Hello Guest it is January 29, 2020, 01:55:45 PM

Author Topic: Work offsets  (Read 11402 times)

0 Members and 1 Guest are viewing this topic.

Offline BR549

*
  •  6,925 6,925
    • View Profile
Re: Work offsets
« Reply #10 on: September 15, 2011, 11:09:11 PM »
You just don't use toolComp with Fixture offsets OR deep subs.

I feel your pain BUT it is what it is. (;-(

(;-) TP

Offline Riley

*
  •  43 43
    • View Profile
Re: Work offsets
« Reply #11 on: September 16, 2011, 09:17:13 PM »
I'm not sure why but on a windows7 box the toolpath is fine. Every combination of tcomp and subs in any work offset I have tried works normal. Is it possible something on that xp box is corrupt?

Offline BR549

*
  •  6,925 6,925
    • View Profile
Re: Work offsets
« Reply #12 on: September 16, 2011, 09:35:34 PM »
I have found it broken on W2k XP and Vista so far. Have not tried it on Win7 yet.

Please list the code you were using.  Also include what the modal calls were in the mode list.

(;-) TP

Offline Riley

*
  •  43 43
    • View Profile
Re: Work offsets
« Reply #13 on: September 16, 2011, 10:05:21 PM »
G15 G0 G53 G17 G40 G20 G90 G94 G55 G49 G98 G64 G97

Hi, not even sure what a G97 is but its in there....thanks for the help with this one! Most of the programs I have needed in the past the wizards worked just fine for but now I need to run a lot of parts and want to handle them as little as possible. This is only a sample program to make sure I can get everything working right before I start coding the actual parts. Wish I had another xp box to test it on.

Offline BR549

*
  •  6,925 6,925
    • View Profile
Re: Work offsets
« Reply #14 on: September 17, 2011, 12:29:15 AM »
NOPE it does not work here, same thing.

I can do what you wanted but it is not a pretty thing to do. Instead of using a Fixture offset, G92 or G52 You can use a G53 move in machine coords then use a macro to reset machine Zero. That process works EVERY time correctly. Trouble is YOU Have to keep track of where you are instead of MACH doing the hard work(;-)
G54
M98 P1 L1
G53 X6.000
M80  ( SetMachZero(0), SetMachZero(1)  )
M98 P2 L1
G53 X12.000
M80
M98 P3 L1
G53 X-18.000
M80
M30

Offline BR549

*
  •  6,925 6,925
    • View Profile
Re: Work offsets
« Reply #15 on: September 17, 2011, 12:57:57 AM »
There IS one other way that is not as messy. It keeps the Mach coord base intact so you at least know where you are(maybe). It also works EVERY time. IF you set the Work 0,0 as refhome(machine 0,0) then it it is fairly simple.

G54
M98 P1 L1
G0 X6.000
M80  ( zeroX, zeroY  )
M98 P2 L1
G0 X6.000
M80
M98 P3 L1
G53 X0.000
M80
M30

HOPE it helps,(;-) TP
« Last Edit: September 17, 2011, 12:59:46 AM by BR549 »

Offline BR549

*
  •  6,925 6,925
    • View Profile
Re: Work offsets
« Reply #16 on: September 17, 2011, 11:59:08 AM »
RIley I have developed a WORKAROUND for you that makes sense. We have to get creative and shift the Fixture offset BEFORE you leave the sub. Then it will work every time. The only limit IS you have to make sure all the fixture calls are in the same order of progression as the #var formula to index up the number. NOte that it starts with G54 then each loop indexes the G54 UP 1 number G54,G55,G56,etc. IT will not allow you to randomly switch Fixtures but at least it does give you an Option with TC and fixtures.

I have narrowed this problem down to a very specific area in MACH3 that should not be hard to find(;-).

N0000 (Filename: TCtest.tap)
N0010 (Post processor: Mach3.scpost)
N0020 (Date:09/16/11 Time:11:36:09 PM)
N0030 G20 (Units: Inches)
N0040 G40 G90  G54
N0050 F1
N0060 (Part: TCtest)
N0070 (Operation: Outside Offset, 0, T1: Mill/router, 0.5 in diameter, 0.02 in Deep)
N0080 (Intake)
N0090 S1000 G00 Z0.5000
#100 = 54
N0110 (Mill/router, 0.5 in diameter)
N0120 T1 M06
N0140 S1000 M03 F30
%
G0 X0Y0
M98 P1 L4
M30
%
o1
G0 X6 Y1.799
M8
N0100 X6.000 Y1.799
N0001 G41 D1
N0150 G00 X4.8900 Y2.4278
N0160 Z0.0197
N0170 G01 Z-0.020 F10
N0180 G01 X4.2500 Y1.7878 Z-0.0200  F30.0
N0190 G01 Y0.0000 Z-0.020
N0200 G02 X4.0000 Y-0.2500 Z-0.0200 I-0.2500 J0.0000
N0210 G01 X0.0000 Z-0.020
N0220 G02 X-0.2500 Y0.0000 Z-0.0200 I0.0000 J0.2500
N0230 G01 Y4.0000 Z-0.020
N0240 G02 X0.0000 Y4.2500 Z-0.0200 I0.2500 J0.0000
N0250 G01 X4.0000 Z-0.020
N0260 G02 X4.2500 Y4.0000 Z-0.0200 I0.0000 J-0.2500
N0270 G01 Y1.7878 Z-0.020
N0280 G01 X4.8900 Y1.1478 Z-0.0200
N0290 G00 Z0.5000
N0300 G40
N0310 G00 X6.000 Y1.799
N0320 M09 (Coolant off)
#100=[#100+1]
G#100
N0330 M99
%

Hope that helps, (;-) TP


Offline Riley

*
  •  43 43
    • View Profile
Re: Work offsets
« Reply #17 on: September 17, 2011, 12:42:06 PM »
You ARE the man! I can't thank you enough! I really was not even close to that after days of attempts. I guess it's like they say about skinning that old cat. That gives me a great platform for a mutiple vise setup. I'm thinking the next best thing to mach is this site!

Offline Riley

*
  •  43 43
    • View Profile
Re: Work offsets
« Reply #18 on: September 17, 2011, 03:21:06 PM »
I am set to run this job, thanks again. I am cutting three holes for switches in the left side vice, a hole for a cord in middle vise, and right side vise runs the same part as the first. I have to keep pretty close numbers on stations 1 and 3. The hole cutout is not too critical so I removed the g41 in that sub. Try the attached code out and it should run fine. Then enable tcomp in the second sub and see what happens. I am good to go and I thank you for the help just wanted some feedback on why one sub can be run as often as I like with comp but a second sub with comp will crash out.

Offline BR549

*
  •  6,925 6,925
    • View Profile
Re: Work offsets
« Reply #19 on: September 17, 2011, 08:50:21 PM »
HIYA Riley, I think I can save you some more time (;-). I came up with a workaround that will allow you to do as you wish roam in the Workoffsets as you please.

DO NOT USE G54 as your base offset.      Use G55 and above as your base offset X0Y0 THEN you can program as you wish it will work 24/7. JUST DO NOT USE G54 anywhere(;-)

I think I have the BUG narrowed down to just a small window of possiblities now.

Give it a try, Let me know IF it works for you. (;-) TP