Re: [Emc-users] Tool table, setting up offsets with a caliper
On Wed, 08 Sep 2010 22:22 -0700, Speaker To-Dirt speaker_2_d...@yahoo.com wrote: For what it's worth. I stumbled across this by accident. At a tool change take your tool to an area where there's still a surface z0.000. End the move with z1.000. Remove the tool, and insert the new tool. Now use a clamp arm from your clamp kit that is 1 on a side. Raise or lower the knee until your tool is just touching the upper surface of your clamp arm. You're now indexed 1.00x inches above your work. Be careful with this. Clamps sets are not precision items. If you measure your 1 thick clamps with a micrometer, I wouldn't be at all surprised to find that one clamp is 1.004, and another is 0.998. I'd only be a little surprised to find that a single clamp is 1.001 at one end and 1.003 on the other end. A dowel pin works great for this - very precise, and you can simply push it against the side of the tool, then raise the tool (or lower the knee) slowly until the pin rolls under. Don't lower the tool onto the dowel (or a clamp, or any other piece of metal). It doesn't take much to chip the edge of a carbide tool, or dull a steel one. John Kasunich -- John Kasunich jmkasun...@fastmail.fm -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper
On 9 September 2010 15:52, John Kasunich jmkasun...@fastmail.fm wrote: A dowel pin works great for this - very precise, and you can simply push it against the side of the tool, then raise the tool (or lower the knee) slowly until the pin rolls under. I think I have just found a use for the shank of the 6mm carbide milling cutter I broke. -- atp -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
On 7 September 2010 16:50, Igor Chudov ichu...@gmail.com wrote: So say I touch off with one tool from tool table, then switch tool to my desired cutting tool, and the cutting tool would automagically be adjusted vertically to compensate for difference in offsets between the cutting tool and the tool I used to touch off Z. My understanding is that you can set the tool lengths in the tool-table from any convenient reference on the tooholders, as long as that is consistent. Best of all might be to measure the tool in-situ to the spindle face, because that compensates for taper diameter variations leading to the holders settling in different positions. Of course, one way to then measure the tools is using the axis screw, ie by using the touch-off option. With a tool loaded, and assuming an accurate tool table, you should be able to then touch-off the work or fixture into a coordinate system using any tool, as the tool offset from the table is part of the calculation. (At least i very much hope it is, otherwise that way lies madness :-) Rather than use a spare holder with a dowel in, I think you could use a solid face of a specific holder to zero your height gauge, and still use that holder for tools. A measuring fixture (a dummy spindle nose) sounds like something well worth having. Ideally this needs to contact the holder where the spindle does, not on a flange (though that would be a lot easier) -- atp -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
Igor, The whole point of tool length offsets is to run the program as if all tools are the same length. Early NC machines had the tool length incorporated in the program and the operator had to match each tool length to the programmed tool length for each tool. There were elaborate tool holders to be able to adjust the tool length. How you get there is not important. Repeating yourself is important. I like positive values in tool length compensation as this makes 3 axis, 4 axis and 5 axis machines appear (and setup and adjust) the same to operators. Many people prefer negative tool length offsets as this causes the tool to move Z positive when the tool length offset is canceled. If you have only 3 axis machines then negative offsets are usually safer and easier. You can use tool length offsets in several ways. The best way to determine your preferred method is to experiment with tool length offsets and work coordinate settings (g54 - g59). This can give you a very comfortable, fast method to set up your machine. There is no ONE best way for everyone. I prefer using a repeatable spot on the table and a known tool set device. I have a 1/2 dowel in my pocket (have had for many years). This is my tool set device. I roll it under the tool while moving the tool up incrementally. When it slips through you know you are within the increment setting of the surface you are setting zero from. I like to use the same spot on the table for all tools and setups. I use g54 offsets to then move the Z zero point from the top of the setting surface to whatever zero setting the program requires. have fun Stuart -- dos centavos -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
