Without soft-

limits

it doesn’t really matter where the Z home is. ISTR that the

earlier THC

posts did use probe but there were reliability problems. It may

well be

that the problems have now been solved with the later versions of

Mach.

You should either use a Mach M03 macro to do the probe and use a

non-THC

post or let SheetCam take care of all of the work. Trying to mix

the two

is likely to cause more problems than it solves.

Erik, if you work out the correct G-code sequence for a probe-zero
cycle, I’ll write a post that will generate it for you. I can’t

test the

code myself as I don’t have THC. In fact my plasma isn’t even

working at

the moment…

Les

i respectfully disagree on the Z home issue. Homes define a
specific known location. Most homes are used to either define a
table 0 or an offset from a zero. The X and Y 0 points on a table
are vital locations to know in order to re-position in the case a
loss of position while cutting. The whole point of “referencing” is
to establish a known point from which all other moves evolve.

Z is another matter. It’s normally accepted that the top of
material is the Z 0. not some place up in the air on the Z axis. In
plasma it’s even more important to find the top of material as heat
and forces make that change. With SheetCAM you have the option of
not having to re-establish TOM (Top Of Material)by using the
refdistance variable. No other CAM solution offers this and it’s
valuable.

Using the Z home as the touch off on z offers the fact you can add
in the switch offset (negative number) in MACH in the Homing section
or use the switch offset value in SheetCAM.

The probe is used to extablish points above zero.

It’s not hard to use either. With almost 500 units (THC300 and
MP1000 Digital units) in use and a lot of them using SheetCAM, we
know the approach works.

You are right about trying to use a mixed approach of the custom M03
macro AND the Sheetcam approach…it dosen’t work.

6

Hi Tom,

i respectfully disagree on the Z home issue. Homes define a
specific known location.

On pretty much every CNC machine I have worked on, homes are used to
establish the machine’s absolute position(machine coordinates). Most
commercial machines will not let you do much until you have referenced
to the home switches.

Most homes are used to either define a
table 0 or an offset from a zero. The X and Y 0 points on a table
are vital locations to know in order to re-position in the case a
loss of position while cutting.

In most cases, homes aren’t at work at 0,0,0. They are at some arbitrary
position that is convenient to the machine manufacturer. Once the
machine knows it’s absolute position it can then use work offsets to
establish work 0,0,0

The whole point of “referencing” is
to establish a known point from which all other moves evolve.

Exactly. If you use the work as Z= machine 0 the the machine has no way
of knowing where the top of travel is. If you are using soft limits then
this is a major problem. If you aren’t using soft limits then it will
work fine, even if it isn’t technically correct. You’ll soon enough find
the top of travel when you hit the limit switch…

Z is another matter. It’s normally accepted that the top of
material is the Z 0.

Again we have the difference between machine coordinates and work
coordinates. Work X0,Y0,Z0 are not always the same place for every job.
Machine 0,0,0 should always be in the same place.

Using the Z home as the touch off on z offers the fact you can add
in the switch offset (negative number) in MACH in the Homing section
or use the switch offset value in SheetCAM.

You should be able to do this using probe as well. Instead of tweaking
the machine coordinates with home, you probe then tweak the work
coordinates. The end result to the user is the same, apart from the fact
that the machine still knows exactly where the ends of travel are.

The probe is used to extablish points above zero.

Probe can be used to establish points anywhere.

It’s not hard to use either. With almost 500 units (THC300 and
MP1000 Digital units) in use and a lot of them using SheetCAM, we
know the approach works.

The question is, how many are using soft limits? Without soft limits,
this distinction between work and machine coordinates is pretty
academic. I admit I haven’t actually used probe in this way and as you
say, you have a lot of experience using home. There is a strong argument
for ‘if it ain’t broke don’t fix it’. However the great thing about
SheetCam and Mach is that you can easily change things if you don’t like
the way they work.

Les

7

— In sheetcam@yahoogroups.com, Leslie Newell <lesnewell@…> wrote:

Hi Tom,

i respectfully disagree on the Z home issue. Homes define a
specific known location.

On pretty much every CNC machine I have worked on, homes are used to
establish the machine’s absolute position(machine coordinates). Most
commercial machines will not let you do much until you have

referenced

to the home switches.

Most homes are used to either define a
table 0 or an offset from a zero. The X and Y 0 points on a

table

are vital locations to know in order to re-position in the case a
loss of position while cutting.

In most cases, homes aren’t at work at 0,0,0. They are at some

arbitrary

position that is convenient to the machine manufacturer. Once the
machine knows it’s absolute position it can then use work offsets to
establish work 0,0,0

The whole point of “referencing” is
to establish a known point from which all other moves evolve.

Exactly. If you use the work as Z= machine 0 the the machine has no

way

of knowing where the top of travel is. If you are using soft limits

then

this is a major problem. If you aren’t using soft limits then it

will

work fine, even if it isn’t technically correct. You’ll soon enough

find

the top of travel when you hit the limit switch…

Z is another matter. It’s normally accepted that the top of
material is the Z 0.

