cncchipmaker
-
Posts
190 -
Joined
-
Last visited
-
Days Won
1
Content Type
Profiles
Forums
Downloads
Store
eMastercam Wiki
Blogs
Gallery
Events
Posts posted by cncchipmaker
-
-
We use a rotation macro at work. It depends on how your machine is set up. If you know trig and know how to manipulate your system variables you can create your own version.
-
Has anyone used one of the macros yet? I am just curious.
-
rpadyk please give this a try:
O3333(SPIRAL ROUGH ID POCKET)
(INCREMENTAL AND ABSOLUTE MACRO)
(MUST HAVE START HOLE IN CENTER)
(UNPROVEN)
(FORMAT G65/G66 QSTDRZEFV)
(Q = #17 - STEPOVER IN Z/ DOC)
(S = #19 - STEPOVER IN X/ PERCENTAGE)
(T = #20 - TOOL DIAMETER)
(D = #7 - PART INTERNAL DIAMETER)
(R = #18 - R PLANE)
(Z = #26 - Z START/ TOP OF STOCK)
(E = #8 - END OF POCKET IN Z)
(F = #9 - FEEDRATE)
(V = #22 - 1 FOR VARIABLE FEEDRATE, 0 = FIXED)
(*********************************)
(CALCULATE DOC IN Z)
#100=ABS[#26]-ABS[#8]
#100=ABS[#100]
IF[[#26*#8]GE0]GOTO1
#100=ABS[#26]+ABS[#8]
N1#101=ROUND[#100/#17]
#102=#100/#101
IF[#102GT[#100/2.]]THEN#102=#100
(CALCULATE DOC IN X)
#103=[#19*.01]*#20
#104=[#7/2.]-[#20/2.]
#105=ROUND[#104/#103]
#106=#104/#105
IF[#106GT[#104/2.]]THEN#106=#104
#107=#5001
#108=#5002
G0G90X#107Y#108
Z[#26+.1]
G1Z#26F#9
#109=#5003-#102
#116=3.14*[#106*2.]
#119=#9
#126=#106
WHILE[#101GT0]DO1
IF[#101EQ0]GOTO10
#101=#101-1.
G90G1Z#109F#119
G91G41X#106
G03I-[#106]
#105=#105-1.
#106=#106+#126
IF[#105EQ0]GOTO20
WHILE[#105GT0]DO2
IF[#105EQ0]GOTO20
#129=#119*[[3.14*[#106*2.]]/#116]
IF[#22EQ0]THEN#129=#119
G03X-[#106*2.]I-[#106]F#129
#105=#105-1.
#106=#106+#126
IF[#105EQ0]GOTO20
#129=#119*[[3.14*[#106*2.]]/#116]
IF[#22EQ0]THEN#129=#119
G03X[#106*2.]I#106F#129
#105=#105-1.
#106=#106+#126
END2
N20
IF[#5001LT#107]GOTO30
G03I-[#106]
GOTO40
N30
G03I#106
N40
G90G1G40X#107Y#108F100.
#109=#109-#102
END1
N10
G90G0Z#18
M99
-
1
-
-
Sorry rpadyk, I did not give you what you really wanted. I am however working on a pocket id macro that does what you are looking for but its at work and I will have to wait after the holiday to get it to you.
-
Give this a try. I did not have one written so I made up this new one. It is setup for horizontal milling so you can see in the Y axis where it starts and stops. Let me know if it works please. I do not get a chance to prove everything out here at work.
O6011(FINISH ID)
(ABSOLUTE MACRO)
(UNPROVEN)
(FORMAT G65/G66 TCDRZEFS)
(T = #20 - TOOL DIAMETER)
(C = #3 - CUTTER COMP DISTANCE)
(FROM EDGE OF TOOL)
(D = #7 - PART INTERNAL DIAMETER)
(R = #18 - R PLANE)
(E = #8 - END OF ID IN Z)
(F = #9 - FEEDRATE)
(S = #19 SPRING PASSES 3 MAX)
(*********************************)
#103=#5001
#105=#5002
#109=#19
IF[#109GT3.]THEN#109=3.
#113=#105
#115=#105+[[[#7/2.]-[#20/2.]]-#3]
#105=#105+[[#7/2.]-[#20/2.]]
#155=0
#155=#155+[[#7/2.]-[#20/2.]]
