Machsupport Forum
Third party software and hardware support forums. => Mach3 and G-Rex => Topic started by: Learn on June 13, 2014, 12:21:01 PM
-
Ok I run all sorts of mills at work and we never have to enter the tool length of any cutters . We work off offsets and manually pick up all of our cutters and use the tool changer everyday.
The only time I ever need to get a length is for calibrating my laser on my fidia but the rest of the machines we NEVER need length.
The only reason I ask is I want to pick up my cutters like I do at work and do manual tool changes in my IH cnc ???
Besides I don't have an extra holder for a dedicated indicator nor do I have a height gauge ???
-
Learn,
I am trying to understand what you mean. Are you using work offsets like G54 for each tool?
The purpose of tool length is to let use a number of tools at every work offset location. So if you had 5 tools and four vises all holding the same part you'd set 5 tool lengths and four work offests so you could machine at each location using all five tools.
Please explain further.
-
Ok at work we use the tool changer religiously and not once have I ever set a length for the cutters.
hass
hurco
YCM
Vison wide
eumach
all of these machines we set the cutter off the work price and run with it . All in the same off set .
we use g90g43h# in all of our paths along with the m6t# .
so basicly we never set lengths of cutters we just scratch them ( pick them up off of a 1,2,3 block) load the program and run it.
now at home I won't be able to just kick off the program and sit back down and program the next job I will have to tend to the tool changes and do it manual :( lol . I hope this makes sense.
I do understand lenths as well as the fidia I have a laser and it picks the length off all the cutters sorta like I would have to do in mach 3 then touch off on a work price with a tool that has been lasersd and enter my z offset in .
I just curious why I have to go with the last route with the lengths . The machine should know its position as it has been homed out correct?. I just ordered a couple more holders so I would have cutters and drills
made up I only have 5-6 tools that I use .
thanks in advance
-
Oh and another thing with the larger machines listed above besides the fidia we do not have to enter what kind of cutter it is. The fidia it has to know diameter and radius as it is a 3+2 machine and everything is to the center of ball for the rtcp.
-
we use g90g43h# in all of our paths along with the m6t# .
G43 is tool length offset, and uses the tool length to offset the tool.
I do understand lengths as well as the fidia I have a laser and it picks the length off all the cutters sorta like I would have to do in mach 3
So the laser is measuring the tool length.
I'm pretty sure you're using the length at work, and you just don't realize it. Unless you touch off every tool before you use it, the lengths have to be stored. If you use an ATC without the control knowing the tool lentgh, then you're using an ATC like a manual tool change.
In Mach3, if you zero the tool each time you change it, then Mach3 doesn't need to know the length, UNLESS you use a G43 length offset.
Mach3 also doesn't need to know the diameter, unless you're using G41/G42 comp.
And Mach3 has no idea, and doesn't care what kind of tool it is.
-
Learn,
You are setting tool lengths when you touch off cutters to the top of a part, because in those machines it is done automatically. Those machines all have a tool table in the control that you can access and see the length offset for each tool.
I worked at a place that did it that way for years. Once I taught the operators that tools could be touched off anywhere, and any ONE tool could then pick up the top of the part we stopped setting tools to the top of the part. Using a common place, that is not the part, to set tools means that tools can be set at any time, even after the usual reference point on a part has been machined away. This means if a tool wears out you can replace it in the middle of machining a part if needed.
Using a reference tool, typically an edge finder or touch probe kept in a tool holder saves even more time. I had to laugh that the machinists were installing and removing their personal edge finder at the beginning and end of every shift! The company purchased an inexpensive edge finder and one more tool holder and it paid for itself by the end of the week!
My home machine uses Tormach holders that are repeatable. I bought one extra holder for the edge find and never take it out of the holder, its my reference tool. I don't have accurate home switches, so I have to reset my tools only after a reset of Mach3, which typically means once I have set them I work all day without ever setting them again.
-
we use the 123 block on the table with a known offset that we key in the offset location
I know the machines have a tool table but it is done automatically .
so basically I need a tools that never changes as a ref tool. and a height gauge << both items I do not have.
I guess I will improvise
-
we use g90g43h# in all of our paths along with the m6t# .
G43 is tool length offset, and uses the tool length to offset the tool.
I do understand lengths as well as the fidia I have a laser and it picks the length off all the cutters sorta like I would have to do in mach 3
So the laser is measuring the tool length.
I'm pretty sure you're using the length at work, and you just don't realize it. Unless you touch off every tool before you use it, the lengths have to be stored. If you use an ATC without the control knowing the tool lentgh, then you're using an ATC like a manual tool change.