Again we have the difference between machine coordinates and work
coordinates. Work X0,Y0,Z0 are not always the same place for every

job.

Machine 0,0,0 should always be in the same place.

Using the Z home as the touch off on z offers the fact you can

add

in the switch offset (negative number) in MACH in the Homing

section

or use the switch offset value in SheetCAM.

You should be able to do this using probe as well. Instead of

tweaking

the machine coordinates with home, you probe then tweak the work
coordinates. The end result to the user is the same, apart from the

fact

that the machine still knows exactly where the ends of travel are.

The probe is used to extablish points above zero.

Probe can be used to establish points anywhere.

It’s not hard to use either. With almost 500 units (THC300 and
MP1000 Digital units) in use and a lot of them using SheetCAM, we
know the approach works.

The question is, how many are using soft limits? Without soft

limits,

this distinction between work and machine coordinates is pretty
academic. I admit I haven’t actually used probe in this way and as

you

say, you have a lot of experience using home. There is a strong

argument

for ‘if it ain’t broke don’t fix it’. However the great thing about
SheetCam and Mach is that you can easily change things if you don’t

like

the way they work.

Les

8

Hi Les,

I agree with you on all those points,another thing is for it to work
the way Tom says the G28.1 way,i would have to set up my z axis in
Mach3 to Ref home toward the table,So when i first turn on my machine
in the morning or after last shift had it running ,I would hit ref
all axis under mach and the z would move toward the table and go into
the grid of the table,then trip the floating head switch,next the X
axis would try to move and bust the torch right off,this would not be
good,How in Toms way could you setup your physical limits and could
it be possible to use soft limits that Mach3 was designed for?

Like you said machine cords and work cords are two different things,I
wouldn’t want any Gcode running and messing with my physical limits
on the Min and Max travels of my machine.I’m a firm believer in soft
limits on all of my machines I build,My motors are very powerfull and
could damage it self if it went past them at full speed and I’m sure
alot of people use them,especialy on big mills with heavy loads this
is where soft limits would consider the load and ramp it down.

I think the Probe command would be the best way to go,because all I
want to do is set the surface as 0.00 and not my machine
cords,another benifit would be is I could adjust the lost switch
travel,cutting height,and others right at the computer for fine
tuning,but I like also letting the person setting up the drawing to
control these things,letting the operator sometimes might not be a
good thing for some shops,so having these under SheetCam are nice,it
would be nice if SheetCam and Mach could talk to each other some how
and have a overide for those setting at the computer if needed,maybe
SheetCam could set them in the begining and mach could have a overide
for them or a correction value.

I think I have it worked out now,but will still need to get the M03
from Bob or Jim,and use the right SheetCam post processor without the
THC.
Thanks for the help everyone.

Erik

— In > sheetcam@yahoogroups.com> , Leslie Newell <lesnewell@> wrote:

Hi Tom,

i respectfully disagree on the Z home issue. Homes define a
specific known location.

On pretty much every CNC machine I have worked on, homes are used

to

establish the machine’s absolute position(machine coordinates).

Most

commercial machines will not let you do much until you have

referenced

to the home switches.

Most homes are used to either define a
table 0 or an offset from a zero. The X and Y 0 points on a

table

are vital locations to know in order to re-position in the case

a

loss of position while cutting.

In most cases, homes aren’t at work at 0,0,0. They are at some

arbitrary

position that is convenient to the machine manufacturer. Once the
machine knows it’s absolute position it can then use work offsets

to

establish work 0,0,0

The whole point of “referencing” is
to establish a known point from which all other moves evolve.

Exactly. If you use the work as Z= machine 0 the the machine has

no

way

of knowing where the top of travel is. If you are using soft

limits

then

this is a major problem. If you aren’t using soft limits then it

will

work fine, even if it isn’t technically correct. You’ll soon

enough

find

the top of travel when you hit the limit switch…

Z is another matter. It’s normally accepted that the top of
material is the Z 0.

Again we have the difference between machine coordinates and work
coordinates. Work X0,Y0,Z0 are not always the same place for

every

job.

Machine 0,0,0 should always be in the same place.

Using the Z home as the touch off on z offers the fact you can

add

in the switch offset (negative number) in MACH in the Homing

section

or use the switch offset value in SheetCAM.

You should be able to do this using probe as well. Instead of

tweaking

the machine coordinates with home, you probe then tweak the work
coordinates. The end result to the user is the same, apart from

the

fact

that the machine still knows exactly where the ends of travel are.

The probe is used to extablish points above zero.

Probe can be used to establish points anywhere.

It’s not hard to use either. With almost 500 units (THC300 and
MP1000 Digital units) in use and a lot of them using SheetCAM,

we

know the approach works.

The question is, how many are using soft limits? Without soft

limits,

this distinction between work and machine coordinates is pretty
academic. I admit I haven’t actually used probe in this way and

as

you

say, you have a lot of experience using home. There is a strong

argument

for ‘if it ain’t broke don’t fix it’. However the great thing

about

SheetCam and Mach is that you can easily change things if you

don’t

like

the way they work.

