sensing program zero

dunno if flashcut is still alive but anyway, i made some gcode to find XYZ stock origin using a touchprobe #ProbeSize should be set in the variables menu to the diameter of the probe tip

bring the probe tip to within .5/.5/.5 of the edges to check for, set program to zero, run this gcode. it'll end up at 0,0,.2 , setting the tool length of the probe makes it effective 0, i thought about adding a tool change at the top to a preset tool for the probe in the library.

I7 is the probe line, change for your setup. i ran it about 30 times in a row and i was getting around .0001 or better repeat-ability, also i did notice that the FlashCut Relative XYZ DRO has a math error, if you reset it to 0,0,0 and then keep running and resetting the program original it'll drift over by around .0001 each run) strange stuff.

It searches Z down, X - to X+ then Y+ to Y-

Quote:

---

(Switch to imperial)
G20
(Go to Program Z0)
G01Z0F5
(Go to Program X0Y0)
G01Y0X0F5
(search z for .5" at feed rate of 1) input line 7
G31 Z-.5 I7 S1 E0 F1
(Program.Z is ?)
(set Program Z to 0, with compensation)
G92 Z#ProbeSize/2
(Dwell .5 second)
G04 P.5
(Move to Program.Z.1 above part)
G01Z.1F5
(Move to Program.X-.3)
G01X-.3F5
(Move to Program.Z-.03 below part , maybe use ball size?)
G01Z-.03F1
(search X for .5" at feed rate of 1) input line 7
G31 X.5 I7 S1 E0 F1
(set Program X to 0, with compensation)
G92 X-#ProbeSize/2
(Dwell .5 second)
G04 P.5
(move away from part in X)
G01 X-.2F5
(Move to Program.Y.4, still below part in Z)
G01 Y.4F5
(move into part on X, z is below top)
G01 X.1F5
(search Y for -1" at feed rate of 1) input line 7
G31 Y-1 I7 S1 E0 F1
(set Program Y to 0, with compensation)
G92 Y#ProbeSize/2
(Dwell .5 second)
G04 P.5
(move above part)
G01Z.2F5
(move over corner)
G01X0Y0F5

---

G92 Z#ProbeSize/2 should be G92 Z#0 if you're measuring the over all length of the touch probe and not removing half the size of the ball.

I was just wondering if anyone had done this for FC, thanks.

Quote:

---

Originally Posted by Fastest1

I was just wondering if anyone had done this for FC, thanks.

---

I have made similar routines over the years and use them with Flashcut........ I'd have to look at them to see what methods I used, but I would assume they would look similar to the OP's.

Anything for center finding?

Quote:

---

Originally Posted by datac

I have made similar routines over the years and use them with Flashcut........ I'd have to look at them to see what methods I used, but I would assume they would look similar to the OP's.

---

i did a corner finding one, center of a hole and a few others i'll post when i get home.

Code:

---

N100 GLOBAL REAL #XC #YC #ZC
N102 GLOBAL REAL #PX #PY #PX1 #PY1 #PX2 #PY2 #CX #CY #RAD #STEP
N103 GLOBAL REAL #DXDY
N103 GLOBAL REAL #DXDY1

N104 (Switch to imperial)
N106 G20

N108 (switch to the touch probe, set your tool as needed)
N110 M06 T100

N112 (Go to Program X0Y0)
N114 G01Y0X0F5

N116 G31 X-1 I7 S1 E0 F1

N118 G01 X#Program.X/2 Y0 F5

N122 (search Y axis to -1 at feed rate of 1 input line 7)
N124 G31 Y-1 I7 S1 E0 F1

N126 (First point is Program.X.Program.Y)
N128 #PX = #Program.X
N130 #PY = #Program.Y

(N131 M00 #PX & " " & #PY

N132 (Step back slightly to take probe off surface)
N133 G01 X#Program.X/3 Y#Program.Y/2 F5

N138 (search Y axis to 2 at feed rate of 1 input line 7)
N140 G31 Y.5 I7 S1 E0 F1

N142 (Second point is Program.X.Program.Y)
N144 #PX1 = #Program.X
N146 #PY1 = #Program.Y

(N147 M00 #PX1 & " " & #PY1

N149 G01 X#PX/3 Y#Program.Y/3 F5

N154 (search X axis to 2 at feed rate of 1 input line 7)
N156 G31 X2 I7 S1 E0 F1

N158 (Third point is Program.X.Program.Y)
N160 #PX2 = #Program.X
N162 #PY2 = #Program.Y

