Re: [CAD_CAM_EDM_DRO] emc g92

Hi Tom,

Are you running The Sherline version of EMC? I simply MUST have G92 for
touching off in X and Y, and also the tool length in Z. I'm currently
using my STEP4 controller, not EMC. I want to run Sherline's EMC, as
soon as I get it's machine running again!

I use G92 as Jon suggests to set X,Y and Z, but not IN the program, I do
it manually with MDI. Does EMI tolerate this? I don't currently do
tool changes in the program, I just make separate programs. I take it
you're using G92 to set Z 0.005 or whatever after the M06? Humm, maybe
I can incorporate something like that. Do you have a code snip?

I was thinking of putting in a dialog box that would automatically set
the 0.1" offsets for LL, UL, UR, LR for me.


Alan KM6VV


Tom Hubin wrote:

> Jon Elson wrote:
>
>>Tom Hubin wrote:
>>
>>
>>>I gave up on EMC and use TurboCnc primarily because I have found no way
>>>to reliably set the axis values from within a Gcode program.
>>>
>>>
>>
>>Maybe I should describe how I set up my tools on simple workpieces.
>>I lower the tool ontil it is almost touching the work. I then slip a piece
>>of paper that I know is .005" thick under the tool, and jog down until
>>the paper is pinched. I then right click on the Z axis and type .005
>>and hit the enter key. For X and Y, I use an edgefinder and jog over
>>until the edgefinder deflects to the side, then I stop the spindle (F9).
>>I right click on the axis, enter either .1 (the radius of the edgefinder)
>>or -.1, depending on which side of the part I'm on. Then, hit enter.
>>
>>If I'm doing something that requires changing tools several times, I can
>>put the offsets for the different tool lengths in the tool table, and set up
>>the program to select the right tool offset with G43 H(tool #).
>>
>>Jon
>
>
> ************************************************
>
> Hello Jon,
>
> I have seen no way to follow your procedure on a standard Sherline 5410
> (metric 5400) mill.
>
> I change drill chucks, drill bits, endmills, endmill holders, collets,
> etc. often within a Gcode program. I have no automatic tool changer. I
> have no way to control offsets.
>
> With TurboCnc the operator follows the prompted instructions and
> installs the specified bit in the appropriate chuck then jogs to barely
> contact the appropriate reference surface. When the program resumes it
> uses G92 to set the Z position to a useful and meaningful value.
>
> This may seem amateurish to somebody who has production type equipment
> but what I have is an amateur machine. The procedure I use with G92
> works very well with TurboCnc. There appears to be no way to automate to
> the same degree using EMC on a standard Sherline mill.
>
> Below is a typical program of mine which runs well with TurboCnc 3.1a.
> Some of my other Gcode programs use G92 to set Z to a nonzero value at
> the reference surface. The case you describe using a spacer to protect
> the finished surface would be one example of setting to a nonzero value.
>
> How would you do this (ignore the subroutine stuff) with EMC on a simple
> mill like my Sherline 5410 (one stepper motor for each of three axes,
> manual spindle on/off and speed control, no limit or home switches,
> common drill bits and endmills)?
>
> Why does the use of G92 in EMC cause unpredictable behaviour like
> crashing bits down into the workpiece or up to the top of the Z column?
> BTW, this does not happen when the G92 block itself is encountered. It
> happens when the program terminates with M02 if G92 is used somewhere
> within the program.
>
> Does anybody actually use G92 within a Gcode program using EMC? If so, I
> would like to see and run that Gcode program. If not, I suspect that is
> because G92 is dangerous because the EMC interpreter does things with
> G92 that no mere mortal can predict. Any Gcode instruction that requires