In Mach3, if you zero the tool each time you change it, then Mach3 doesn't need to know the length, UNLESS you use a G43 length offset.
Mach3 also doesn't need to know the diameter, unless you're using G41/G42 comp.
And Mach3 has no idea, and doesn't care what kind of tool it is.
ok cool I will try that out
-
Ger21 so basically if I home it out when I set each cutter then save the length in the table I won't need to use the g43 correct ?
-
I don't know what you mean by "home it out". You only need the length in the table to use G43. If you don't use G43, then you don't need the length.
I don't use G43, but I use an auto zero macro with two plates that automatically measures the tools after a tool change.
-
home out = ref the X Y or Z
but I mis read it . you auto zero ti each time you tool change so that will take up time as well.
ok ill use my tool setter I have and measure the face of the spindle to the end of a holder and use that as my main cutter and store it as a tool that wont be used .
so pretty much get the length of the cutter (reference tool ill use my edge finder) store the number
follow this step for all other cutters
SAVE tool table
This is the part that confuses me
now do I pick that edge finder up on the work piece ? use the gauge length on the off set page and then do I pick up all other cutters off the work piece s well??
when I post my paths make sure I use the G43 and tool number a?
Thanks for the help so far. As soon as I get off work I will go home and try this out .
-
Learn,
The reference tool could be any tool you use often. I use an edge finder because I use it all the time. I don't use a height gauge I use a 0.5" pin I roll under the tool. I like using a large pin so I never accidently jog the tool into the part or the table. You just tell Mach 3 the size of the pin or height gauge.
-
Gary thanks
so how do you find the length of your tool then ?
I guess I don't understand how you get your over all length then
-
Ok I am trying to get the lengths of the cutters and entering them in .
I am zeroing out a 123 block on the spindle face then putting in a cutter and moving up and getting length and trying to enter it in. Once I enter it in it looks as if it is in English. I work in metric. But that's only the tool table.
looks as if I scraped an endmill now with this last test . I'm getting frustrated with this as I can find the lengths and add them in but mach 3 is awkward for me going backwards I guess. I've been in the trade since the late 90's and thought this would be a bit easier to understand. Grrrr
-
Learn,
I will admit that tool length setting in Mach 3 REALLY had me going for a while! It took me a couple of hours one day determined to get it to work before I finally got it. So I'll try to save you some of the tools I broke by giving you one huge hint. When you press reset or rewind a program in Mach 3 it executes a G40 tool length cancellation automatically. This is deadly!! Because if you make a move with the previous tool still in the spindle it will move the Z to a zero length tool and almost certainly crash it. The correct length for the tool doesn't get set until the program reaches a tool change for that specific tool.
In mach3 and other CNC programs the tool length is kept in a table of offsets. The tool length gets applied at the tool change if you call the H word along with the tool number and then do a G43, which actually moves the Z to make the end of the new tool exactly where the end of the reference tool would be.
On the Offsets screen in Mach 3 in the lower right portion of the screen is where you enter the tool number and then touch off the tool to get the length. The reference tool, my edge finder is tool zero and it's length offset is zero in the table. All other tools get an offset plus or minus the length of my reference tool. You'll see this if you click the Save Tool Offsets button. These offsets are retentive even if you turn the machine off. So if you power the machine back up and pick up Z zero using the reference tool all other tools will still be the correct length when they are called, and you don't have to set them again.
If you are smart about this you may keep certain tools always in a holder and mark the holder with the tool number, then always use that tool number in your programs for that tool. You then don't have to touch off that tool again until you change it out because it is dull.
You need to play with this some. I'll bet you view what you do at work in a new light once you have this working on your own machine.
-
Learn,
Bummer! I started writing the post above and stopped for dinner. The answer to your crash is in that post. Sorry about that.
-
Learn,
I will admit that tool length setting in Mach 3 REALLY had me going for a while! It took me a couple of hours one day determined to get it to work before I finally got it. So I'll try to save you some of the tools I broke by giving you one huge hint. When you press reset or rewind a program in Mach 3 it executes a G40 tool length cancellation automatically. This is deadly!! Because if you make a move with the previous tool still in the spindle it will move the Z to a zero length tool and almost certainly crash it. The correct length for the tool doesn't get set until the program reaches a tool change for that specific tool.
In mach3 and other CNC programs the tool length is kept in a table of offsets. The tool length gets applied at the tool change if you call the H word along with the tool number and then do a G43, which actually moves the Z to make the end of the new tool exactly where the end of the reference tool would be.