Stuart, thanks. Great explanation. I already set up a little tool table. One more question, is, once I set up the tool table, how to set the initial offset so that the first tool chosen in the program, would be properly adjusted for height. Should I select my first tool in MDI (say M6T2), and then set G54 coordinate, and then run the program where M6T2 is stated again? - Igor On Wed, Sep 8, 2010 at 8:05 AM, Stuart Stevenson stus...@gmail.com wrote: Igor, The whole point of tool length offsets is to run the program as if all tools are the same length. Early NC machines had the tool length incorporated in the program and the operator had to match each tool length to the programmed tool length for each tool. There were elaborate tool holders to be able to adjust the tool length. How you get there is not important. Repeating yourself is important. I like positive values in tool length compensation as this makes 3 axis, 4 axis and 5 axis machines appear (and setup and adjust) the same to operators. Many people prefer negative tool length offsets as this causes the tool to move Z positive when the tool length offset is canceled. If you have only 3 axis machines then negative offsets are usually safer and easier. You can use tool length offsets in several ways. The best way to determine your preferred method is to experiment with tool length offsets and work coordinate settings (g54 - g59). This can give you a very comfortable, fast method to set up your machine. There is no ONE best way for everyone. I prefer using a repeatable spot on the table and a known tool set device. I have a 1/2 dowel in my pocket (have had for many years). This is my tool set device. I roll it under the tool while moving the tool up incrementally. When it slips through you know you are within the increment setting of the surface you are setting zero from. I like to use the same spot on the table for all tools and setups. I use g54 offsets to then move the Z zero point from the top of the setting surface to whatever zero setting the program requires. have fun Stuart -- dos centavos -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
On 8 September 2010 14:20, Igor Chudov ichu...@gmail.com wrote: Should I select my first tool in MDI (say M6T2), Don't forget the G43... -- atp -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
the g43 is the important part you need to turn on the tool length offset for the tool in the spindle and then the tool will be able to set the work piece coordinate zero On Wed, Sep 8, 2010 at 8:26 AM, Andy Pugh a...@andypugh.fsnet.co.uk wrote: On 8 September 2010 14:20, Igor Chudov ichu...@gmail.com wrote: Should I select my first tool in MDI (say M6T2), Don't forget the G43... -- atp -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- dos centavos -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
Got it. Do in MDI: M6 T2 G43 (then set height using a sliding gage block) (then set Z=zero) (then start program that again asks for T2.) - Igor On Wed, Sep 8, 2010 at 9:20 AM, Stuart Stevenson stus...@gmail.com wrote: the g43 is the important part you need to turn on the tool length offset for the tool in the spindle and then the tool will be able to set the work piece coordinate zero On Wed, Sep 8, 2010 at 8:26 AM, Andy Pugh a...@andypugh.fsnet.co.uk wrote: On 8 September 2010 14:20, Igor Chudov ichu...@gmail.com wrote: Should I select my first tool in MDI (say M6T2), Don't forget the G43... -- atp -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- dos centavos -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
looks good On Wed, Sep 8, 2010 at 9:25 AM, Igor Chudov ichu...@gmail.com wrote: Got it. Do in MDI: M6 T2 G43 (then set height using a sliding gage block) (then set Z=zero) (then start program that again asks for T2.) - Igor On Wed, Sep 8, 2010 at 9:20 AM, Stuart Stevenson stus...@gmail.com wrote: the g43 is the important part you need to turn on the tool length offset for the tool in the spindle and then the tool will be able to set the work piece coordinate zero On Wed, Sep 8, 2010 at 8:26 AM, Andy Pugh a...@andypugh.fsnet.co.uk wrote: On 8 September 2010 14:20, Igor Chudov ichu...@gmail.com wrote: Should I select my first tool in MDI (say M6T2), Don't forget the G43... -- atp -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- dos centavos -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- dos centavos -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
On 8 September 2010 15:25, Igor Chudov ichu...@gmail.com wrote: (then start program that again asks for T2.) Maybe practice on polystyrene foam... -- atp -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