> experiments, observations, and a 20 page report on the results needs
> some work.
>
> Tom Hubin
> thubin@...
>
> **************************************
>
> M00 ; File: Cube05\Cage\Bottom\Drill.cnc 15 July 2004
>
> G90 ; absolute
> G70 ; inches
>
> M00 ; use approx 2.0 x 2.0 x 1.8 aluminum block
> M00 ; ref corner is (right, back, top) = (+1.0, +1.0, 0.0)
> M00 ; (0,0,0) is (center, center, top)
>
> ;**************************************************
>
> M00 ; Load medium center drill and touch surface
> G92 Z 0.0 ; define surface as z=0
> G00 Z 0.040 ; raise the bit
> M00 ; Tighten bit and start spindle 2800 RPM
>
> ; five 1/8" dowel holes
>
> G00 X +0.100 Y +0.800
> G81 X 0.000 Y +0.700 Z -0.040 R 0.040 F 2.0
>
> G00 X -0.600 Y +0.100
> G81 X -0.700 Y +0.000 Z -0.040 R 0.040 F 2.0
>
> G00 X +0.100 Y +0.100
> G81 X 0.000 Y +0.000 Z -0.040 R 0.040 F 2.0
>
> G00 X +0.800 Y +0.100
> G81 X +0.700 Y +0.000 Z -0.040 R 0.040 F 2.0
>
> G00 X +0.100 Y -0.600
> G81 X 0.000 Y -0.700 Z -0.040 R 0.040 F 2.0
>
> ; four tap 4-40 holes
>
> G00 X -0.49055 Y +0.69055
> G81 X -0.59055 Y +0.59055 Z -0.040 R 0.040 F 2.0
>
> G00 X +0.69055 Y +0.69055
> G81 X +0.59055 Y +0.59055 Z -0.040 R 0.040 F 2.0
>
> G00 X -0.49055 Y -0.49055
> G81 X -0.59055 Y -0.59055 Z -0.040 R 0.040 F 2.0
>
> G00 X +0.69055 Y -0.49055
> G81 X +0.59055 Y -0.59055 Z -0.040 R 0.040 F 2.0
>
> G00 Z +0.2 ; raise the bit
> G00 X +1.25 Y 0.0 ; position to change bits
>
> ;**************************************************
>
> M00 ; Load #43 (0.089 inch) drill and touch surface
> G92 Z 0.0 ; define surface as z=0
> G00 Z 0.040 ; raise the bit
> M00 ; Tighten bit and start spindle 2800 RPM
>
> ; four tap 4-40 holes
>
> G00 X -0.49055 Y +0.69055
> G82 X -0.59055 Y +0.59055 Z -0.175 R +0.040 F 8.473 #250
>
> G00 X +0.69055 Y +0.69055
> G82 X +0.59055 Y +0.59055 Z -0.175 R +0.040 F 8.473 #250
>
> G00 X -0.49055 Y -0.49055
> G82 X -0.59055 Y -0.59055 Z -0.175 R +0.040 F 8.473 #250
>
> G00 X +0.69055 Y -0.49055
> G82 X +0.59055 Y -0.59055 Z -0.175 R +0.040 F 8.473 #250
>
> G00 Z +0.2 ; raise the bit
> G00 X +1.25 Y 0.0 ; position to change bits
>
> ;**************************************************
>
> M00 ; Load 7/64 drill and touch surface
> G92 Z 0.0 ; define surface as z=0
> G00 Z 0.040 ; raise the bit
> M00 ; Tighten bit and start spindle 2800 RPM
>
> ; five 1/8" dowel holes
>
> G00 X +0.100 Y +0.800
> G82 X 0.000 Y +0.700 Z -0.114 R +0.040 F 10.412 #250
>
> G00 X -0.600 Y +0.100
> G82 X -0.700 Y +0.000 Z -0.114 R +0.040 F 10.412 #250
>
> G00 X +0.100 Y +0.100
> G82 X 0.000 Y +0.000 Z -0.114 R +0.040 F 10.412 #250
>
> G00 X +0.800 Y +0.100
> G82 X +0.700 Y +0.000 Z -0.114 R +0.040 F 10.412 #250
>
> G00 X +0.100 Y -0.600
> G82 X 0.000 Y -0.700 Z -0.114 R +0.040 F 10.412 #250
>
> G00 Z +0.2 ; raise the bit
> G00 X +1.25 Y 0.0 ; position to change bits
>
> ;**************************************************
>
> M00 ; Load 0.120" endmill and touch surface
> G92 Z 0.0 ; define surface as z=0
> G00 Z 0.040 ; raise the bit
> M00 ; Tighten bit and start spindle 2800 RPM
>
> ; five 1/8" dowel holes
>
> G00 X +0.100 Y +0.800
> G82 X 0.000 Y +0.700 Z -0.114 R +0.040 F 1.0 #250
>
> G00 X -0.600 Y +0.100
> G82 X -0.700 Y +0.000 Z -0.114 R +0.040 F 1.0 #250
>
> G00 X +0.100 Y +0.100
> G82 X 0.000 Y +0.000 Z -0.114 R +0.040 F 1.0 #250
>
> G00 X +0.800 Y +0.100
> G82 X +0.700 Y +0.000 Z -0.114 R +0.040 F 1.0 #250
>
> G00 X +0.100 Y -0.600
> G82 X 0.000 Y -0.700 Z -0.114 R +0.040 F 1.0 #250
>
> G00 Z +0.2 ; raise the bit
> G00 X +1.25 Y 0.0 ; position to change bits
>
> ;**************************************************
>
> M00 ; Load 0.1260" flat reamer and touch surface
> G92 Z 0.0 ; define surface as z=0
> G00 Z 0.040 ; raise the bit
> M00 ; Tighten bit and start spindle 400 RPM
>
> ; five 1/8" dowel holes
>
> G00 X +0.100 Y +0.800
