I have a little bit of info here: http://gnipsel.com/linuxcnc/g-code/lathe02.html
JT On 6/25/2015 9:45 AM, Gene Heskett wrote: > > On Thursday 25 June 2015 06:42:55 John Thornton wrote: >> On my lathe I only touch off to fixture the Z axis and use the spindle >> face as my fixture. X is always touched off to the material in the >> tool table. I don't use the touch off buttons because I've added some >> PyVCP buttons to do the touch offs. >> >> Touch off to spindle face >> MDI_COMMAND = G10 L11 P#5400 Z0.0 >> Update the tool offset for chicken checks >> MDI_COMMAND = G43 >> Touch off Z to the material face with a 3/8" dowel >> MDI_COMMAND = G10 L20 P1 Z0.375 >> >> My basic procedure is to touch off Z to the spindle then if it makes >> sense for that tool cut and measure the od and touch off to the tool >> table that diameter. For drills I use an indicator to center the drill >> chuck and make that X0. >> >> JT > How to do that reliably when the drill is toolpost mounted has so far > escaped me John. But on my toy, I find the toolpost mounted drill is > far handier than the tailstock usage. My tailstock is a far far cry > from spindle aligned. Sideways (x offset) I can adjust, clumsily, but > up and down (call it y) is several degrees off axis and would need more > cast iron added to the castings to correct. > > So I put a small center drill in the chuck, hope it is sufficiently > aligned axially since the toolpost doesn't have a 90 degree lockdown > pin, then bring the drill to the face and diddle both x and y(toolpost > locking height) until it is well centered, then finish the pilot hole. > Change to a drill bit, discover the toolpost is a degree out of > alignment & turn it till the drill is aligned, then drill the starter > hole for the boring job. Needlessly complex, but works as long as the > drill is sharp enough that its backthrust doesn't cause the toolpost to > slip. Drill Doctor demanded to achieve that reliably. > > A tut on how you do it, on your web site, would get read and re-read by > this user. > >> On 6/24/2015 11:06 PM, Tom Easterday wrote: >>> For tool and work offsets on my mill I follow the advice given here: >>> http://wiki.linuxcnc.org/cgi-bin/wiki.pl?MillSetup >>> <http://wiki.linuxcnc.org/cgi-bin/wiki.pl?MillSetup> which in a >>> nutshell says: you set one tool (an edge finder perhaps) at a >>> specific point and then reference all tools (in length, ie. Z) to >>> that reference tool. So settings in my mill tool table have Z >>> values that are +/- the difference in length between the reference >>> tool and the given tool. >>> >>> I am trying to set up the tool table for a lathe and am having >>> problems. I see that the advice for doing this differs from what I >>> am doing above on my mill. So, I was trying to follow the advice in >>> section 21.4 of the Linuxcnc User Manual: >>> http://www.linuxcnc.org/docs/2.7/pdf/LinuxCNC_User_Manual.pdf >>> <http://www.linuxcnc.org/docs/2.7/pdf/LinuxCNC_User_Manual.pdf> >>> >>> I have the Z offsets in the tool table and that part seems to be >>> working. However, I am having problems getting the X offsets to >>> work (even though i think i am doing exactly the same thing as Z). >>> I set the X offset by doing this: >>> >>> In MDI issue: T1 M6 G43 >>> Turned down some stock to 0.55” >>> Select “Touch off to fixture” in Machine menu >>> Make sure X is the selected radio button >>> Select “Touch off Tool” button (This button is new in Axis in 2.7 I >>> think?) (Bug? in 2.7.0~pre6 - the dialog for this button refers to >>> Workpiece not Fixture) Enter 0.275 (yes, I entered a positive number >>> even though my tool is above the spindle centerline - is that >>> correct?) >>> >>> In the tool table I get an X value that basically looks like a >>> distance from G53 X0 (something like 1.XXXX). >>> >>> Then to enter a second tool: >>> In MDI issue: T8 M6 G43 (This is a 0.25” drill) >>> Bring it down to touch the top of a 0.100” pin which is on top of my >>> 0.55” workpiece Select “Touch off to fixture” in Machine menu >>> Make sure X is the selected radio button >>> Select “Touch off Tool” button >>> Enter 0.275 + 0.100 + 0.125 = 0.5 (yes, I entered a positive number >>> even though my tool is above the spindle centerline - is that >>> correct?) >>> >>> In the tool table, again, I get an X value that basically looks like >>> a distance from G53 X0. >>> >>> When I go back to tool T1 (T1 M6 G43) and then issue a G0 X0 the >>> tool goes to the center of the spindle as it should. >>> >>> But, if I return to tool T8 (T8 M6 G43) and issue a G0 X0 the drill >>> does not go to the center of the spindle. And it’s distance away is >>> not any of the measurements above, in other words I can’t figure out >>> where I went wrong. >>> >>> Perhaps I should just be following the procedure I used on the mill >>> and just forget about “Touch off to fixture” and “Touch off Tool” >>> and enter values +/- of the reference tool? >>> >>> I am quite confused at this point. I have looked at JT’s tutorials, >>> and all the Linuxcnc manuals and other random documents that talk >>> about this, but every time I think I understand and try the >>> procedure I get the wrong result. By the way, I have entered the >>> ORIENTATION and the FRONT and BACK ANGLES in the tool table for >>> these tools, could those things (if I happened to enter them >>> incorrectly) effect the X offset? >>> >>> -Tom > Cheers, Gene Heskett ------------------------------------------------------------------------------ Monitor 25 network devices or servers for free with OpManager! OpManager is web-based network management software that monitors network devices and physical & virtual servers, alerts via email & sms for fault. Monitor 25 devices for free with no restriction. Download now http://ad.doubleclick.net/ddm/clk/292181274;119417398;o _______________________________________________ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
