Re: [Emc-users] G83 Bug in Lathe Mode?
On 16 March 2010 00:23, Steve Blackmore st...@pilotltd.net wrote: The reason for the G18 was to make G2 and G3 work in other parts of the code. G18 means canned-cycle movement in Y, so it is an error to use G18 and a canned cycle with a lathe. Huhhh??? G83 includes both movement (in the specified plane) to a position and then a drilling cycle. If G18 is programmed then the initial movement is in the XZ plane followed by a peck-drill movement in the Y axis. Makes no sense whatsoever to program G17 when you are working in XZ plane? In some ways, no. But then G17 only mentions the Y axis in the documentation/description. It also indicates which axis is to be used for the canned-cycle movement and a change to the description text would fix the apparent nonsensicality. With a lathe G83 could equally well be used for peck-drilling holes in the end of the work with a drill in the toolpost (my current usage) but it also seems very well suited to peck-parting work in which case the movement would be in the X axis. There needs to be some way to tell EMC which one you want, and G17/18/19 do seem like the most compliant way to do that. One proposal that has occurred to me would be to add G18.1 and G18,3, both mean that arcs are to be created in the XZ plane, with G18.1 indicating canned-cycle movements in the X axis and G18.3 in the Z (G18.2 would be movement in Y, perhaps a cut-off slide or drilling head) This proposal would mean that G81.3 could be programmed at the beginning and then all conventional lathe-turning operations would work as expected. -- atp -- Download Intel#174; Parallel Studio Eval Try the new software tools for yourself. Speed compiling, find bugs proactively, and fine-tune applications for parallel performance. See why Intel Parallel Studio got high marks during beta. http://p.sf.net/sfu/intel-sw-dev ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] G83 Bug in Lathe Mode?
Makes no sense whatsoever to program G17 when you are working in XZ plane? In some ways, no. But then G17 only mentions the Y axis in the documentation/description. It also indicates which axis is to be used for the canned-cycle movement and a change to the description text would fix the apparent nonsensicality. With a lathe G83 could equally well be used for peck-drilling holes in the end of the work with a drill in the toolpost (my current usage) but it also seems very well suited to peck-parting work in which case the movement would be in the X axis. There needs to be some way to tell EMC which one you want, and G17/18/19 do seem like the most compliant way to do that. One proposal that has occurred to me would be to add G18.1 and G18,3, both mean that arcs are to be created in the XZ plane, with G18.1 indicating canned-cycle movements in the X axis and G18.3 in the Z (G18.2 would be movement in Y, perhaps a cut-off slide or drilling head) This proposal would mean that G81.3 could be programmed at the beginning and then all conventional lathe-turning operations would work as expected. we already have G17.1/G18.1/G19.1 and they are explicitly the planes UV/WU/VW Regards, Alex -- Download Intel#174; Parallel Studio Eval Try the new software tools for yourself. Speed compiling, find bugs proactively, and fine-tune applications for parallel performance. See why Intel Parallel Studio got high marks during beta. http://p.sf.net/sfu/intel-sw-dev ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] G83 Bug in Lathe Mode?
On 16 March 2010 10:28, Alex Joni alex.j...@robcon.ro wrote: This proposal would mean that G81.3 could be programmed at the beginning and then all conventional lathe-turning operations would work as expected. we already have G17.1/G18.1/G19.1 and they are explicitly the planes UV/WU/VW Sorry, I really should have checked first. I guess I should stop trying to be lazy then, and just program a G17 before a G83 and a G18 before a G2 or G3. -- atp -- Download Intel#174; Parallel Studio Eval Try the new software tools for yourself. Speed compiling, find bugs proactively, and fine-tune applications for parallel performance. See why Intel Parallel Studio got high marks during beta. http://p.sf.net/sfu/intel-sw-dev ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] G83 Bug in Lathe Mode?