Les

9

Eric,
You need to edit the RefAll Home button.
click on
Operator
Edit Botton Script
then click on REF ALL HOME button
a drop down will appear.
place an apsotrophe before the first line
as below
’ DoButton(24) ’ 24 is the Z axis home
Click on files and save.
Then it will home the Y, then X , the A if you have one.
I will change my Set file to reflect that.
Sorry for the confusion.
Jim


----- Original Message -----
From: “Erik” <pfauto@comcast.net>
To: <sheetcam@yahoogroups.com>
Sent: Monday, April 16, 2007 4:27 PM
Subject: [sheetcam] Re: G28.1 problems THC300 setup Mach3


Hi Les,

I agree with you on all those points,another thing is for it to work
the way Tom says the G28.1 way,i would have to set up my z axis in
Mach3 to Ref home toward the table,So when i first turn on my machine
in the morning or after last shift had it running ,I would hit ref
all axis under mach and the z would move toward the table and go into
the grid of the table,then trip the floating head switch,next the X
axis would try to move and bust the torch right off,this would not be
good,How in Toms way could you setup your physical limits and could
it be possible to use soft limits that Mach3 was designed for?

Like you said machine cords and work cords are two different things,I
wouldn’t want any Gcode running and messing with my physical limits
on the Min and Max travels of my machine.I’m a firm believer in soft
limits on all of my machines I build,My motors are very powerfull and
could damage it self if it went past them at full speed and I’m sure
alot of people use them,especialy on big mills with heavy loads this
is where soft limits would consider the load and ramp it down.

I think the Probe command would be the best way to go,because all I
want to do is set the surface as 0.00 and not my machine
cords,another benifit would be is I could adjust the lost switch
travel,cutting height,and others right at the computer for fine
tuning,but I like also letting the person setting up the drawing to
control these things,letting the operator sometimes might not be a
good thing for some shops,so having these under SheetCam are nice,it
would be nice if SheetCam and Mach could talk to each other some how
and have a overide for those setting at the computer if needed,maybe
SheetCam could set them in the begining and mach could have a overide
for them or a correction value.

I think I have it worked out now,but will still need to get the M03
from Bob or Jim,and use the right SheetCam post processor without the
THC.
Thanks for the help everyone.

Erik

— In > sheetcam@yahoogroups.com> , Leslie Newell <lesnewell@> wrote:

Hi Tom,
On pretty much every CNC machine I have worked on, homes are used

to

establish the machine’s absolute position(machine coordinates).

Most

commercial machines will not let you do much until you have

referenced

to the home switches.

table

a

In most cases, homes aren’t at work at 0,0,0. They are at some

arbitrary

position that is convenient to the machine manufacturer. Once the
machine knows it’s absolute position it can then use work offsets

to

establish work 0,0,0
Exactly. If you use the work as Z= machine 0 the the machine has

no

way

of knowing where the top of travel is. If you are using soft

limits

then

this is a major problem. If you aren’t using soft limits then it

will

work fine, even if it isn’t technically correct. You’ll soon

enough

find

the top of travel when you hit the limit switch…
Again we have the difference between machine coordinates and work
coordinates. Work X0,Y0,Z0 are not always the same place for

every

job.

Machine 0,0,0 should always be in the same place.

add

section

You should be able to do this using probe as well. Instead of

tweaking

the machine coordinates with home, you probe then tweak the work
coordinates. The end result to the user is the same, apart from

the

fact

that the machine still knows exactly where the ends of travel are.
Probe can be used to establish points anywhere.

we

The question is, how many are using soft limits? Without soft

limits,

this distinction between work and machine coordinates is pretty
academic. I admit I haven’t actually used probe in this way and

as

you

say, you have a lot of experience using home. There is a strong

argument

for ‘if it ain’t broke don’t fix it’. However the great thing

about

SheetCam and Mach is that you can easily change things if you

don’t

like

the way they work.

Les

10

Hi Les,
I got the M03 code to work,but I had to edit allot of this to make it work the way I want,Here is the code that I use in the M03,Bob’s website had one but don’t know how it would have worked for anyone right,since his code didn’t read the probe position it just went back up the switch travel and the cutheight,since my z axis had a 10:1 gear reduction it took longer to come to a stop and over shot the switch well bob’s didn’t add this in to move back up to so it left the torch on the plate :)Here is my Revised version which should work for most people Using the THC300 Boards,I Comment my code so anyone can read it without any question as to what it does.