G0G90X#103Y#115
Z#18
G1Z#8F50.
G41Y#105F[#9/3.]
WHILE[#119GE0]DO1
IF[#119LT0]GOTO10
#119=#119-1.
G03J-#155Z#106F#9
END1
N10G90G03J-#155
G1G40Y#115
G0Z#18
X#103Y#113
M99
-
I need to update one of the macros because I found an error in it when I was reviewing it, sorry I am not perfect. Please replace the ID-Cone Macro with this:
O6888(CUT 0-180 DEG ID TAPER)
(ABSOLUTE SURFACING MACRO)
(UNPROVEN)
(FORMAT G65/G66 AQDTSRZEF)
(A = #1 - INCLUDED ANGLE OF PART FROM BOTTOM)
(Q = #17 - STEPOVER IN Z/ CUSP HEIGHT)
(D = #7 - TOOL DIAMETER)
(T = #20 - TOOL RADIUS/ BALL OR BULL)
(S = #19 - PART ID/ TOP)
(R = #18 - R PLANE)
(Z = #26 - Z START ZERO)
(E = #8 - END OF TAPER IN Z)
(F = #9 - FEEDRATE)
(***********************************)
#100=ABS[#26]-ABS[#8]
#100=ABS[#100]
IF[[#26*#8]GE0]GOTO1
#100=ABS[#26]+ABS[#8]
N1#101=ROUND[#100/#17]
#102=#100/#101
IF[#102GT[#100/2]]GOTO1000
#103=#5001
#105=#5002
#113=#105
#115=[[#19/2]-[#7/2]]-.1
#115=#105+#115
#155=0
IF[#7EQ[#20*2]]GOTO10
#105=#105-[[#7/2]+#20]
#155=#155-[[#7/2]+#20]
N10#105=#105+[#19/2]
#155=#155+[#19/2]
#125=90.+[#1/2]
#105=#105-[#20/TAN[#125/2]]
#155=#155-[#20/TAN[#125/2]]
G0G90X#103Y#115
Z[#26+.1]
G1Z#26F#9
#106=#5003
G41Y#105
WHILE[#101GE0]DO1
IF[#101LT0]GOTO100
#101=#101-1.
G90G02J-#155F[#9]
#105=-[TAN[#1/2]*#102]
#155=#155-[TAN[#1/2]*#102]
G91G1Y#105Z-[#102]F[#9/3]
END1
N100G0G90Z#18
X#103Y#113
M99
N1000#3000= 1( Q VALUE TOO BIG )
-
Here you go. You will have to create subs with your font and size of number starting with program 8100 representing zero, 8101 representing 1 and so forth. These subs should be posted in incremental.
O8116( S/N MACRO )
( USE OFFSET #100 FOR SERIAL # )
( 00.0001 WILL ENGRAVE 1 )
( 1ST NUMBER )
#138=[#100*.1]
#140=FIX[#138]
#141=#140+8100.
( 2ND NUMBER )
#138=[#140*10]
#139=FIX[#100]
#140=#139-#138
#142=#140+8100.
( 3RD NUMBER )
#138=[#139*10]
#139=FIX[#100*10]
#140=#139-#138
#143=#140+8100.
( 4TH NUMBER )
#138=[#139*10]
#139=FIX[#100*100]
#140=#139-#138
#144=#140+8100.
( 5TH NUMBER )
#138=[#139*10]
#139=FIX[#100*1000]
#140=#139-#138
#145=#140+8100.
( 6TH NUMBER )
#138=[#139*10]
#139=FIX[#100*10000]
#140=#139-#138
#146=#140+8100.
( ARGUMENT )
IF[#141GT8100.]GOTO1
IF[#142GT8100.]GOTO2
IF[#143GT8100.]GOTO3
IF[#144GT8100.]GOTO4
IF[#145GT8100.]GOTO5
IF[#146GT8100.]GOTO6
GOTO100
N1M98P#141
N2M98P#142
N3M98P#143
N4M98P#144
N5M98P#145
N6M98P#146
(UPDATE SERIAL NUMBER)
N100#100=#100+.0001
M99
-
Yes, it is for using a hard tool touch off ike using a piece of .001 shim stock or a .5 inch Joe block. You would have to subtract these values after the touch of or you could just change the macro like this:
.001 shim #5003-.001 or .5 Joe Block #5003-.5.