Sorry, I really should have checked first. I guess I should stop trying to be lazy then, and just program a G17 before a G83 and a G18 before a G2 or G3. dont forget M30 etc will cancel planes back to G18, as well as cancel feed per rev etc, so you always have to defind your plane at the program start etc rob -- Download Intel#174; Parallel Studio Eval Try the new software tools for yourself. Speed compiling, find bugs proactively, and fine-tune applications for parallel performance. See why Intel Parallel Studio got high marks during beta. http://p.sf.net/sfu/intel-sw-dev ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] G83 Bug in Lathe Mode?
On Tue, 16 Mar 2010 10:18:11 +, you wrote: On 16 March 2010 00:23, Steve Blackmore st...@pilotltd.net wrote: The reason for the G18 was to make G2 and G3 work in other parts of the code. G18 means canned-cycle movement in Y, so it is an error to use G18 and a canned cycle with a lathe. Huhhh??? G83 includes both movement (in the specified plane) to a position and then a drilling cycle. If G18 is programmed then the initial movement is in the XZ plane followed by a peck-drill movement in the Y axis. Makes no sense whatsoever to program G17 when you are working in XZ plane? In some ways, no. But then G17 only mentions the Y axis in the documentation/description. It also indicates which axis is to be used for the canned-cycle movement and a change to the description text would fix the apparent nonsensicality. With a lathe G83 could equally well be used for peck-drilling holes in the end of the work with a drill in the toolpost (my current usage) but it also seems very well suited to peck-parting work in which case the movement would be in the X axis. There needs to be some way to tell EMC which one you want, and G17/18/19 do seem like the most compliant way to do that. One proposal that has occurred to me would be to add G18.1 and G18,3, both mean that arcs are to be created in the XZ plane, with G18.1 indicating canned-cycle movements in the X axis and G18.3 in the Z (G18.2 would be movement in Y, perhaps a cut-off slide or drilling head) This proposal would mean that G81.3 could be programmed at the beginning and then all conventional lathe-turning operations would work as expected. There should be no need whatsoever for all that added .1 stuff. Programming G17 G2 or G18 G2 should do the arc in the respective plain, end of story. Canned cycles should be treated similar. For example - Here's how Mach does peck drilling. For mill mode the retract plane is assumed to be perpendicular to the axis of the currently selected plane, ie Z for XY plane, Y for XZ plane and X for YZ plane. For Turn mode the R plane is assumed to be along the X axis unless you tell it otherwise. Retract plane direction can be overridden with G17, G18, G19. This code applies to turn, and is similar for mill with the addition of a Y parameter. 1) G83ZzzXxxRrrQqq The Q is peck distance, the R is retract distance, and Z and X are obvious. X is assumed to be zero if not on the line. If set, it will drill at that X, but be warned its a dual axis move to the X,Z start coordinate. 2) G83.1ZzzXxxRrrQqq This is a faster peck cycle, the drill will retract only the Q distance on each peck. You will end out at either R plane or the original starting point on the Z depending on the G98 or G99 in effect. G83ZzzXxx Rrr QqqG99 will end up at the original Z plane, G98 will end up at the retract R plane. This is true of both the high speed peck as well as the G83 R plane drill cycle.. G98 and G99 are canned cycle return modes, G99 will take you in the retract plane at the distance indicated after the R word, G98 will take you in the retract plane to the position you were in before the canned cycle started. Mach also supports G81 - plain drilling and G82 Drill with dwell. Steve Blackmore -- -- Download Intel#174; Parallel Studio Eval Try the new software tools for yourself. Speed compiling, find bugs proactively, and fine-tune applications for parallel performance. See why Intel Parallel Studio got high marks during beta. http://p.sf.net/sfu/intel-sw-dev ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] G83 Bug in Lathe Mode?