'M03 Code
'THC300 Users With Floating Head Running The M03 G31 Probe Cycle,By Erik Pecchi CNCINMOTION.COM(Rev 1) 4-23-07
'Note found out if you have a spindle DWELL other than 0 it will not add the correct PierceDelay after turning on the Torch
'Users should use the P&F SET File for proper DRO’S and Leds on the screen,But you just need the right ones on any screen Set,See below
'DRO’S (1000,1001,1002,1003)

CurrentFeed = GetOemDRO(818) 'Get The Current Feedrate

ProbeFeed = 20 '(testing for now) GetUserDRO(1152) 'You Could Put A Probing Feedrate Here Instead

CutHeight = GetUserDRO(1003) 'This Reads The THC300.Set Screens Intinal Cut Height DRO

SwitchTravel = GetUserDRO(1002)'This Reads The THC300.Set Screens Switch Travel DRO

PierceDelay = GetUserDRO(1001)'This Reads The PierceDelay DRO

PierceHeight = GetUserDRO(1000)'This Reads The PierceHeight DRO


'Code “G90 F” &ProbeFeed
If GetOemLed (825)=0 Then ’ This Is The Digitize Input Pin
Code “G31Z-8 F” &ProbeFeed’This Moves Z Axis Down 8" This Is A User Defined Travel
While IsMoving()
Wend
Code “G4 P0.25”'Pause For Dro To update,don’t really need these tho
ZProbePos = GetVar(2002)'This Is The Probe Positions DRO
Code “G0 Z” &ZProbePos 'Move Back To Where The Switch Was Closed
While IsMoving ()
Wend
Code “G92Z0” 'Zero’s The Z To 0.0 -Another Way Is To Insert This Code To Update The DRO “Call SetDro (2, 0.0)”
Code “G4 P0.25” 'Pause For Dro To Update.
Code “G0 Z” &(PierceHeight + SwitchTravel) 'Change The Z To Pierce Height + SwitchTravel,see below Pierce up high
Code “F” &CurrentFeed
While IsMoving ()
Wend
DoSpinCW()
Code “G4 P” & (PierceDelay)
Code"G0Z"&CutHeight ’ Pierced up high then go to cut height
Code “F” &ProbeFeed

Else
Code “(Torch Is On Surface Hit STOP Button,& Fix Torch Tip)”
Exit Sub
End If



Now here is another thing that i need to get resolved,Since i don’t need SheetCam to worry about the Piercedelay,EndDelay,CutHeight,or PierceHeight,I’m not sure what post to use so i’m starting with the simplest one mach2plasma.post, How can i get rid of the PierceHeight when using the Mach2.Post,Running this post it inserts the PierceHeight of 0.00 which makes the torch go to the surface,then it runs the M03,Here is a example from the mach2 plasma .Post,not sure if this is where it is or not to be looking?


function pendown()
if (preheat > 0.001) then
modaltext (" G00")
modalnumber (" Z", cutheight * scale, “0.0000”)
text (“\n G04 P”)
number (preheat,“0.###”)
eol()
end
modaltext (" G00")
modalnumber (" Z", pierceheight * scale, “0.0000”)
text (“\n M03\n”)
if (piercedelay > 0.001) then
text (" G04 P")
number (piercedelay,“0.###”)
eol()
end
end




I opened the Mach2plasma.post file and under the Pendown i see there you check to see if Preheat is Greater then 0.001 then do something but under PierceHeight there is no if statement checking if it is Greater then 0.001 then don’t insert the code ,

Modaltext(“G00”)
Modalnumber(“z”,PierceHeight*scale.“0.000”)
text(“\nM03\n”)


I’m not sure how this code is being used,but looks close to VB

I Just need sheetcam to check the PierceHeight and see if it is 0.000 then Don’t insert the Pierceheight line of code.
Here is a small shape that i have been working on,and the Gcode it creates:

N0000 (Filename: leg plate.tap)
N0010 (Post processor: P&F.post)
N0020 (Date: 4/23/2007)
N0030 G20 (Units: Inches)
N0040 G53 G90 G40
N0050 F1
N0060 S500
N0070 (Part: leg plate)
N0080 (Process: Plasma, 1, 1\2" Steel .060Kerf)
N0090 G00 Z0.5000
N0100 M06 T2 F35 (1\2" Steel .060Kerf)
N0110 G00 Z0.5000
N0120 X0.2973 Y0.3145
N0130 Z0.0000 -------------------------------------------This is where i don’t need this line of code
N0140M03
N0150 G02 X0.1550 Y0.5000 I0.0497 J0.1855 F35.0
N0160 X0.1550 Y0.5000 I0.3450 J0.0000
N0170 X0.1906 Y0.5464 I0.0480 J0.0000
N0180 M05
N0190 G00 Z0.5000
N0200 X0.2973 Y4.3145
N0210 Z0.0000 -------------------------------------------This is where i don’t need this line of code
N0220M03
N0230 G02 X0.1550 Y4.5000 I0.0497 J0.1855
N0240 X0.1550 Y4.5000 I0.3450 J0.0000
N0250 X0.1906 Y4.5464 I0.0480 J0.0000
N0260 M05
N0270 G00 Z0.5000
N0280 X4.2973 Y4.3145
N0290 Z0.0000 -------------------------------------------This is where i don’t need this line of code
N0300M03
N0310 G02 X4.1550 Y4.5000 I0.0497 J0.1855
N0320 X4.1550 Y4.5000 I0.3450 J0.0000
N0330 X4.1906 Y4.5464 I0.0480 J0.0000
N0340 M05
N0350 G00 Z0.5000
N0360 X4.2973 Y0.3145
N0370 Z0.0000 -------------------------------------------This is where i don’t need this line of code
N0380M03
N0390 G02 X4.1550 Y0.5000 I0.0497 J0.1855
N0400 X4.1550 Y0.5000 I0.3450 J0.0000
N0410 X4.1906 Y0.5464 I0.0480 J0.0000
N0420 M05
N0430 G00 Z0.5000
N0440 X-0.1723 Y4.9355
N0450 Z0.0000 -------------------------------------------This is where i don’t need this line of code
N0460M03
N0470 G02 X-0.0300 Y4.7500 I-0.0497 J-0.1855
N0480 G01 Y0.2500
N0490 G03 X0.2500 Y-0.0300 I0.2800 J0.0000
N0500 G01 X4.7500
N0510 G03 X5.0300 Y0.2500 I0.0000 J0.2800
N0520 G01 Y4.7500
N0530 G03 X4.7500 Y5.0300 I-0.2800 J0.0000
N0540 G01 X0.2500
N0550 G03 X-0.0300 Y4.7500 I0.0000 J-0.2800
N0560 G02 X-0.0656 Y4.7036 I-0.0480 J0.0000
N0570 M05
N0580 G00 Z0.5000
N0590 M05 M30