-
Anyone out there get a chance to use any of the macros yet or have any questions?
-
I was going through my files and realized that I spelled square wrong on a couple of folders, oops my brain must have been on overload.
-
Hi Guys
FANUC 18I-MB5 CONTROL
Not sure if I'm on the right thread here. I need some advice on origin shift after I probed my part with a Renishaw probe.
I'll try to explain what I would like to do. I have a flat composite part with stiffeners glued onto it. The stiffeners are T-shaped with the T-leg basically standing upright. Holes need to be drilled through the stiffeners from the top in the Z- direction. Before I can do that, I need to determine the correct position of each stiffener. The only way for me to do that is by using a Renishaw probe. If you look in the program below, I basically probed certain positions in the X- direction. That actual value gets saved on the control from variable #111 onwards. That is after the calculation was made with the stylus size etc.
All of that is working very well. Each position that I probe gets saved in the next variable number. i.e. #112, #113, #114, etc. (See blocks N28; N40; N52)
Here's an extract from my program to show how the probing works. I only copied the first 3 probing positions as an example:
N1 G92.1 X0 Y0 Z0 B0 C0
N2 G5P0
N3 G52 X0 Y0 Z0
N4 (*****************)
N5 G55
N6 ( 6 MM PROBE)
N7 G53 G90 G00 G49 Z0 H0
N8 T15 M6
N9 G55
N10 G0 B0. C0.
N11 H15
N12 G359
N13 M5
N14 G91 G43 H15 Z0
N16 G90
N16 G0 X-91.52 Y110.282 B0. C0.
N17 Z62.
N18 ( TP015 - PROBE STIFFENERS)
N19 ( PROBE CYCLE)
N20 M46
N21 G4 X2.
N22 G0 X-91.52 Y110.282 Z62. B0. C0. M81
N23 G31 G1 Z27. F300.
N24 G31 X-111.52
N25 G4 X0.5
N26 G91 X10.
N27 G90 G31 X-111.52 F60
N28 #111=#5061
N29 G0 X-91.52
N30 Z62.
N31 #100=#4111
N32 #101=#[#100+13000]+#[#100+12000] (PROBE RADIUS)
N33 #111=#111-#101-[-101.52]
N34 G0 Y254.4
N35 G31 G1 Z27. F300.
N36 G31 X-111.52
N37 G4 X0.5
N38 G91 X10.
N39 G90 G31 X-111.52 F60
N40 #112=#5061
N41 G0 X-91.52
N42 Z62.
N43 #100=#4111
N44 #101=#[#100+13000]+#[#100+12000] (PROBE RADIUS)
N45 #112=#112-#101-[-101.52]
N46 G0 Y553.4
N47 G31 G1 Z27. F300.
N48 G31 X-111.52
N49 G4 X0.5
N50 G91 X10.
N51 G90 G31 X-111.52 F60
N52 #113=#5061
N53 G0 X-91.52
N54 Z62.
N55 #100=#4111
N56 #101=#[#100+13000]+#[#100+12000] (PROBE RADIUS)
N57 #113=#113-#101-[-101.52]
The problem comes in where I would like to shift the drill positions now. (See extract below of where I want to call an offset variable each time)
I have an exact point where I would like to drill the first hole according to the part model. Because the stiffeners can be glued out of position slightly, I have to probe their actual position. Now I would like to shift that drill point with the deviation I determined with the probe. Hope this all makes sense. How do I do that? For instance, if the hole that I would like to drill first is closest to variable #111, I would like to offset my X- value with the value that was written in #111 and so forths. When ever I call a variable at a hole, that X- value for that specific hole must be shifted with the value in the variable. By the way, in my CAM software I can tell the probe whether I want to probe in the X- or Y- direction. In this case all the probe points were done in the X- direction.
If you look at the next program extract:
N167 ( 2.7 DIA TWIST DRILL)
N168 G49
N169 G53 G90 G00 G49 Z0 H0
N170 T14 M6
N171 G55
N172 G0 B0. C0.
N173 H14
N174 G359
N175 S8230 M3
N176 G05P10000R10
N177 G43.4 H14
N178 G0 X113.4 Y1439.808 B0. C0.
N179 Z62.