(N163 M00 #PX2 & " " & #PY2

N164 (Go to Program X0Y0)
N166 G01Y0X0F5

IF [#PX1 - #PX] = 0 THEN
#PX1  = #PX1 + 0.0001
ENDIF

IF [#PX2 - #PX1] = 0 THEN
#PX2  = #PX2 + 0.0001
ENDIF

IF [#PY1 - #PY] = 0 THEN
#PY1  = #PY1 + 0.0001
ENDIF

IF [#PY2 - #PY1] = 0 THEN
#PY2  = #PY2 + 0.0001
ENDIF


#DXDY = [#PY1 - #PY] / [#PX1 - #PX]

N174 #DXDY1=[[#PY2]-[#PY1]]/[[#PX2]-[#PX1]]

(M00 #DXDY & " " & #DXDY1

IF [#DXDY1 + #DXDY] = 0 THEN
M00 "Either lines are on same coord or too small area"
ENDIF

N176 #CX=[[[#DXDY]*[#DXDY1]]*[[#PY]-[#PY2]]+[[#DXDY1]*[[#PX]+[#PX1]]]-[[#DXDY]*[[#PX1]+[#PX2]]]]/[[2.]*[[#DXDY1]-[#DXDY]]]
N178 #CY=[[-1.]/[#DXDY]]*[[#CX]-[[#PX]+[#PX1]]/[2.]]+[[#PY]+[#PY1]]/[2.]

(N180 #RAD=[SQRT[[[[#PX1]-[#CX]]*[[#PX1]-[#CX]]]+[[[#PY1]-[#CY]]*[[#PY1]-[#CY]]]]]*[2.]

N182 M00 #CX & " " & " " & #CY & " " & #RAD
N183 M00 #PX & " " & #PY & "; " & #PX1 & " " & #PY1 & "; " & #PX2 & " " & #PY2

N184 M00

---

Code:

---

(Probe Left/Back set as program zero, move to Right/Front, set program zero to half/current position)

GLOBAL REAL #XWidth
GLOBAL REAL #YWidth

GLOBAL REAL #XCenter
GLOBAL REAL #YCenter

GLOBAL STRING #Message

#XWidth = 0
#YWidth = 0

#XCenter = 0
#YCenter = 0

(Switch to imperial)
G20
M06 T100

(Go to Program Z0)
G01Z0F5

(Go to Program X0Y0)
G01Y0X0F12

(search z for .5" at feed rate of 1) input line 7
G31 Z-.5 I7 S1 E0 F1

(Program.Z is ?)
(set Program Z to 0, no compensation since its the bottom of the probe, not the middle)
G92 Z0

(Dwell .1 second)
G04 P.1

(Move to Program.Z.1 above part)
G01Z.1F20

(Move to Program.X-.3, since origin is rough)
G01X-.3F20

(Move to Program.Z-.03 below part , maybe use ball size + ?)
G01Z-.07F20

(fast search X for .5" at feed rate of 6) input line 7
G31 X.5 I7 S1 E0 F5

(quickly step back a tad)
G01 X#Program.X - .1F20

(slow search X for .5" at feed rate of 1) input line 7
G31 X.15 I7 S1 E0 F1

(set Program X to 0, with compensation)
G92 X-#Probe1SizeL/2

(move away from part in X)
G01 X-.2F20

(Move to Program.Y, still below part in Z)
G01 Y.2F20

(move into part on X, z is below top)
G01 X.1F20

(fast search Y for -1" at feed rate of 6 input line 7 )
G31 Y-1 I7 S1 E0 F6

(move back away from part)
G01 Y#Program.Y + .1 F12

(slow search Y for .15" at feed rate of 1 input line 7 )
G31 Y-.15 I7 S1 E0 F1

(set Program Y to 0, with probe ball compensation)
G92 Y#Probe1SizeL/2

(move back away from part)
G01 Y#Program.Y + .1 F12

(move above part)
G01Z.2F20

(move over RoughX,RoughY guessed size of box at F5)
G01 X#RoughX Y-#RoughY/2 F40

(move down to below edge of part)
G01Z-.07F20

(fast search for X2, search for -1 in X)
G31 X-1 I7 S1 E0 F6

(move out a tad)
G01 X#Program.X + .1 F12

(slow search)
G31 X-.2 I7 S1 E0 F1

( size of object in X , these fail when not in simulator mode)
#XWidth = #Program.X - #Probe1SizeL/2
#XCenter = #XWidth/2