I guess i could set the pierceHeight to match my Rapid clearence it might work,just thinking about it now,but not sure.
So will you need to make a new post,or is there one i can use that will work,i figured you would know the best.
This machine is going to Egypt so i need it to work perfect here before i ship it.
Thanks Les

Erik Pecchi




----- Original Message -----
From: Leslie Newell
To: sheetcam@yahoogroups.com
Sent: Friday, April 13, 2007 5:56 PM
Subject: Re: [sheetcam] Re: G28.1 problems THC300 setup Mach3


I have to admit I also think probe is better than home. Home should be
for the machine’s physical limits, not the position of the work.
Probably very few people bother to use soft-limits. Without soft-limits
it doesn’t really matter where the Z home is. ISTR that the earlier THC
posts did use probe but there were reliability problems. It may well be
that the problems have now been solved with the later versions of Mach.

You should either use a Mach M03 macro to do the probe and use a non-THC
post or let SheetCam take care of all of the work. Trying to mix the two
is likely to cause more problems than it solves.

Erik, if you work out the correct G-code sequence for a probe-zero
cycle, I’ll write a post that will generate it for you. I can’t test the
code myself as I don’t have THC. In fact my plasma isn’t even working at
the moment…

Les

Erik wrote:

Yes im using the latest version of Mach3,I think my problem is with
the g28.1 routine which is a reference home command,i don’t see how
this would ever work for someone!From what i got from it,is that it
moves a axis toward the ref switch,and sets the machine cords to o.oo
so if i set my z axis up so it homes toward the table(which is wrong)
this will go down and touch off the plate and then next line of code
set 0.00 it would kinda work ,but now the machine mech limits are
ref off of the plate surface and not the physical min and max
travels of the that axis.This way seems all wrong and the g31 probe
comand should be the way to go,but i will have to find the right
post processor for sheetcam to add the right m03,m05 to the code in
the right place,and change the m03 in thc300 folder for the code
from bob cambells pdf,but there is the problem i can’t find that m03
file anywhere ,can anyone help me on this,I got a headache from this
one,looking at the code in the pdf its all wrong and looks like it
won’t work there is (wendif),
I would think i’m not the only person running the THC300 kit and the
THC300 setup files,But bob’s Websits is missing the m03 file for
everything to work,and the sheetcam post processor also to work
along with the m03.

Any help would be nice.

Thanks Erik


[Non-text portions of this message have been removed]

11

Sorry Everyone I wanted this to go to Les himself,and not the group.

Thanks Erik


[Non-text portions of this message have been removed]

12

Hi Erik,

The pierce height is hard-coded. You have two options:

  1. Take all Z moves out of the post. Mach must then control the Z axis.
    To do this you need to modify the M5 macro to move the Z to clearance
    height. You also need to set up the init string to move Z to clearance
    height. To do this, look in the post for lines like this:
    modalnumber (" Z", endz * scale, “0.0000”)
    and remove them. You will also need to take out the two Z moves from
    function pendown(). They look something like this:
    modaltext (" G00")
    modalnumber (" Z", cutheight * scale, “0.0000”)
    Most commercial plasma cutters work this way. The only disadvantage of
    this method is that you cannot use ramped leadins. Ramped leadins can
    improve tip life with thicker material.

  2. Ignore any move where z <= 0 (plasma should never go below Z=0).
    In function pendown() remove change two lines:
    modaltext (" G00")
    modalnumber (" Z", pierceheight * scale, “0.0000”)
    to
    if(pierceheight <=0) then
    modaltext (" G00")
    modalnumber (" Z", pierceheight * scale, “0.0000”)
    end

In function move() change this line:
modalnumber (" Z", endz * scale, “0.0000”)
to:
if(endz <=0) then
modalnumber (" Z", endz * scale, “0.0000”)
end

Posts are written in Lua <www.lua.org>. They do have an on-line manual
but it can be hard going in places. In SheetCam’s posts directory is a
file called Post processor.rtf. This file documents the SheetCam
extensions to Lua.