On Tue, Mar 16, 2010 at 6:52 AM, Steve Blackmore st...@pilotltd.net wrote: There should be no need whatsoever for all that added .1 stuff. Let's say you have a machine with a tool that can point in a direction other than perpendicular to one of the orthogonal planes. Let's say you want to drill a hole along the tool axis. Or let's say you want to mill a circle perpendicular to the current tool axis. G17.1 will allow that where G17 will allow the motion only in relation to the XY plane. G17 and G17.1, etc, allow the programmer/machinist to specify the machining conditions/parameters as necessary to control the machine as desired. I think it is a good thing. thanks Stuart -- dos centavos -- Download Intel#174; Parallel Studio Eval Try the new software tools for yourself. Speed compiling, find bugs proactively, and fine-tune applications for parallel performance. See why Intel Parallel Studio got high marks during beta. http://p.sf.net/sfu/intel-sw-dev ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] G83 Bug in Lathe Mode?
Running this code gives me the error Y value unspecified in xz plane canned cycle Which is a bit of a surprise given that the machine is a lathe (and LATHE = 1) Replacing the G18 with G17 fixes the problem, but seems a bit counter-intuitive. ;Test G7 ; Lathe Diameter Mode G18 ; XZ Plane G21 ; Metric Units G90 ; Absolute Distance ;Drilling g0 x0 G97 M3 S800 G98 G83 R0.5 Z-6 Q3 M2 -- atp -- Download Intel#174; Parallel Studio Eval Try the new software tools for yourself. Speed compiling, find bugs proactively, and fine-tune applications for parallel performance. See why Intel Parallel Studio got high marks during beta. http://p.sf.net/sfu/intel-sw-dev ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] G83 Bug in Lathe Mode?
On 15 March 2010 22:05, Andy Pugh a...@andypugh.fsnet.co.uk wrote: Running this code gives me the error Y value unspecified in xz plane canned cycle Which is a bit of a surprise given that the machine is a lathe (and LATHE = 1) Replacing the G18 with G17 fixes the problem, but seems a bit counter-intuitive. Chris has explained why this is on IRC, but I am still not convinced it makes sense. The reason for the G18 was to make G2 and G3 work in other parts of the code. G18 means canned-cycle movement in Y, so it is an error to use G18 and a canned cycle with a lathe. However, it also doesn't seem to make any real sense to program G17 (X,Y plane) on a machine which doesn't even have a Y axis. I might have argued that G83 etc are unambiguous on a lathe, but I suppose in principle you could use it as a peck-parting cycle in X. So I don't know what the answer is, but being asked to specify a Y value for a machine with no Y axis certainly isn't the clearest error message and changing planes on a single-plane machine seems unintuitive. -- atp -- Download Intel#174; Parallel Studio Eval Try the new software tools for yourself. Speed compiling, find bugs proactively, and fine-tune applications for parallel performance. See why Intel Parallel Studio got high marks during beta. http://p.sf.net/sfu/intel-sw-dev ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] G83 Bug in Lathe Mode?
On Mon, 15 Mar 2010 22:46:02 +, you wrote: On 15 March 2010 22:05, Andy Pugh a...@andypugh.fsnet.co.uk wrote: Running this code gives me the error Y value unspecified in xz plane canned cycle Which is a bit of a surprise given that the machine is a lathe (and LATHE = 1) Replacing the G18 with G17 fixes the problem, but seems a bit counter-intuitive. Chris has explained why this is on IRC, but I am still not convinced it makes sense. The reason for the G18 was to make G2 and G3 work in other parts of the code. G18 means canned-cycle movement in Y, so it is an error to use G18 and a canned cycle with a lathe. Huhhh??? However, it also doesn't seem to make any real sense to program G17 (X,Y plane) on a machine which doesn't even have a Y axis. I might have argued that G83 etc are unambiguous on a lathe, but I suppose in principle you could use it as a peck-parting cycle in X. Makes no sense whatsoever to program G17 when you are working in XZ plane? I know that Mach has two distinct sets of code for things like canned cycles, one for mill and one for turn. I know that to be fact as I worked with Art correcting the existing Mill ones to work correctly in Turn. Perhaps it's being fudged to avoid writing more code? Steve Blackmore -- -- Download Intel#174; Parallel Studio Eval Try the new software tools for yourself. Speed compiling, find bugs proactively, and fine-tune applications for parallel performance. See why Intel Parallel Studio got high marks during beta. http://p.sf.net/sfu/intel-sw-dev ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