N180 G49
N181 G5P0
N182 G52 X[#117] Y0
N183 G43.4 H14
N184 ( TP001 - DRILL 2.7 PILOT HOLES)
N185 ( DRILL CYCLE)
N186 X113.4 Y1439.808 Z80.22
N187 X113.4
N188 M80
N189 ( DEEPHOLE DRILL)
N190 X113.4
N191 Z12.22
N192 G1 Z8.22 F494.
N193 G0 Z12.22
N194 Z9.72
N195 G1 Z4.22
N196 G0 Z12.22
N197 Z5.72
N198 G1 Z0.22
N199 G0 Z12.22
N200 Z1.72
N201 G1 Z-2.253
N202 G0 Z51.968
N203 ( DEEPHOLE DRILL)
N204 X92.6
N205 Z12.22
N206 G1 Z8.22
N207 G0 Z12.22
N208 Z9.72
N209 G1 Z4.22
N210 G0 Z12.22
N211 Z5.72
N212 G1 Z0.22
N213 G0 Z12.22
N214 Z1.72
N215 G1 Z-2.253
N216 G0 Z80.22
N217 G49
N218 G5P0
N219 G52 X[#116] Y0
N220 G43.4 H14
N221 ( TP001 - DRILL 2.7 PILOT HOLES STIFFENERS)
N222 ( DRILL CYCLE)
N223 X-92.6 Y1439.808 Z80.22
N224 X-92.6
N225 ( DEEPHOLE DRILL)
N226 X-92.6
N227 Z12.22
N228 G1 Z8.22
N229 G0 Z12.22
N230 Z9.72
N231 G1 Z4.22
N232 G0 Z12.22
N233 Z5.72
N234 G1 Z0.22
N235 G0 Z12.22
N236 Z1.72
N237 G1 Z-2.253
N238 G0 Z51.968
N239 ( DEEPHOLE DRILL)
N240 X-113.4
N241 Z12.22
N242 G1 Z8.22
N243 G0 Z12.22
N244 Z9.72
N245 G1 Z4.22
N246 G0 Z12.22
N247 Z5.72
N248 G1 Z0.22
N249 G0 Z12.22
N250 Z1.72
N251 G1 Z-2.253
N252 G0 Z80.22
N253 G49
N254 G5P0
Block N178 is where the first hole position is.
Block N182 calls for the X- offset. (Using the variable saved in #117)
The shift does actually happen there. The machine physically moves with the amount that was saved in #117. It ads the difference to X113.4 value that is at block N178.
The problem comes in where the machine hits the next X- value and the next and the next. I would like to drill a set of holes around variable #117 for instance. I want it to keep that offset for each X- value until I call a different variable. When it gets another X- value like block N186, it moves to that exact value. Completely ignoring the offset that it just used.
My whole explanation is about this. I want the control to use that #111 or #112 or #113, etc. for each X- value until I change the variable number or when it reaches a tool change which will clear all offsets.
Is there a way that one can program it in such a way?
I was thinking at one point to add the variable to each and every X- value myself, in order for the shift to take place. The control does not accept my format. I keep on getting an alarm that says "No value after address".
Here is what I was thinking of doing.
At each X- value, just add #111 or #112 to that value. Can it be done and how?
Can I not change block N186 like this?
X113.4+[#117] Y1439.808 Z80.22
or
[X113.4+#117] Y1439.808 Z80.22
or
X113.4+#[#117] Y1439.808 Z80.22
I don't have any clues left. This would have make logic sense to me. Just add the little bit of offset to your X- or Y- value and then drill the hole.
Hope someone can shed some light on this.
Thanks
I believe your syntax is a little off and that is why you are getting the alarms. Please try it this way.
X[113.4+#117].
-
Most of these I wrote about five years ago when I first realized how powerful custom macro b was. I would have to say that most applications for these would be for tooling but we have used them for parts here at work. If it is not clear as to what something does for you guys please ask and I will gladly answer any questions for you. Remember if it says not proven it means I have not even cut any chips with it yet. So, it is worthy of a dry run if you want to play with it. I believe most or all of the toolpath I incorporated has a .100 thousandths clearance on all of the moves. If you would like to change something with one of them we can do that here as well. Just post the macro with your request and I can help you change it. One I forgot to add to the list was my most recent. It is a tool change macro that automatically sets each tool. Should work for most fanucs and robodrills.