(move away from x in positive direction)
G01 X#Program.X + .2 F12

( this moves XY and Z for some reason in simulator? )
G01Z.2F20

(Move to Program.Y-.4, still below part in Z)
G01 X#RoughX/2 Y-#RoughY F40

(move into part on X, z is below top)
G01Z-.07F12

(search Y for 1" at feed rate of 6 input line 7)
G31 Y.1 I7 S1 E0 F6

G01 Y#Program.Y-.1 F12

(search Y for 1" at feed rate of 1 input line 7)
G31 Y.1 I7 S1 E0 F1

( size of object in Y  - #Probe1SizeL/2)
#YWidth = #Program.Y + #Probe1SizeL/2

(away from part)
G01 Y#Program.Y - .1F12

#YCenter = #YWidth/2

(move z above part)
G01Z.2F12

G01 X#XCenter Y#YCenter F40

(update screen)
#XWidth1 = #XWidth
#YWidth1 = #YWidth

---

rectangle center

i remoted in and pulled them off the cnc machine, but i'll add notes when i can

Code:

---

GLOBAL REAL #PX #PY #PX1 #PY1
GLOBAL REAL #CX #CY

(Switch to imperial)
G20

(switch to the touch probe, set your tool as needed)
M06 T100

(Go to Program X0Y0)
G01Y0X0F5

G31 X-1 I7 S1 E0 F1
#PX = #Program.X
G01 X#Program.X+0.08 F1

G31 Y-1 I7 S1 E0 F1
#PY = #Program.Y

G01 Y#Program.Y+0.08 F1

G31 Y.5 I7 S1 E0 F1
#PY1 = #Program.Y

G01 Y#Program.Y-0.08 F1

G31 X2 I7 S1 E0 F1
#PX1 = #Program.X

G01Z.2F5

M00 #PX & " " & #PY  & #PX1 & " " & #PX1


#CX = #PX1 - #PX
#CY = #PY1 - #PY 

#CX = #CX /2
#CY = #CY /2

#CX = #PX + #CX
#CY = #PY + #CY

G01 X#CX Y#CY

M00 #CX & " " & #CY

---

Quote:

---

Originally Posted by Fastest1

Anything for center finding?

---

Below is what I use for center finding... note that I have one on the machine that runs this twice in a row for holes. Doing it twice gave me more assurance and accuracy. Also note, you need to install the #ProbeSize reference and Probe Diameter in the Variables Table.

------------------------------------

(Probe Hole Center - Tested)
(X-Y Center Hole Probe Routine)
(Start program in center area of opening, .050 Down Z into Hole)
(Seek travel distance is 2" in each axis - adjustable in G31 lines below)
(#ProbeSize is set in Variables)
G90
G20
G01 X0 Y0 Z0 F8
(Find X Center)
G31 X-2 I1 S1 E0 F8
G92 X0.0
G01 X#ProbeSize / 2 F8
/G04 P.2
G31 X2 I1 S1 E0 F8
#x1 = #Program.X
#xc1 = #x1 / 2
/G04 P.2
G1 X#xc1 F8
G92 X0.0
(Find Y Center)
G31 Y-2 I1 S1 E0 F8
G92 Y0.0
G01 Y#ProbeSize / 2 F8
/G04 P.2
G31 Y2 I1 S1 E0 F8
#y1 = #Program.Y
#yc1 = #y1 / 2
/G04 P.2
G1 Y#yc1 F8
G92 Y0.0
G01 Z0.200
G92 Z0
M00 "Remember to set Z Zero for tooling"
M99

-------------------------------------------------------------------

Though it could definitely be user error. I get an error in FC before even starting with this code. I did edit it to be the correct input line. The probe diameter is set in my touch probe settings. Is there something else I am missing? I am having some luck with charliex's

Quote:

---

Originally Posted by datac

Below is what I use for center finding... note that I have one on the machine that runs this twice in a row for holes. Doing it twice gave me more assurance and accuracy. Also note, you need to install the #ProbeSize reference and Probe Diameter in the Variables Table.