For tool measurements off the taper of the holder, for cat 40 and cat 50 at least it should be easy to even purchase blocks to use on the surface plate with a height gage. Every place I worked at had some, so I never had to source out. If this is available for your tool holders it provides nice consistent measurements. Simplicity over a matching ring on blocks would be my thought here. Both work the same in the end, less parts to keep clean and together would make things more convenient. Now if you mount this to a plate and make a bar with grooves 1 apart wide enough to to hold an arm that positions a micrometer spindle over the center of the tools, you have a nice presetter. The grooves counted get you the inches, the micrometer head the decimals. This is nice for shop use if you want to keep surface plate and height gage out of the shop. Below is a i think this would work in emc2 (don't have a running emc2 machine yet) If you touch work offset with one of the tools measured in such a presetter, you should be able to relate the presetter numbers with emc2. As the delta between the tools would be the same, as long as the control knows where Z0 is with one of the tools, it would know it for the rest. We use this and it works perfect until we have someone flip numbers and rapid into the part. And still, the benefit of setting up tools for the next job, while the machine runs, always pays off. We made a program that runs each tool .005 over a 2 touch probe. If it lights up, check tool length, it's at least preventing crashes, easier to rerun to cut more than to add material. ;) Hope any of this is of use to you. On Sep 8, 2010 9:51 AM, Andy Pugh a...@andypugh.fsnet.co.uk wrote: On 8 September 2010 15:25, Igor Chudov ichu...@gmail.com wrote: (then start program that again ... Maybe practice on polystyrene foam... -- atp -- This SF.net Dev2... -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper
For what it's worth. I stumbled across this by accident. At a tool change take your tool to an area where there's still a surface z0.000. End the move with z1.000. Remove the tool, and insert the new tool. Now use a clamp arm from your clamp kit that is 1 on a side. Raise or lower the knee until your tool is just touching the upper surface of your clamp arm. You're now indexed 1.00x inches above your work. Andrew -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper
Your knee is your tool offset table. On Thu, Sep 9, 2010 at 12:22 AM, Speaker To-Dirt speaker_2_d...@yahoo.comwrote: For what it's worth. I stumbled across this by accident. At a tool change take your tool to an area where there's still a surface z0.000. End the move with z1.000. Remove the tool, and insert the new tool. Now use a clamp arm from your clamp kit that is 1 on a side. Raise or lower the knee until your tool is just touching the upper surface of your clamp arm. You're now indexed 1.00x inches above your work. Andrew -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- dos centavos -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] Tool table, setting up offsets with a caliper.
Guys, First off, thanks to all for porting EMC to 10.04, it is fantastic. Just a question. I use quick change toolholders based on NMTB-30. I am trying to get a tool table started. And I wonder if I can simply measure the total length of the tool, in toolholder, with a caliper, and then subtract say 4 inches and use that as offset. OFFSET = TOTAL LENGTH - 4 inches Is that completely wrong? At least this way, it is easy to set up a tool table and it does not require complicated tool setters, etc. - Igor -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
you can use the measured tool length as the number in the tool table you will need to set your z zero to use the measured tool length On Tue, Sep 7, 2010 at 10:17 AM, Igor Chudov ichu...@gmail.com wrote: Guys, First off, thanks to all for porting EMC to 10.04, it is fantastic. Just a question. I use quick change toolholders based on NMTB-30. I am trying to get a tool table started. And I wonder if I can simply measure the total length of the tool, in toolholder, with a caliper, and then subtract say 4 inches and use that as offset. OFFSET = TOTAL LENGTH - 4 inches Is that completely wrong? At least this way, it is easy to set up a tool table and it does not require complicated tool setters, etc. - Igor -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- dos centavos -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
