Printable View
Hi everyone, im a Mach3 newbie. rebuilt my cnc machine from DSP control to mach3. Everything is actually up and running.
but, if i do a job, boring several holes, i have this problem that after every hole, spindle rises, and then hold about 2 seconds before moving to next hole.
Im using Bobcad/cam, dwell time is set to zero... help anyone, please ?
post your g-code.
Hi, well i contacted machsupport, and they found nothing wrong with my g-code. I tried it myself on another computer, with paralell port settings, and it worked out ok.Quote:
Originally Posted by ger21
Machsupport think it is something wrong with computer or external motion device. So i hooked up a laptop to the cnc, and used same settings, plugins etc, and got the same problem.
I attached the plugin here, dont know if anyone can see something wrong with it ?
Here is g code as well :
(BEGIN PREDATOR NC HEADER)
(MACH_FILE=3AXVMILL_MM.MCH)
(MTOOL T1 S1 D8. H127. DIAM_OFFSET 1 = 4.)
(MTOOL T2 S1 D5. H127. DIAM_OFFSET 2 = 2.5)
(MTOOL T3 S1 D10. H127. DIAM_OFFSET 3 = 5.)
(SBOX X0. Y0. Z-25.4 L900. W1620. H0.)
(END PREDATOR NC HEADER)
%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - 1620H.NC)
(POST - MACH 3 MILL METRIC)
(DATE - FRI. 03/20/2015)
(TIME - 10:20PM)
N100 G21 G40 G49 G54 G80 G90 G91.1
N101 G53 Z0.
(JOB 1 HOLE RANDOM POINT PATTERN)
(8MMTAPPSTAMME)
N102 M06 T1
N103 S18000 M03
N104 G00 G90 G54 X857.5 Y107.
N105 G43 H1 Z2.54 M08
N106 G81 G98 X857.5 Y107. Z-17.403 R2.54 F3000.
N107 X793.5
N108 X473.5
N109 X409.5
N110 X153.5
N111 X89.5
N112 Y869.
N113 X153.5
N114 X409.5
N115 X473.5
N116 X793.5
N117 X857.5
(JOB 2 HOLE RANDOM POINT PATTERN)
(8MMTAPPSTAMME)
N118 S18000
N119 G00 X857.5 Y1290.
N120 G81 G98 X857.5 Y1290. Z-21.403 R2.54 F3000.
N121 X793.5
N122 X633.5
N123 X569.5
N124 M09
N125 M05
N126 G53 Z0.
N127 M01
(JOB 3 HOLE RANDOM POINT PATTERN)
(5MM STAMMEHULL)
N128 M06 T2
N129 S18000 M03
N130 G00 G90 G54 X839. Y520.
N131 G43 H2 Z2.54 M08
N132 G81 G98 X839. Y520. Z-15. R2.54 F3000.
N133 Y488.
N134 Y456.
N135 Y424.
N136 Y392.
N137 Y360.
N138 Y328.
N139 Y296.
N140 Y264.
N141 Y232.
N142 Y200.
N143 Y552.
N144 Y584.
N145 Y616.
N146 Y648.
N147 Y680.
N148 Y712.
N149 Y744.
N150 Y776.
N151 Y808.
N152 Y968.
N153 Y1000.
N154 X450. Y808.
N155 Y776.
N156 Y744.
N157 Y712.
N158 Y680.
N159 Y648.
N160 Y616.
N161 Y584.
N162 Y552.
N163 Y520.
N164 Y488.
N165 Y456.
N166 Y424.
N167 Y392.
N168 Y360.
N169 Y328.
N170 Y296.
N171 Y264.
N172 Y232.
N173 Y200.
N174 X47.
N175 Y232.
N176 Y264.
N177 Y296.
N178 Y328.
N179 Y360.
N180 Y392.
N181 Y424.
N182 Y456.
N183 Y488.
N184 Y520.
N185 Y552.
N186 Y584.
N187 Y616.
N188 Y648.
N189 Y680.
N190 Y712.
N191 Y744.
N192 Y776.
N193 Y808.
N194 X839. Y1448.
N195 Y1480.
N196 M09
N197 M05
N198 G53 Z0.
N199 M01
(JOB 4 PROFILE)
(CUT 10)
N200 M06 T3
N201 S18000 M03
N202 G00 G90 G54 X905. Y-5.