O0001(AUTOMATIC TLO MACRO)
(CHANGE 2000 TO 2200 FOR ROBODRILL)
(YOU MUST MANUALLY SET #100 & #101)
(DO NOT FORGET THE DECIMALS)
M00
#100=1.(FIRST TOOL TO SET)
#101=10.(LAST TOOL TO SET)
N1T#100M06
#102=#100+2000.
M00
(TOUCH TOOL)
(HIT CYCLE START)
#[#102]=#5003
G91G28Z0
G90
#100=#100+1.
IF[#100LT#101]GOTO1
M30
-
So I have decided I am going to share my custom macro B programs. These programs generate 3D and basic 2D shapes for CNC mills. The C variable on the radius macros is the angle of incremental rotation that you want to cut in degrees.
-
1
-
3
-
-
Here is my latest macro for standard mills. I have only dry ran it and not been able to cut any chips with it yet. I am not familiar with mill turns so in order for me create the macro you are looking for I would need to know your exact variable inputs, the variables that you have at your disposal and what you need the macro to do exactly in order for me to help you. Thanks.
O5656(DIAMOND PIN MACRO)
(PIN AT 0 DEGREES IS VERTICAL)
(ABSOLUTE MACRO)
(FORMAT G65/G66 ABDTMWREFS)
(A = #1 - INCLUDED ANGLE OF PIN)
(60 DEGREES IS COMMON)
(B = #2 - G68 ROTATION FROM 0 DEGREES)
(D = #7 - DIAMETER OF PIN)
(T = #20 - TOOL DIAMETER)
(M = #13 - MATERIAL SIZE)
(SQUARE OR ROUND)
(W = #23 - WIDTH OF PIN CONTACT)
(R = #18 - R PLANE)
(E = #8 - END OF EM IN Z)
(F = #9 - FEEDRATE)
(S = #19 - # OF SPRING PASSES)
(*********************************)
(LIMIT SPRING PASSES TO 3.)
IF[#19GT3.]THEN#19=3.
(STORE CURRENT XY POSTION)
#100=#5001
#101=#5002
(CALCULATE TANGENT POSITIONS)
(BASED ON ARGUMENT -A-)
(-X-/-I-)
#102=[#23/2.]+[COS[#1/2.]*[#20/2.]]
(-Y-/-J-)
#123=ASIN[#23/2.]/[#7/2.]
#103=[COS[#123]*[#7/2.]]+[sIN[#1/2.]*[#20/2.]]
(CALCULATE FIRST POSITION -X-)
#105=#102+[TAN[#1/2.]*[#103]]
(CALCULATE MATERIAL CLEARANCE)
#106=[#13/2.]+[#20/2.]+.1
(STORE EACH LOCATION)
#110=#100-#106
#111=#101
#112=#100-#105
#113=#100-#102
#114=#101+#103
#115=#100+#102
#116=#101+#103
#117=#100+#105
#118=#101
#119=#100+#102
#120=#101-#103
#121=#100-#102
#122=#101-#103
(SET SPRING PASS COUNTER)
#149=#19
(SET ROTATION)
#530=#2
IF[#2GT180.]THEN#530=#2-360.
G68R#530
(GOTO 1ST POSTION)
G0G90X#110Y#111
Z[#8+.1]
G1Z#8F#9
G41X#112
WHILE[#149GE0]DO1
IF[#149LT0]GOTO10
#149=#149-1.
G1X#113Y#114
G02X#115Y#116I#102J-[#103]
G1X#117Y#118
X#119Y#120
G02X#121Y#122I-[#102]J#103
G1X#112Y#111
END1
N10G1G40G90X#110
G0Z#18
G69
X#100Y#101
M99
-
I hope someone out there will have a use for this. Someone at work gave me the idea. Check it out.
O5656(DIAMOND PIN MACRO)
(PIN AT 0 DEGREES IS VERTICAL)
(ABSOLUTE MACRO)
(UNDER DEVELOPMENT)
(FORMAT G65/G66 ABDTMWREFS)
(A = #1 - INCLUDED ANGLE OF PIN)
(60 DEGREES IS COMMON)
(B = #2 - G68 ROTATION FROM 0 DEGREES)
(D = #7 - DIAMETER OF PIN)
(T = #20 - TOOL DIAMETER)
(M = #13 - MATERIAL SIZE)
(SQUARE OR ROUND)
(W = #23 - WIDTH OF PIN CONTACT)
(R = #18 - R PLANE)
(E = #8 - END OF EM IN Z)
(F = #9 - FEEDRATE)
(S = #19 - # OF SPRING PASSES)
(*********************************)
(LIMIT SPRING PASSES TO 3.)