On Tue, Sep 07, 2010 at 10:17:01AM -0500, Igor Chudov wrote: Just a question. I use quick change toolholders based on NMTB-30. I am trying to get a tool table started. And I wonder if I can simply measure the total length of the tool, in toolholder, with a caliper, and then subtract say 4 inches and use that as offset. Yes sort of. If you measure the entire holder including the drawbar screw part, I think you'll probably find some unwanted variation. You should find a way to measure from the taper instead. If you can turn up a ring that matches the taper, and you set that over a hole in your surface plate (or support it up on a pair of 123 blocks if you don't have a hole) and then use a height gauge to measure the tool, you'll get much better results. Also, QC30 holders have a feature that NMTB30 don't: they have a ground flange that is precisely sized and positioned relative to the taper. You might find that you have fine results just setting the flange on 123 blocks and measuring the tool with a height gauge. The flange on those holders is going to be much more trustworthy than the drawbar end. Chris -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
On Tue, Sep 7, 2010 at 10:27 AM, Stuart Stevenson stus...@gmail.com wrote: you can use the measured tool length as the number in the tool table you will need to set your z zero to use the measured tool length Stuart, do you mean that I have to set my zero by touch off? So say I touch off with one tool from tool table, then switch tool to my desired cutting tool, and the cutting tool would automagically be adjusted vertically to compensate for difference in offsets between the cutting tool and the tool I used to touch off Z. Right? Just tryin' to be clear. Thanks1 i -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
Igor Chudov wrote: Guys, First off, thanks to all for porting EMC to 10.04, it is fantastic. Just a question. I use quick change toolholders based on NMTB-30. I am trying to get a tool table started. And I wonder if I can simply measure the total length of the tool, in toolholder, with a caliper, and then subtract say 4 inches and use that as offset. OFFSET = TOTAL LENGTH - 4 inches OK, I developed a procedure some time ago for doing this. It worked with EMC1, it should work the same way with EMC2. I made a thing that looks like a cylindrical square, but has a female R-8 taper in it. I set it on my surface plate and used a height gauge to read the total height of the cutting edge. I picked one tool as a master and calculated the length of all other tools relative to the master one. I could then enter this difference in length for all tools other than the master, which was set to zero. Using the master tool, I could do a touch-off on the workpiece. Switching to other tools and applying the length offset worked very well. See http://pico-systems.com/preset.html for a couple pics. I haven't done this in a while, as having no ATC, it is much simpler to do all work with one tool, passing all workpieces through the fixture, then change tools and perform work on all parts with that tool. Jon -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
Igor Chudov wrote: Guys, First off, thanks to all for porting EMC to 10.04, it is fantastic. Just a question. I use quick change toolholders based on NMTB-30. I am trying to get a tool table started. And I wonder if I can simply measure the total length of the tool, in toolholder, with a caliper, and then subtract say 4 inches and use that as offset. OFFSET = TOTAL LENGTH - 4 inches Is that completely wrong? At least this way, it is easy to set up a tool table and it does not require complicated tool setters, etc. - Igor What I do is put a dowel pin in a holder and dedicate it to being tool Zero. Type M6T0 and G43H0 in MDI. Bring tool0 down to a setter or a block. Press the end key and set to 0.0 . Now mount a loaded tool holder and bring it down to the same setter or block. Record the reading and tool number. Repeat until you run out of holders. Fill up your tool table. My method of using a block is to jog the tool down to slightly lower than the block then slowly raise it till the block slips under. To set workpiece zero simply install tool zero, jog down to set the block, hit the end key, type in the thickness of the block and all tools will referance from that. The advantage to this method is you always have one absolute referance point with tool zero. Ed. -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
Ed, thanks. What do you use to locate Z edge of a part? You cannot use a ball end electronic edge finder, right? - Igor On Tue, Sep 7, 2010 at 11:56 AM, Ed ate...