N203 G43 H3 Z2.54 M08
N204 G00
N205 G01 Z-18. F3000.
N206 Y1630.584 F6000.
N207 X-5. Y882.362
N208 Y-5.
N209 X905.
N210 G80
N211 G00 Z2.54
N212 Z1.29
N213 G01 Z-19.25 F3000.
N214 Y1630.584 F6000.
N215 X-5. Y882.362
N216 Y-5.
N217 X905.
N218 G00 Z2.54
N219 M09
N220 M05
N221 G53 Z0.
N222 G53 Y0.
N223 M02
(END OF PROGRAM)
N224 M30
%
You're using an ncPod? Afaik, that plugin was never finished. I'd move on to a more modern controller that has someone supporting it.
Ohh, well, yes, i guess :)Quote:
Originally Posted by ger21
Its from http://www.cdxhctech.com/ , they are supporting it, kind of...you know..
Its a jungle out there with controllers, i think, so i did not know what to look for..
OK, then, that's not what I thought it was.
You should send all this information to the manufacturer and see if they can fix the plugin for you.
Yes i know, im in dialog with them, but its going slow, and there is a language issue as well, their english is worse than mine :)Quote:
Originally Posted by ger21
I guess Mach support did not look at your program to carefullyQuote:
Originally Posted by kvadda
After each canned cycle you need to cancel with a G80
Also it may work in Mach3 but it should not, is a G53 by itself, the last G53 move/use is correct as it has a G0 move before it
So after each Canned Cycle operation you need it to look like this
G80G0Z0. (after each Canned Cycle Operation)
You last part of you program is almost correct
N218G80 G00 Z2.54 ( this line should have the cancellation of the canned cycle, just add the G80 )
N219 M09
N220 M05
N221 G53 Z0.
N222 G53 Y0.
So if you don't have a G0 move before the use of a G53 then it can/should be used like this
G0G53
It seems you have a computer or control settings that need some change as well, your program should run, ok but make the changes, as I have & try it
hi,Quote:
Originally Posted by mactec54
thanks for the info !!
Bobcad dint see this either... I hope its possible for them to include this in the post-processor ? So i dont have to edit every job ?
kvadda
Yes this is an easy postprocessor change, for them
While you are at getting some changes done, this part needs some work also
Because this is a profile operation no G80 is needed, only at the end of each canned cycle
N200 M06 T3
N201 S18000 M03
N202 G00 G90 G54 X905. Y-5.
N203 G43 H3 Z2.54 M08
N204 G00 ( this G00 should be removed as well it has no function, in this position )
N205 G01 Z-18. F3000.
N206 Y1630.584 F6000.
N207 X-5. Y882.362
N208 Y-5.
N209 X905.
N210 G80 ( remove this G80 )
N211 G00 Z2.54
N212 Z1.29
N213 G01 Z-19.25 F3000.
N214 Y1630.584 F6000.
N215 X-5. Y882.362
N216 Y-5.
N217 X905.
N218 G00 Z2.54
N219 M09
N220 M05
N221 G53 Z0.
N222 G53 Y0.
N223 M30 (Put the M30 Here, Remove the M02 )
%
Don't need the M02 in there, when using a M30
Thanks for all help Mactec, i will send them this info. I will also have a look at it myself, trying to learn how this works. I have this sick mind that, something others can do...i can as well...:drowning:Quote:
Originally Posted by mactec54
A little update on this. the manufacturer of the usbpod made me a new driver, and problem solved !
Good that the board is well supported.
hi Mactec,Quote:
Originally Posted by mactec54
now i read that part where you think i have some computer or control settings that needs some change. getting curious of what ?
I think it have som "hickups" from time to time.... And it doesnt cut 2 parts similar... G code below, it cutted the 2 longest parts, with almost 1mm difference
And, if i jog between the tool change, it set zero +37mm x axis and about -15mm y axis...
(BEGIN PREDATOR NC HEADER)
(MACH_FILE=3AXVMILL_MM.MCH)
(MTOOL T1 S1 D8. H127. DIAM_OFFSET 1 = 4.)
(MTOOL T2 S1 D10. H127. DIAM_OFFSET 2 = 5.)
(SBOX X0. Y0. Z-25.4 L330. W1761. H0.)