------------------------------------

(Probe Hole Center - Tested)
(X-Y Center Hole Probe Routine)
(Start program in center area of opening, .050 Down Z into Hole)
(Seek travel distance is 2" in each axis - adjustable in G31 lines below)
(#ProbeSize is set in Variables)
G90
G20
G01 X0 Y0 Z0 F8
(Find X Center)
G31 X-2 I1 S1 E0 F8
G92 X0.0
G01 X#ProbeSize / 2 F8
/G04 P.2
G31 X2 I1 S1 E0 F8
#x1 = #Program.X
#xc1 = #x1 / 2
/G04 P.2
G1 X#xc1 F8
G92 X0.0
(Find Y Center)
G31 Y-2 I1 S1 E0 F8
G92 Y0.0
G01 Y#ProbeSize / 2 F8
/G04 P.2
G31 Y2 I1 S1 E0 F8
#y1 = #Program.Y
#yc1 = #y1 / 2
/G04 P.2
G1 Y#yc1 F8
G92 Y0.0
G01 Z0.200
G92 Z0
M00 "Remember to set Z Zero for tooling"
M99

-------------------------------------------------------------------

---

Btw, Thank You both. I am going to be enjoying this machine soon.

Quote:

---

Originally Posted by charliex

G92 Z#ProbeSize/2 should be G92 Z#0 if you're measuring the over all length of the touch probe and not removing half the size of the ball.

---

No matter what I do this doesnt work for me. Can you elaborate on the use of G92 Z#0 instead of Z#ProbeSize/2 ?

not sure what you mean, so i'll assume and make eli5 notes,ProbeSize is the size of the ball of the touch probe itself, so typically what you want in 3d probing is the center of the ball not the outside edge,s o half the width is the center.

in flashcut if you define the variable ProbeSize to the width of the ball , then the existing code will set the offset to the probed position with the half the width of the ball, so again the center of the ball, if set to 0 then it wont compensate for the size of the probe ball, and when it touches the object, the point where the probe contacts the surface will become the actual program Z offset, same for any axis using the probe.

Typically you'd want to predefine ProbeSize in the flashcut variables screen to the measured width of the probe tip. i'll post a screenshot of my setup when i get home if it helps, or if misunderstood what you were asking let me know!


cheers

My probes physical tip is .1570" in diameter. The tool length offset is 3.3999". I have the tip size entered for tool 10 in my case.
Any pictures will help.

Quote:

---

Originally Posted by Fastest1

My probes physical tip is .1570" in diameter. The tool length offset is 3.3999". I have the tip size entered for tool 10 in my case.
Any pictures will help.

---

add it like this

First, Thank you so much for answering and the quickness was unexpected. I am assuming the first 4 values in the user variables applies to this conversation. There are 4 you have listed and not knowing the diameter of your probe it is ignorant to assume. What are the 4 different variables?
I see
#ProbeSize
#ProbeSizeL
#ProbeSize1
#ProbeSize1L
I am at a loss for the 4 different boxes.
I do understand where to enter them ;-) Just not why or what they represent.
#

Quote:

---

Originally Posted by charliex

add it like this

---

CharlieX, Thanks again.
Ended up using only the #ProbeSize, selected Real and added the probes tip diameter .1570. It seems to be working well.
Copied a few of the macros off of this thread and get mixed results. Mostly the probe is either probing an incorrect direction or sequence than I need.
I will look into modifying them for my use or understanding.
Funny that FC has program sensing but wont allow different settings on each axis simultaneously.
At least I did realize I could select X & Y and positive direction of travel to probe at the same time ;-)

I spoke too soon. Though I have a much better work around than I did. I still dont understand the user variables well enough.

i have two touch probes, and they have different attachments for the end ball, one small, one large ball. so there are two sets of variables for each of the probes, you only need the first one


i assume the setup of our machines is similar for axis direction :)

Charlie, I hope you are still monitoring this ;-) Should I delete the second probe in my user variables? Or is there harm in having both listed but no values on the second one?
I have copied and pasted all of the gcodes and macros I have seen here but nothing works as a center finder. I wonder if there are user variables that I am not filling in properly? In regards to the files for different probing routines, are these only kept as a gcode or is there a way to install them as routines or selections from the FC pages?

Quote:

---

Originally Posted by charliex

add it like this

---

Is this the center finding routine?
If so when I run it, there is a dialog box at the end of the process that shows 2 different decimals.
They appear to be the amounts of correction needed in the X and then Y axis to be at dead center.
Can anyone verify this?

