Re: [Emc-users] tool length compensation
Stuart Stevenson wrote: Gentlemen, I am installing EMC2 on a Cincinatti 5 axis. This is sooner than I had planned. The timeframe is compressed. I work good under pressure. It is usually caused by procrastination (mine). This is not the case this time. I need to get the machine running by Friday of next week. Any and all help/comments/opinions will be greatly appreciated. Wow, that is sudden. Which Cinci? Did the control die on blue or green? Or are you putting the brown one back together? Regards, John Kasunich - This SF.net email is sponsored by: Microsoft Defy all challenges. Microsoft(R) Visual Studio 2008. http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] tool length compensation
On Fri, Feb 29, 2008 at 04:04:51PM -0600, Chris Radek wrote: The actual difference with the 5 axis kinematics machine is that you should specify [TRAJ]TLO_IS_ALONG_W=1. Then when you use G43 H_ or G43.1 K___, the length offset, no matter whether it comes from the tool table (G43) or gcode (G43.1), is applied to the W axis. The only thing your cam needs to do is move the W axis (G0 W0) so the length offset gets applied. I wanted to add this for non-5-axis folks: This new option of TLO along W doesn't need special kinematics or 5 axis machinery or anything else special. If you have a CNC knee on your knee mill, and you call it W, you could just as easily use it for tool length compensation. This would give you full quill travel no matter the length of the tool. Very neat. Chris - This SF.net email is sponsored by: Microsoft Defy all challenges. Microsoft(R) Visual Studio 2008. http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] tool length compensation
Hi Dynamics tool length compensation for 5 axis in 3D world much complicated. First, tool compensation for 2 axis include touch with probe corner of the table and controller calculated rotation only one axis B that touch table with probe to define Z and it will compensate to tool length. For 5 axis need move axis B, C or A, to make targeted surface perpendicular to the probe and than everything same as for 2 axis routine for tool length compensation. Thanks Aram On Fri, Feb 29, 2008 at 02:51:20PM -0600, Stuart Stevenson wrote: Gentlemen, I am installing EMC2 on a Cincinatti 5 axis. This is sooner than I had planned. The timeframe is compressed. I work good under pressure. It is usually caused by procrastination (mine). This is not the case this time. I need to get the machine running by Friday of next week. Any and all help/comments/opinions will be greatly appreciated. The 5 axis tool length compensation is implemented with G43.1 instead of G43. This is no problem whatsoever. This is like the Fanuc and Haas controls. I would like to use the H number from the tool.tbl file with the G43.1 in the same manner as the H number with the G43. I grepped the directory and didn't find any reference to how the G43 and G43.1 were implemented. Where would I find the code to change the usage? thanks Stuart You misunderstand how G43/G43.1 work. They do not work differently for multiaxis machines. The tool table works as usual with G43 H_. G43.1 lets you specify the length directly in the gcode (G43.1 K___) and it sounds like you will not use this. The actual difference with the 5 axis kinematics machine is that you should specify [TRAJ]TLO_IS_ALONG_W=1. Then when you use G43 H_ or G43.1 K___, the length offset, no matter whether it comes from the tool table (G43) or gcode (G43.1), is applied to the W axis. The only thing your cam needs to do is move the W axis (G0 W0) so the length offset gets applied. Chris - This SF.net email is sponsored by: Microsoft Defy all challenges. Microsoft(R) Visual Studio 2008. http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users - This SF.net email is sponsored by: Microsoft Defy all challenges. Microsoft(R) Visual Studio 2008. http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] tool length compensation