If you modify a post, give it a different name otherwise it will get
overwritten if you update SheetCam.

Les



pfauto wrote:

Now here is another thing that i need to get resolved,Since i don’t need SheetCam to worry about the Piercedelay,EndDelay,CutHeight,or PierceHeight,I’m not sure what post to use so i’m starting with the simplest one mach2plasma.post, How can i get rid of the PierceHeight when using the Mach2.Post,Running this post it inserts the PierceHeight of 0.00 which makes the torch go to the surface,then it runs the M03,Here is a example from the mach2 plasma .Post,not sure if this is where it is or not to be looking?

13

— In sheetcam@yahoogroups.com, “Erik” <pfauto@…> wrote:

Hi Les,

I agree with you on all those points,another thing is for it to work
the way Tom says the G28.1 way,i would have to set up my z axis in
Mach3 to Ref home toward the table,So when i first turn on my machine
in the morning or after last shift had it running ,I would hit ref
all axis under mach and the z would move toward the table and go into

I fixed all of that by just removing the “Home All” button on our
screens and putting in a custom button called “Ref XY”. It just does a
reference move to the XY homes and leaves the Z where it is (normally
parked at the rapid clearance height) I also have another button
called “Load Material” that moves the machine to a preset XYZ location
to load material.

In over four years of plasma cutting on my table with no far limits I
have never banged the top of my Z. Since I have a 6 inch stroke and
all my cutting is done in the first 1" of travel, nothing in my code
ever lifts it more than 1" above the reference height on Z (top of
material).

We advise operators to manually reference each axis individually at
machine startup. (using the REF buttons we put next to each DRO) If
they really want to ref Z it needs to be with a piece of material on
the grid

Since the very first move in the code using the SheetCAM THC post is
to move to the first pierce point and establish the top of material I
never worry about where Z “thinks” it is as long as I can look at the
table and determine it’s some distance above the table.

Soft limits are nice but they only work if you have them enabled in
MACH…yet another setting the operator has to confirm. They can get
turned off easily and then you have no software protection.

Putting all of the parameters in MACH3 for pierce delay, Pierce
height, Cut height, etc that are normally embedded in the g-code by
SheetCAM forces the operator to check more things before the cut and
have a higher technical understanding of what all those parameters
mean. Heck, I sometimes forget to readjust my cut current after
switching material and tips ! There are enough parameters to check to
get a good cut without having to put in new values in DRO’s.

I guess a lot of this has to do with the fact my approches are done
from a practical standpoint having cut miles of steel in the last 5
years using both the THC300 and MP1000-THC in a small shop
environment, and seeing just about everything screw up that can.

I will say this from experience: If you come up with a system that
uses special macros in MACH your support issues WILL increase. Combine
that with screens and custom DRO’s, and you setup an environment where
confusion will reign. If you then make it so they have to have the
macro AND a custom post in SheetCAM for MACH, your support issues with
increase exponentially.

As one of the primary support persons for the THC300 and MP1000-THC
units I will openly state that anyone that wants to use Erik’s custom
macro needs to direct any support issues to him.

Tom Caudle
www.CandCNC.com

14

Tom Wrote "
In over four years of plasma cutting on my table with no far limits I
have never banged the top of my Z. Since I have a 6 inch stroke and
all my cutting is done in the first 1" of travel, nothing in my code
ever lifts it more than 1" above the reference height on Z (top of
material)."

Do you have Softlimits turned on on your machine?
Does anyone else ever run your machine?
If so how do they know where the physical limits of the machine are if you don’t use softlimits?

“We advise operators to manually reference each axis individually at
machine startup. (using the REF buttons we put next to each DRO) If
they really want to ref Z it needs to be with a piece of material on
the grid”

I agree homing at start up is very important!

“Since the very first move in the code using the SheetCAM THC post is
to move to the first pierce point and establish the top of material I
never worry about where Z “thinks” it is as long as I can look at the
table and determine it’s some distance above the table.”

Using it the way I do ,I push the Default RefAllButton,and my Z moves up away from the table Ref’s itself and then on to the other Axis left
The M03 when used finds the top of the plate.


“Soft limits are nice but they only work if you have them enabled in
MACH…yet another setting the operator has to confirm. They can get
turned off easily and then you have no software protection.”

That’s why I want to use them on my machine!

“Putting all of the parameters in MACH3 for pierce delay, Pierce
height, Cut height, etc that are normally embedded in the g-code by
SheetCAM forces the operator to check more things before the cut and
have a higher technical understanding of what all those parameters
mean. Heck, I sometimes forget to readjust my cut current after
switching material and tips ! There are enough parameters to check to
get a good cut without having to put in new values in DRO’s.”

I agree this is not a good idea either,What would be nice,if some how SheetCam could set up the correct DRO’s when a file is loaded then the user could make a adjustment if needed,as the tips wear out or whatever chanded the cut Quality,Or is this what scale in the post processor does under mach does it overide the settings by a percentage?