Quote:

---

Originally Posted by charliex

Code:

---

N100 GLOBAL REAL #XC #YC #ZC
N102 GLOBAL REAL #PX #PY #PX1 #PY1 #PX2 #PY2 #CX #CY #RAD #STEP
N103 GLOBAL REAL #DXDY
N103 GLOBAL REAL #DXDY1

N104 (Switch to imperial)
N106 G20

N108 (switch to the touch probe, set your tool as needed)
N110 M06 T100

N112 (Go to Program X0Y0)
N114 G01Y0X0F5

N116 G31 X-1 I7 S1 E0 F1

N118 G01 X#Program.X/2 Y0 F5

N122 (search Y axis to -1 at feed rate of 1 input line 7)
N124 G31 Y-1 I7 S1 E0 F1

N126 (First point is Program.X.Program.Y)
N128 #PX = #Program.X
N130 #PY = #Program.Y

(N131 M00 #PX & " " & #PY

N132 (Step back slightly to take probe off surface)
N133 G01 X#Program.X/3 Y#Program.Y/2 F5

N138 (search Y axis to 2 at feed rate of 1 input line 7)
N140 G31 Y.5 I7 S1 E0 F1

N142 (Second point is Program.X.Program.Y)
N144 #PX1 = #Program.X
N146 #PY1 = #Program.Y

(N147 M00 #PX1 & " " & #PY1

N149 G01 X#PX/3 Y#Program.Y/3 F5

N154 (search X axis to 2 at feed rate of 1 input line 7)
N156 G31 X2 I7 S1 E0 F1

N158 (Third point is Program.X.Program.Y)
N160 #PX2 = #Program.X
N162 #PY2 = #Program.Y

(N163 M00 #PX2 & " " & #PY2

N164 (Go to Program X0Y0)
N166 G01Y0X0F5

IF [#PX1 - #PX] = 0 THEN
#PX1  = #PX1 + 0.0001
ENDIF

IF [#PX2 - #PX1] = 0 THEN
#PX2  = #PX2 + 0.0001
ENDIF

IF [#PY1 - #PY] = 0 THEN
#PY1  = #PY1 + 0.0001
ENDIF

IF [#PY2 - #PY1] = 0 THEN
#PY2  = #PY2 + 0.0001
ENDIF


#DXDY = [#PY1 - #PY] / [#PX1 - #PX]

N174 #DXDY1=[[#PY2]-[#PY1]]/[[#PX2]-[#PX1]]

(M00 #DXDY & " " & #DXDY1

IF [#DXDY1 + #DXDY] = 0 THEN
M00 "Either lines are on same coord or too small area"
ENDIF

N176 #CX=[[[#DXDY]*[#DXDY1]]*[[#PY]-[#PY2]]+[[#DXDY1]*[[#PX]+[#PX1]]]-[[#DXDY]*[[#PX1]+[#PX2]]]]/[[2.]*[[#DXDY1]-[#DXDY]]]
N178 #CY=[[-1.]/[#DXDY]]*[[#CX]-[[#PX]+[#PX1]]/[2.]]+[[#PY]+[#PY1]]/[2.]

(N180 #RAD=[SQRT[[[[#PX1]-[#CX]]*[[#PX1]-[#CX]]]+[[[#PY1]-[#CY]]*[[#PY1]-[#CY]]]]]*[2.]

N182 M00 #CX & " " & " " & #CY & " " & #RAD
N183 M00 #PX & " " & #PY & "; " & #PX1 & " " & #PY1 & "; " & #PX2 & " " & #PY2

N184 M00

---

---

yep its shows the difference

you can store both variables at once, mine looks like this

https://i.imgur.com/1wCXSJX.png

Thanks so much for the reply! In my case the Y seems to take a - number using the recommendation. I wonder if my Y is backwards?

or mine is :)

As long as the center is found. Thanks again.

Quote:

---

Originally Posted by Fastest1

As long as the center is found. Thanks again.

---

yep no worries, i've been using this script for a while now.. . working on an upgrade to one my other flashcut add ons at the moment too. hopefully i get somewhere with it this weekend.not sure how many FC people there are out there :)

Quote:

---

Originally Posted by charliex

yep no worries, i've been using this script for a while now.. . working on an upgrade to one my other flashcut add ons at the moment too. hopefully i get somewhere with it this weekend.not sure how many FC people there are out there :)

---

I know nothing about making the scripts or even how to install them other than loading GCode.
Mach was a little different and I could find screens and options, FC not so much ;-)
I would enjoy your sharing the one you are working on.
Also in the center finding one mentioned just above.
Why doesnt the measured error automatically correct in the DRO’s (if accepted)?
I just write them down or take a pic and enter the dimensions manually.
Am I missing a technique?
It seems I cant get any actions from the PC til I close that dialog box.



Sent from my iPhone using Tapatalk Pro