You misunderstand how G43/G43.1 work. They do not work differently for multiaxis machines. The tool table works as usual with G43 H_. G43.1 lets you specify the length directly in the gcode (G43.1 K___) and it sounds like you will not use this. The actual difference with the 5 axis kinematics machine is that you should specify [TRAJ]TLO_IS_ALONG_W=1. Then when you use G43 H_ or G43.1 K___, the length offset, no matter whether it comes from the tool table (G43) or gcode (G43.1), is applied to the W axis. The only thing your cam needs to do is move the W axis (G0 W0) so the length offset gets applied. Chris (snip) On Fri, Feb 29, 2008 at 04:04:51PM -0600, Chris Radek wrote: The actual difference with the 5 axis kinematics machine is that you should specify [TRAJ]TLO_IS_ALONG_W=1. Then when you use G43 H_ or G43.1 K___, the length offset, no matter whether it comes from the tool table (G43) or gcode (G43.1), is applied to the W axis. The only thing your cam needs to do is move the W axis (G0 W0) so the length offset gets applied. I wanted to add this for non-5-axis folks: This new option of TLO along W doesn't need special kinematics or 5 axis machinery or anything else special. If you have a CNC knee on your knee mill, and you call it W, you could just as easily use it for tool length compensation. This would give you full quill travel no matter the length of the tool. Very neat. Chris Chris, You are correct. I didn't understand. I do now. Your way is the way it should be done. The Fanuc and Haas machines use the tool length in the tool table but then for 5 axis tool length compensation they need to use G43.1 (Fanuc) and G143 (Haas). I have never understood why the need to have two different codes, they work the same. If the machine will do 5 axis tool length compensation it will do 3 axis compensation with the same G code. The only difference is you will need to begin using a positive tool length offset for all your tool lengths. It is easy once you get used to it. Thanks for the explanation. I am in the middle of changing the kinematics file to handle the mechanics of the Cinci's. I will also implement the geometric compensation I talked about. This will tell me for sure if it is working correctly. I know it is working. I am confident it is correct but I don't KNOW it is correct. thanks Stuart ps. sorry for the incorrect subject in my previous reply - This SF.net email is sponsored by: Microsoft Defy all challenges. Microsoft(R) Visual Studio 2008. http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] tool length compensation
On Fri, 29 Feb 2008, Chris Radek wrote: On Fri, Feb 29, 2008 at 04:04:51PM -0600, Chris Radek wrote: The actual difference with the 5 axis kinematics machine is that you should specify [TRAJ]TLO_IS_ALONG_W=1. Then when you use G43 H_ or G43.1 K___, the length offset, no matter whether it comes from the tool table (G43) or gcode (G43.1), is applied to the W axis. The only thing your cam needs to do is move the W axis (G0 W0) so the length offset gets applied. I wanted to add this for non-5-axis folks: This new option of TLO along W doesn't need special kinematics or 5 axis machinery or anything else special. If you have a CNC knee on your knee mill, and you call it W, you could just as easily use it for tool length compensation. This would give you full quill travel no matter the length of the tool. Very neat. Now you've got me confused a bit. I thought that UVW were cartesian vectors parallel/orthogonal to the tool orientation vector. For example, if your tool axis is parallel to the Z vector then W would also be parallel to Z. But if the tool tip is rotated in A then W would be rotated in A as well. So what gives? Is W simply a reference to a joint when using a trivial kinematics machine? If so, then does the behavior change dramatically when we add a trunion table to our knee mill? Will the real W please stand up! warning: the following may contain ostentatious pedantry not suitable for miners, spoken-word poets, politicians, and other heathen peoples I propose that we use the term vector to refer to a mathematical entity defining a space, (as in basis vector), joint for constrained moving physical assemblies, and axis as a straight line along which some physical object travels or rotates about. This allows a space defined by X, Y and Z vectors, but one can also have a physical joint named the Z axis if there is a linear joint that is always parallel to the Z vector. If there are two linear joints always parallel to the Z vector then it doesn't make sense to call one of them the Z axis and not the other one. You cannot have a rotary table named the C axis if the location of the center of rotation changes, for example if you have moved the tool tip, or if you define the origin to be in a location that is not centered on the axis of the rotary table, which is pretty much always. The part program MUST specify whether it represents vector coordinates (g91z1 means move the tool tip? perpendicular to the work plane) or joint coordinates (g91z1 means retract the quill) and right now RS274NGC doesn't specify which, at least from my understanding. How does one get a herd of cats to speak the same