> G81 X 0.000 Y +0.700 Z -0.114 R +0.040 F 12.0
>
> G00 X -0.600 Y +0.100
> G81 X -0.700 Y +0.000 Z -0.114 R +0.040 F 12.0
>
> G00 X +0.100 Y +0.100
> G81 X 0.000 Y +0.000 Z -0.114 R +0.040 F 12.0
>
> G00 X +0.800 Y +0.100
> G81 X +0.700 Y +0.000 Z -0.114 R +0.040 F 12.0
>
> G00 X +0.100 Y -0.600
> G81 X 0.000 Y -0.700 Z -0.114 R +0.040 F 12.0
>
> G00 Z +0.2 ; raise the bit
> G00 X +1.25 Y 0.0 ; position to change bits
>
> ;**************************************************
>
> M00 ; Load 3/32 inch endmill and touch surface
> G92 Z 0.0 ; define surface as z=0
> G00 Z 0.040 ; raise the bit
> M00 ; Tighten bit and start spindle 2800 RPM
>
> ; four tap 4-40 holes
>
> G00 X -0.49055 Y +0.69055
> G82 X -0.59055 Y +0.59055 Z -0.175 R +0.040 F 1.0 #250
>
> G00 X +0.69055 Y +0.69055
> G82 X +0.59055 Y +0.59055 Z -0.175 R +0.040 F 1.0 #250
>
> G00 X -0.49055 Y -0.49055
> G82 X -0.59055 Y -0.59055 Z -0.175 R +0.040 F 1.0 #250
>
> G00 X +0.69055 Y -0.49055
> G82 X +0.59055 Y -0.59055 Z -0.175 R +0.040 F 1.0 #250
>
> G00 Z +0.2 ; raise the bit
> G00 X +1.25 Y 0.0 ; position to change bits
>
> ;**************************************************
>
> M00 ; Load #4 thread mill and touch surface
> G92 Z 0.0 ; define surface as z=0
> G00 Z 0.2 ; raise the bit
> M00 ; Tighten bit and start spindle 2800 RPM
>
> ; four tap 4-40 holes
>
> G00 X -0.49055 Y +0.69055
> G00 X -0.59055 Y +0.59055
> N210 M60 #2000 ; thread mill helix
>
> G00 X +0.69055 Y +0.69055
> G00 X +0.59055 Y +0.59055
> N220 M60 #2000 ; thread mill helix
>
> G00 X -0.49055 Y -0.49055
> G00 X -0.59055 Y -0.59055
> N230 M60 #2000 ; thread mill helix
>
> G00 X +0.69055 Y -0.49055
> G00 X +0.59055 Y -0.59055
> N240 M60 #2000 ; thread mill helix
>
> G00 Z +0.2 ; raise the bit
> G00 X +1.25 Y 0.0 ; position to change bits
>
> ;**************************************************
>
> M02 ; finished program Cube05\Cage\Bottom\Drill.cnc
>
> ;**************************************************
>
> N2000 ; 0.080 inch threadmill helix for 4-40 holes
> G00 Z -0.165 ; start just above bottom of hole
>
> G91 ; start incremental mode
>
> G01 X -0.0160 F 1.0 ; move to left side of hole
> G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.015
> G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.040
> G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.065
> G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.090
> G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.115
> G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.140
> G73 X0 Y0 J0 I +0.0160 Z +0.025 ; helix to Z -0.165
> G01 X +0.0160 ; move to center of hole
>
> G90 ; restore absolute mode
>
> G00 Z +0.2 ; exit the hole
> M62 ; end of threadmill helix subroutine
>
>
>
> Addresses:
> FAQ: http://www.ktmarketing.com/faq.html
> FILES: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO/files/
> Post Messages: CAD_CAM_EDM_DRO@yahoogroups.com
>
> Subscribe: CAD_CAM_EDM_DRO-subscribe@yahoogroups.com
> Unsubscribe: CAD_CAM_EDM_DRO-unsubscribe@yahoogroups.com
> List owner: CAD_CAM_EDM_DRO-owner@yahoogroups.com, wanliker@..., timg@...
> Moderator: pentam@... indigo_red@... davemucha@... [Moderators]
> URL to this group: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO
>
> OFF Topic POSTS: General Machining
> If you wish to post on unlimited OT subjects goto: aol://5863:126/rec.crafts.metalworking or go thru Google.com to reach it if you have trouble.
> http://www.metalworking.com/news_servers.html
>
> http://groups.yahoo.com/group/jobshophomeshop I consider this to be a sister site to the CCED group, as many of the same members are there, for OT subjects, that are not allowed on the CCED list.
>
> NOTICE: ALL POSTINGS TO THIS GROUP BECOME PUBLIC DOMAIN BY POSTING THEM. DON'T POST IF YOU CAN NOT ACCEPT THIS.....NO EXCEPTIONS........
> bill
> List Mom
> List Owner
>
>
> Yahoo! Groups Links
>
>
>
>
>
>
>
>