“As one of the primary support persons for the THC300 and MP1000-THC
units I will openly state that anyone that wants to use Erik’s custom
macro needs to direct any support issues to him.”

As I stated I din’t want to send this to the group ,It was intended for only Les to get it,I’m not here trying to promote anyone to use my approach.

I know what would solve all these problems if Mach3 when using the G28.1 ,there was Check Box ,under General Config,to set the G28.1 Probe direction,seems all my issues would go away ,There is a checkBox for G28.1 No Intial Move,but I didn’t find any reading meterial on it in the manual or a good search on the forum I’m sure it is there somewhere in the forum’s burried in posts.

Hope I get this all fixed soon,I need to ship this machine,at least now I have two ways they can choose to run the machine the way they want.

Thanks Erik

[Non-text portions of this message have been removed]

15

Hi Erik,

I agree this is not a good idea either,What would be nice,if some how SheetCam could set up the correct DRO’s when a file is loaded then the user could make a adjustment if needed,as the tips wear out or whatever chanded the cut Quality,Or is this what scale in the post processor does under mach does it overide the settings by a percentage?

As far as i know there is no way to transfer numbers from g-code to a
Mach DRO. If there is then a post could be written to do it.

As I stated I din’t want to send this to the group ,It was intended for only Les to get it,I’m not here trying to promote anyone to use my approach.

To be honest, I prefer it to remain on the group. Discussions like this
help stimulate new ideas.

Les

16

As far as I know there is no way to transfer numbers from g-code to a
Mach DRO. If there is then a post could be written to do it.



Les

Hi Les,
Just reaching on this one…But,Could SheetCam be able to change
the .XML file for Mach3,Then for those DRO’s or anything I guess, when
mach Mach3 is started up,having persistent DRO’s checked those
settings will be there,and I think even if they are not checked the
UserDRO’s will stay what you set them for,Just a thought,but I could
see problems with this,unless The user Selected Say A SheetCam.xml
file from the Mach3 Startup window and those current settings were in
that .XML file this way ,the last file processed through sheetcam was
the current settings in the SheetCam .XML file.

I wonder if Art could make the G28.1 Routine have a check box for
making the Z axis travel in the other direction,I see under Ports&Pins
there is a checkbox for No Initial Move,This way I could keep
softlimits on and all my problems would go away,I would like to have
SheetCam set the settings,as I have a possible customer wanting to use
the Hypertherm 260 which has automatic settings of the amps
pressure,gas and other feature.
Thanks Erik

Thanks Erik

17

Hi Erik,

Messing about with Mach’s xml file is potentially dangerous. However,
thinking about it, you can set variables with G-code. You can also read
those variables from Mach macros. It would be possible to set a bunch of
variables then trigger a custom M-code macro to transfer those variables
to DROs or to use them directly. It would be messy but it would work.

Les

Erik wrote:

Hi Les,
Just reaching on this one…But,Could SheetCam be able to change
the .XML file for Mach3,Then for those DRO’s or anything I guess, when
mach Mach3 is started up,having persistent DRO’s checked those
settings will be there,and I think even if they are not checked the
UserDRO’s will stay what you set them for,Just a thought,but I could
see problems with this,unless The user Selected Say A SheetCam.xml
file from the Mach3 Startup window and those current settings were in
that .XML file this way ,the last file processed through sheetcam was
the current settings in the SheetCam .XML file.

I wonder if Art could make the G28.1 Routine have a check box for
making the Z axis travel in the other direction,I see under Ports&Pins
there is a checkbox for No Initial Move,This way I could keep
softlimits on and all my problems would go away,I would like to have
SheetCam set the settings,as I have a possible customer wanting to use
the Hypertherm 260 which has automatic settings of the amps
pressure,gas and other feature.
Thanks Erik

18

— In sheetcam@yahoogroups.com, “pfauto” <pfauto@…> wrote:

Tom Wrote "
In over four years of plasma cutting on my table with no far limits I
have never banged the top of my Z. Since I have a 6 inch stroke and
all my cutting is done in the first 1" of travel, nothing in my code
ever lifts it more than 1" above the reference height on Z (top of
material)."

Do you have Softlimits turned on on your machine?

Nope

Does anyone else ever run your machine?

Yes. In fact most of the jobs are now run by a couple of part timers

If so how do they know where the physical limits of the machine are

if you don’t use softlimits?

I take them by the hand and show them the top of the rails and say
“Don’t raise the head that far or an alarm will go off and you will
receive a painful shock” Since the Z is a stepper and there are hard
stops all it really does is just stall.

Since Sheetcam knows where the table limits are it won’t write code
that will go past the stops so the only way it could happen is if an
operator jogs it all the way.

If I am concerned about safety and far limits I hook up separate
limits and make them turn off the power to the motors. That in fact
is a single connection in any of the controllers we build.


“We advise operators to manually reference each axis individually at
machine startup. (using the REF buttons we put next to each DRO) If
they really want to ref Z it needs to be with a piece of material on
the grid”

I agree homing at start up is very important!