IF[#19GT3.]THEN#19=3.
(STORE CURRENT XY POSTION)
#100=#5001
#101=#5002
(CALCULATE TANGENT POSITIONS)
(BASED ON ARGUMENT -A-)
(-X-/-I-)
#102=[#23/2.]+[COS[#1/2.]*[#20/2.]]
(-Y-/-J-)
#123=ASIN[#23/2.]/[#7/2.]
#103=[COS[#123]*[#7/2.]]+[sIN[#1/2.]*[#20/2.]]
(CALCULATE FIRST POSITION -X-)
#105=#102+[TAN[#1/2.]*[#103]]
(CALCULATE MATERIAL CLEARANCE)
#106=[#13/2.]+[#20/2.]+.1
(STORE EACH LOCATION)
#110=#100-#106
#111=#101
#112=#100-#105
#113=#100-#102
#114=#101+#103
#115=#100+#102
#116=#101+#103
#117=#100+#105
#118=#101
#119=#100+#102
#120=#101-#103
#121=#100-#102
#122=#101-#103
(SET SPRING PASS COUNTER)
#149=#19
(SET ROTATION)
#530=#2
IF[#2GT180.]THEN#530=#2-360.
G68R#530
(GOTO 1ST POSTION)
G0G90X#110Y#111
Z[#8+.1]
G1Z#8F#9
G41X#112
WHILE[#149GE0]DO1
IF[#149LT0]GOTO10
#149=#149-1.
G1X#113Y#114
G02X#115Y#116I#102J-[#103]
G1X#117Y#118
X#119Y#120
G02X#121Y#122I-[#102]J#103
G1X#112Y#111
END1
N10G1G40G90X#110
G0Z#18
G69
X#100Y#101
M99
-
For my return height I use .01" and for a full retract I use .100" above the hole.
Ditto.
-
I would like some more ideas for this stuff. The latest one was a friend of mine who wanted a diamond pin macro which I am working on right now. I will post it when all of the bugs are worked out.
-
Its almost easier to write it by hand. All u have to do is use a W and this allows u to pull out the stock incrementally in Z. Ex if you want to pull one in than, set bar puller, unclamp chuck, W1., clamp, reference return.
-
I worked in a small shop many years ago and all the owner used were 80 deg diamond inserts for rigitity reasons and we would also use left handed tooling to put all of the pressure on the machine instead of pulling up the turret. Depending on how u program the part we would use a .015 rad tool at .004 per revolution with a .005 doc. Now if u are facing and dragging the tool then u would only want to leave .002 on the face for finish.
-
I think they are the same someone just renamed them here for whatever probably non essential reason.
-
I have never machined a magnet before, but if straight carbide does not work try a diamond coating or CBN tool.
-
- Here is my rough draft of the probe calibration Macro for 4 AXIS. Please give me your feed back as I have not proven this out yet. As for the probe head this macro would work regardless of the ruby size. You would just have to change the size of #500.
-
O0001(MITSUI Probe Cal 15M Fanuc)
(Probe Calibration Block Is)
(A 6x6x1 Inch Aluminum Plate)
(Y0 IS BASE OF BLOCK)
(Machine is grided to COR X0 Z0)
G90G10P1L2X0Y0Z0B0
G11
T1
(SET VARIABLES)
(2MM RUBY BALL RADIUS)
#500=[1./25.4]
(X SHIFT)
#501=0
(Y SHIFT)
#502=0
(BALL Z CENTERLINE)
#503=#500
M00
(MEASURE RAIL W/ A MICROMETER)
(CHANGE VARIABLE #600 TO RAIL)
(MEASUREMENT AND THEN xxxxM)
(RAIL AND BORE FOR FULL CLEANUP)
(RUN DRY OR USE ALCOHOL)
#600=1.
M00
N1T1M06
T2
(T1 = .5 4FLT EM)
(CUT RAIL BOTH SIDES)
(REMOVE .005 FROM EACH SIDE)
M03S8000
M11
G0G90G54B-3.