(END PREDATOR NC HEADER)
%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - HYLLE GUDMUND.NC)
(POST - MACH 3 MILL METRIC)
(DATE - MON. 03/23/2015)
(TIME - 02:47PM)
N100 G21 G40 G49 G54 G80 G90 G91.1
N101 G53 Z0.
(JOB 1 HOLE RANDOM POINT PATTERN)
(8MMTAPPSTAMME)
N102 M06 T1
N103 S18000 M03
N104 G00 G90 G54 X20. Y322.
N105 G43 H1 Z2.54 M08
N106 G81 G98 X20. Y322. Z-17.403 R2.54 F3000.
N107 Y290.
N108 X84.
N109 Y322.
N110 X212.
N111 Y290.
N112 X276.
N113 Y322.
N114 Y602.
N115 X212.
N116 X84.
N117 X20.
N118 Y10.
N119 X84.
N120 X212.
N121 X276.
N122 M09
N123 M05
N124 G53 Z0.
N125 M01
(JOB 2 PROFILE)
(CUT 10)
N126 M06 T2
N127 S18000 M03
N128 G00 G90 G54 X331.5 Y8.
N129 G43 H2 Z2.54 M08
N130 G00
N131 G01 Z-13. F3000.
N132 Y292. F6000.
N133 G80
N134 G00 Z2.54
N135 Y320.
N136 G01 Z-13. F3000.
N137 Y604. F6000.
N138 G00 Z2.54
(JOB 3 PROFILE)
(CUT 10)
N139 S18000
N140 X-5. Y-5.
N141 G01 Z-18. F3000.
N142 X335. F6000.
N143 Y305.
N144 X-5.
N145 Y-5.
N146 G00 Z2.54
N147 Z1.29
N148 G01 Z-19.25 F3000.
N149 X335. F6000.
N150 Y305.
N151 X-5.
N152 Y-5.
N153 G00 Z2.54
N154 Y307.
N155 G01 Z-18. F3000.
N156 X335. F6000.
N157 Y617.
N158 X-5.
N159 Y307.
N160 G00 Z2.54
N161 Z1.29
N162 G01 Z-19.25 F3000.
N163 X335. F6000.
N164 Y617.
N165 X-5.
N166 Y307.
N167 G00 Z2.54
N168 X330.5 Y619.
N169 G01 Z-18. F3000.
N170 Y1191. F6000.
N171 X-5.
N172 Y619.
N173 X330.5
N174 G00 Z2.54
N175 Z1.29
N176 G01 Z-19.25 F3000.
N177 Y1191. F6000.
N178 X-5.
N179 Y619.
N180 X330.5
N181 G00 Z2.54
N182 Y1194.
N183 G01 Z-18. F3000.
N184 Y1766. F6000.
N185 X-5.
N186 Y1194.
N187 X330.5
N188 G00 Z2.54
N189 Z1.29
N190 G01 Z-19.25 F3000.
N191 Y1766. F6000.
N192 X-5.
N193 Y1194.
N194 X330.5
N195 G00 Z2.54
N196 M09
N197 M05
N198 G53 Z0.
N199 G53 Y0.
N200 M02
(END OF PROGRAM)
N201 M30
%
kvadda
If your machine is returning to Zero, or part position Zero when it has finished cutting, then you have only the program to look at
You have 2 canned cycles, that you still have not changed in the program both need a G80 to cancel before the next operation, this can throw off the position for the next operation
Your program is incorrect the way it is
When the machine is done cutting, it returns to z zero and y zero.Quote:
Originally Posted by mactec54
If i change tool in the middle of the job, and auto tool zero at same coordinates, without jogging, its ok, but if i jog to another place ( more conveniant place to change tool ) then it zero x and y axis off the original part zero.
I havent done anything with the G80, as long as the drilling cycle was working perfect after i got the new driver...
And now its this out of size matter that grows grey hair on my head.. :)
kvadda
Your drilling cycle is not working perfect, you have to cancel that cycle before you do the profile cut, you need to cancel the drilling cycle before you start the next operation, or it can be out of position a G80 is needed at the end of the drilling cycle
N195 G00 Z2.54
N196 M09
N197 M05
N198 G53 Z0.
N199 G53 Y0.X0. ( you might want to try a X0. Here as well, so you know that all axes are returning to the correct position when finished)