“Since the very first move in the code using the SheetCAM THC post is
to move to the first pierce point and establish the top of material I
never worry about where Z “thinks” it is as long as I can look at the
table and determine it’s some distance above the table.”

Using it the way I do ,I push the Default RefAllButton,and my Z

moves up away from the table Ref’s itself and then on to the other
Axis left

RefAllButton is a no-no in plasma cutting. The button is removed
(just like the Go Home button) from our screens. The custom button
that does the referencing is my “RefXY” button. We even put that in
our Hand controller as a button for the THC. It does not move the Z
on a reference move. On my router (that has no Z home switch) I just
have it lift the head 1" THEN ref XY.

The M03 when used finds the top of the plate.


“Soft limits are nice but they only work if you have them enabled in
MACH…yet another setting the operator has to confirm. They can get
turned off easily and then you have no software protection.”



That’s why I want to use them on my machine!

So the operator can forget and crash the machine thinking they are
protected? hummmmm…

“Putting all of the parameters in MACH3 for pierce delay, Pierce
height, Cut height, etc that are normally embedded in the g-code by
SheetCAM forces the operator to check more things before the cut and
have a higher technical understanding of what all those parameters
mean. Heck, I sometimes forget to readjust my cut current after
switching material and tips ! There are enough parameters to check to
get a good cut without having to put in new values in DRO’s.”

I agree this is not a good idea either,What would be nice,if some

how SheetCam could set up the correct DRO’s when a file is loaded then
the user could make a adjustment if needed,as the tips wear out or
whatever chanded the cut Quality,Or is this what scale in the post
processor does under mach does it overide the settings by a percentage?

None of the parameters involved except possibly feedrate (which you
can override while cutting), and the tip volts on the THC (which also
can be adjusted on the fly) have a lot of effect on cut quality.
Definitely not the pierce height, delay or initial cut height. Those
numbers should not be “messed” with by an unskilled operator. By the
time a tip wears out enough to cause problems with cut quality, you
better replace it because shortly you will hear a “snark” sound and
the machine starts gouging a trench in the top of the metal with no
penetration. Then you have to stop the machine. Replace consummables,
possibly re-reference the XY and then crawl back through the G-code
and restart the cut (and turn off the THC in MACH so the tip won’t
dive into the existing kerf!)


“As one of the primary support persons for the THC300 and MP1000-THC
units I will openly state that anyone that wants to use Erik’s custom
macro needs to direct any support issues to him.”

As I stated I din’t want to send this to the group ,It was intended

for only Les to get it,I’m not here trying to promote anyone to use my
approach.


I know what would solve all these problems if Mach3 when using the

G28.1 ,there was Check Box ,under General Config,to set the G28.1
Probe direction,seems all my issues would go away ,There is a checkBox
for G28.1 No Intial Move,but I didn’t find any reading meterial on it
in the manual or a good search on the forum I’m sure it is there
somewhere in the forum’s burried in posts.

Hope I get this all fixed soon,I need to ship this machine,at least

now I have two ways they can choose to run the machine the way they want.

Thanks Erik

With all due respect the machine could have been shipped 2 weeks ago
if the time spent re-engineering a process that already works was
instead focused on building the machine and not writing a bunch of
custom macros and modifying the posts.


Most shops don’t hire Rhodes Scholars to run a dirty smokey plasma
cutter. The more variables you hand them, the more they will try, and
the more often your phone will ring. So instead of changing a tip
when it starts to show signs of wear, they will try to get more time
from a worn tip and dink with adjustments. I have considered removing
the Feedrate override on some installs just to eliminate one more
variable (:-o

19

Not to bring back an old dead thread, but i have been using g28.1 for z referencing for a long time and it has worked great. I understand both of your guys point of views, although, now i have a reason for maybe changing if possible and keeping the machine coordinates (z in particular) to an exact non changing location.

My machine has 3.5" - 4" of z travel above the table depending on the tip used and placement of the torch in the holder. I have added a rotary tube attachment to the table, and even though it is sunk into the table, 1/2 of the tube + approx 1.25" is above Flat sheet cut height. This means that to cut 5" tube, i would have .25" available z height above it. If i am cutting larger tube and the rapid is set too high, or Sheetcam puts in a clearance height above what is available for square tube, it will stall out and then provide inaccurate z position when it travels back down to reference or continue cutting.

Also i would like to add to the go home feature to have the z retract to as high as possible.

This would make the safe z much more useful also as it would be the uppermost extent of the travel in machine coordinates, period.

These reasons are why i am looking into how to reference my z to the cut surface without affecting my machine coordinates, so i can implement the soft limits and z go to home.

I am familiar with g28.1 as i have been using it a long time. Is the G31 something that i can use instead without complicating things terribly or loosing use of other valuable features. Also, would i be able to use the same switch circuit (multiple switches wired to 1 input) for the z referencing and the plate referencing (if G31) My Post Processor is already massively customized for both flat sheet and rotary cutting.

Just looking for a little input from others in the know with this.

Brian