B0
M10
G0X-4.Y5.8
G43Z5.H1D1
G1Z[[#600/2.]-.005]F5.
X4.F50.
(SPRING PASS)
X-4.
Y10.
M11
G0G90G54B177.
B180.
M10
G1Y5.8
X4.
(SPRING PASS)
X-4.
GOZ5.
M98P8800
M01
N2T2M06
T9000
(T2 = BORING BAR)
(NEED FULL CLEAN UP)
(BORE A HOLE AT X0Y0)
(ALL THE WAY THROUGH BLOCK)
(RUN DRY OR USE ALCOHOL)
M03S1000
M11
G0G90G54B-3.
B0
M10
G0X0Y3.
G43Z5.H2D2
G98G85X0Y3.Z-.55R.55F5.
G0G80Z5.
M98P8800
M01
M00
(MEASURE RAIL AGAIN WITH MIC)
(INPUT #600)
(THIS FEATURE WILL BE USED)
(TO SET #503 AND Z GRID)
#600=.99
M00
(MEASURE BORED HOLE WITH)
(A TRI MIC OR DIAL BORE)
(INPUT #601 WILL BE USED)
(TO SET #500~#502 AND)
(X GRID SHIFT)
#601=1.
M01
N100M00
T9000
(T9000 = 2MM PROBE)
(USING STANDARD 9911 AND 9914)
(MACROS SET #500~#503)
(AND VERIFY GRID)
(IF THIS SECTION OF CODE)
(KEEPS GOING BACK TO)
(N100 CHECK BALL)
(FOR RUNOUT AND/OR SEE)
(IF IT IS LOOSE OR DAMAGED)
T9000M06
M11
G0G90G54B-3.
B0
M10
X0Y3.
G43Z5.H9000D9000
Z.1
(SAFETY Z MACRO)
G65P9910Z0F50.
(SET PROBE HOLE AT B0)
G65P9914D#601R.5Q.5
#500=#500+[#143/2.]
#501=#140/2.
#502=#141/2.
#503=#500
(SET ACCURACY AT .0002)
#602=[#140+#141+#143]/3.
IF[#602GT.0002]GOTO100
G0Z1.
Y5.75
(PROBE RAIL Z AT B0)
G65P9911Z[#600/2.]R.5Q.5
#603=#138
#604=#142
G0Z5.Y10.
M11
G0G90G54B177.
B180.
M10.
X0Y5.75
Z1.
(PROBE RAIL Z AT B180.)
G65P9911Z[#600/2.]R.5Q.5
#605=#138
#606=#142
(CHECK GRID PROBE HOLE AT B180.)
X0Y3.
(SAFEFTY Z MACRO)
G65P9910Z0F50.
G65P9914D#601R.5Q.5
#607=#140
IF[ABS[[#604+#606]/2.]GT.0005]G0T0200
IF[ABS[#607]GT.0005]G0T0300
G0Z5.
M98P8800
M30
M00
N200
(Z GRID IS OFF CHECK #603~#606)
M00
N300
(X GRID IS OFF CHECK #607)
- Here is my rough draft of the probe calibration Macro for 4 AXIS. Please give me your feed back as I have not proven this out yet. As for the probe head this macro would work regardless of the ruby size. You would just have to change the size of #500.
-
Rob, thanks for trying it out. I have plenty more where that came from if you need anything else.
-
Got busy the past couple of weeks with other projects, but I did start to write the 4 axis probe calibration cycle for the Mitsui. It will use variables #500~#503 as the set values for all of the other probe macros. This program will also be able to check and help set the grid of the machine as well. I wont know until we run it, wish me luck.
Cool Macros
in Machining, Tools, Cutting & Probing
Posted
My newest macro for Haas machining centers. My brother needed a way to automatically set G52-G59 using any tool guage length.
O0001
(Use decimal point when changing coordinate system number.)
(Change #600)
#600=52.(Coordinate System)
(Coordinate System Variable Set)
#652=5203.(G52)
#654=5223.(G54)
#655=5243.(G55)
#656=5263.(G56)
#657=5283.(G57)
#658=5303.(G58)
#659=5323.(G59)
(SET Z)
#[600.+#600]=#5023+#[2000.+#3026]
M30