language? I'd appreciate feedback on this, since we tend to take for granted that the person on the receiving end understands what we mean. Sometimes their definitions are a little different and one can appear to them to be saying something different than what we actually meant. We have all these words available from our mathematical heritage, but someone in the early days of EMC decided that Joint and Axis were the only words to use. This hasn't been working so well in actuality, since most people aren't aware of this idealized usage of the terms; they already have meaning (different meanings!) in similar contexts outside of the EMC project. But in addition to that, the words have been used imprecisely throughout EMC's code and documentation. So now there is a mess, and we have to clean up not just the code but our thoughts as well. work harder, work smarter, and do the right thing! (in order of increasing importance) -fenn - This SF.net email is sponsored by: Microsoft Defy all challenges. Microsoft(R) Visual Studio 2008. http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] tool length compensation
Gentlemen, I have been thinking again today. Does EMC have G44, G45, G46, G47 and G48? I just looked at a page explaining these for Fanuc controls. The page explains them different than I remember. My memory says the: G43 is tool length compensation positive in the Z axis G44 is tool length compensation negative in the Z axis G45 is tool length compensation positive along the X or Y axis G46 is tool length compensation negative along the X or Y axis G47 is tool length compensation positive along the other of the X or Y axes G48 is tool length compensation negative along the other of the X or Y axes G49 is tool length compensation cancel for all tool length compensation codes This allows the drill cycles to be usable after a plane shift using G18 or G19. I remember using this only one time ever for drilling. Not a very useful tool in my experience. But, if the G43 tool length compensation is usable at ALL angles and the drill cycles function at all angles this is another matter. I know of NO machine tool with this capability. I know of NO machine controller with this capability. There certainly are controllers with the horsepower to do so and maybe there are some that have that implemented but I know of none. The capability of using the drill cycles at all angles in a program AND MDI would be a KILLER function. A slightly positive addition to the G43 usable at all angles is that would eliminate the need for the G44 through G48 codes. Another huge positive the G43 tool length compensation at all angles gives is true 5 axis tool tip programming. The capability to store the pivot length of the machine and use the tool table for the tool lengths allows progress toward using a CL (Cutter Location) file to directly control the machine. CL file are output out of a myriad of CAM systems. The CL file has POST words such as COOLANT ON. If EMC would read those statements then a CL file would control the machine. If a CL file can control a machine then the CAM system output can be sent directly to the machine bypassing the CL file and the CAM system would then directly control the machine. A CL file contains the I, J and K components of the tool axis vector. This would allow EMC to directly use those numbers rather than calculating them from the A, B and C values in the G code program. At this time the ability to control the machine directly with a CAM system seems scary. But, with the capability comes education and then usefulness. This would be a long way toward enabling the seemingly stuck STEP-NC. Sending the output of a CAM system to the controller instead of an intermediate file would be another KILLER function. I see immediate usefulness with the current capability. I will be replacing the Fanuc 15MB control on my 5 axis bridge ASAP. If anyone wants to see an example of what I am talking about you only need to update EMC and run the 5axis machine sim. Notice how the numbers on the screen are the same numbers regardless of the tool length. Also notice the X, Y and Z numbers would be the same numbers if the program was run in 3 axis mode. Chris Radek has enabled 5 axis tool length compensation and included the pivot length in the kinematics. VERY VERY COOL Comments? Suggestions? Criticisms? Chris - thank you very much Stuart - This SF.net email is sponsored by: Microsoft Defy all challenges. Microsoft(R) Visual Studio 2005. http://clk.atdmt.com/MRT/go/vse012070mrt/direct/01/ ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