@mwt.net wrote: Igor Chudov wrote: Guys, First off, thanks to all for porting EMC to 10.04, it is fantastic. Just a question. I use quick change toolholders based on NMTB-30. I am trying to get a tool table started. And I wonder if I can simply measure the total length of the tool, in toolholder, with a caliper, and then subtract say 4 inches and use that as offset. OFFSET = TOTAL LENGTH - 4 inches Is that completely wrong? At least this way, it is easy to set up a tool table and it does not require complicated tool setters, etc. - Igor What I do is put a dowel pin in a holder and dedicate it to being tool Zero. Type M6T0 and G43H0 in MDI. Bring tool0 down to a setter or a block. Press the end key and set to 0.0 . Now mount a loaded tool holder and bring it down to the same setter or block. Record the reading and tool number. Repeat until you run out of holders. Fill up your tool table. My method of using a block is to jog the tool down to slightly lower than the block then slowly raise it till the block slips under. To set workpiece zero simply install tool zero, jog down to set the block, hit the end key, type in the thickness of the block and all tools will referance from that. The advantage to this method is you always have one absolute referance point with tool zero. Ed. -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
Igor Chudov wrote: Ed, thanks. What do you use to locate Z edge of a part? You cannot use a ball end electronic edge finder, right? - Igor I do use the zero tool. Usually I use a carbide end mill as a feeler. As mentioned earlier, bring tool zero down to just above the work piece, then jog it up until the shank of the end mill just slides under tool zero, then press the END key and enter the diameter in the popup box, press enter and your tool zero is referenced to the top of your workpiece. Always jog upward as you are setting the tool, if you jog down it might affect the position of tool zero. Incremental at .001 works well to fine tune the height. You could use your ball end edge finder as tool zero if you know the travel to actuation. Once you get used to useing a block or tool shank it is almost as fast. Ed. -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
Igor Chudov wrote: On Tue, Sep 7, 2010 at 10:27 AM, Stuart Stevenson stus...@gmail.com wrote: you can use the measured tool length as the number in the tool table you will need to set your z zero to use the measured tool length Stuart, do you mean that I have to set my zero by touch off? When you start EMC2, by default, the workpiece coordinate system you last used is restored. If this was set to some repeatable machine feature like the vise jaw, and you reference everything off that, that might be acceptable. Otherwise, it is probably best to reset some of the workpiece coordinates for each fixture setup. I can tell you of disastrous high-speed plunges into workpieces when I forgot to reset the Z offset, particularly, on a new setup. So say I touch off with one tool from tool table, then switch tool to my desired cutting tool, and the cutting tool would automagically be adjusted vertically to compensate for difference in offsets between the cutting tool and the tool I used to touch off Z. Yes, if the tool lengths of all tools are entered in the table, and you engage tool length offsets on every tool, then this will work. In my system, I do it a little differently, the master tool has a length of zero, and I don't engage the length offset on that tool (it makes no difference as its length is set to zero). To be completely uniform, then you should set the length of all tools, but you have to remember to activate the length offset of that tool before touching it off. Jon -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
Igor Chudov wrote: Ed, thanks. What do you use to locate Z edge of a part? You cannot use a ball end electronic edge finder, right? My hideous technique is to lower the tool close to the part, then feel under the cutting edge with a .005 thick piece of paper. When the paper starts to drag on the cutter, I enter .005 in the touch-off window. This works surprisingly well. Jon -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Tool table, setting up offsets with a caliper.
What I am doing now is setting up a tool table using GUI. I first homed the mill. Then I would load one tool after another: for each of them, I would find the Z coordinate so that they barely clear a gage block. Then, I enter the minus of that as Z attribute of the tool. I will try with a piece of rubber stock, to see if that method gives me consistent height betwen the tool and part, when a certain Z is commanded. - Igor On Tue, Sep 7, 2010 at 8:26 PM, Jon Elson el...@pico-systems.com wrote: Igor Chudov wrote: Ed, thanks. What do you use to locate Z edge of a part? You cannot use a ball end electronic edge finder, right? My hideous technique is to lower the tool close to the part, then feel under the cutting edge with a .005 thick piece of paper. When the paper starts to drag on the cutter, I enter .005 in the touch-off window. This works surprisingly well. Jon -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users -- This SF.net Dev2Dev email is sponsored by: Show off your parallel programming skills. Enter the Intel(R) Threading Challenge 2010. http://p.sf.net/sfu/intel-thread-sfd ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