On the Offsets screen in Mach 3 in the lower right portion of the screen is where you enter the tool number and then touch off the tool to get the length. The reference tool, my edge finder is tool zero and it's length offset is zero in the table. All other tools get an offset plus or minus the length of my reference tool. You'll see this if you click the Save Tool Offsets button. These offsets are retentive even if you turn the machine off. So if you power the machine back up and pick up Z zero using the reference tool all other tools will still be the correct length when they are called, and you don't have to set them again.
If you are smart about this you may keep certain tools always in a holder and mark the holder with the tool number, then always use that tool number in your programs for that tool. You then don't have to touch off that tool again until you change it out because it is dull.
You need to play with this some. I'll bet you view what you do at work in a new light once you have this working on your own machine.
the crash was my trying to reset the machine as I made an MDI move and once I hit reset it just dives. it has happened before even when I was not trying to do anything with the offsets .
I already see things at work in a totally different way LOL.
OK let me see if I am getting this correctly
you use a center drill as our reference tool and is tool # Zero and the length you have is Zero as well? how do you pick that reference tool up to get a length of zero?
I wish there was a good video to watch to explain this . as the tormach one shows entering length that was from a height gauge.
-
OK I got all the tool lengths added in the mach 3 made sure everything was homed out now I am using mm not English just an FYI
I used tool 1 as reference tool just as the tormach video shows followed step by step going over and over the video . I do a t16 m6 g43 h 6 and it has my number as a huge negative number
what could I be doing wrong ????? this is driving me nuts .
-
I came to a conclusion tool offsets don't work on my mach 3 I would love to speak t someone and see if it is just me
-
Edit LOL I got it to work with out using the g43 h# t# man I had tto change the numbers around neg to positive and go in a sequence and now it works . Thanks for all your help
-
I do a t16 m6 g43 h 6
Unless that's a typo, you're using the length of tool #6 for tool #16.
-
Lol type o t6 is my 6mm drill t16 is my 1/2 endmill
-
Got it all set up . I have not tried to use the g43 yet but I can use the tool number and it has made life a lot better . I had a job to do and it had 90+ holes per bar with multiple setups and 4 drills and 1 cutter and wow the time I saved . Thanks all.
-
(https://scontent-b-iad.xx.fbcdn.net/hphotos-xpa1/t1.0-9/p160x160/10392551_570555036399155_300280796853322437_n.jpg)
there is holes on both sides as well
-
Learn,
Good to see you making progress on this. It really does work and I expected you would see the value once you started to understand it. Are you machining more than one of those at a time and using work offsets g54, g55 etc. for the different parts?
-
No I had to slide them 3 times on the mill. Those are 60" long using 2 vises in my IH cnc. Once I start multiple parts I will play around and make sure the g43 is working. I had some issues with my limit switches coming on which messed up a couple of holes but they are still functioning fine for what they are for. I just turned the limits off till I finished the job. Then read up on it and changed a setting in the general area and it seems fine now . Will update later once I use multiple offsets and the g43. Thanks again
-
Learn,
I've done long part in the past, some long copper bus bars that needed a lot of tapped holes. How do you relocate for each position? We actually did it by using a tool or pin in one of the holes. We put the pin in the hole, paused, unclamped the vise, let the tool move to a new programmed location, and reclamped. I am getting ready to drill holes and finish both ends of a long part using this method, by using an end mill to make the holes, round the ends off and relocate the part.
-
I used pins and an edge finder. I also have a coaxial indicator that helps as well
what did you make the copper bias bars for ?
-
Just a grounding buss for a computer room. It needed lot of holes.
-
Well I spoke to my customer and all of counterbore holes need to be for a 3/8 bolt now. After I asked before drilling .grrrrr that's 54 holes I have to re do .
-
Drill press time! Get a subland drill from McMaster Carr or other supplier and knock it out.
-
Nah I don't have a drill press. I'm doing 4 holes at a time
-
Well it still took me near 3 hours and had 4 programs
I was able to do 4 outer holes ( drill path then 3/4" cutter drill path ) on each outer dour holes. I used a block in between with a hole to pin off a locator hole . The came back after wards and drilled and counter bored the last hole .
lessons learned on this job. Order form in place . Then the guy had the nerve to come pick them up with no money another new fuel in place no payment no chips made
-
Now here is a question. Is it worth the time of hooking up an automatic tool setter ?
-
That's a question only you can answer. Depending on how you measure your tools, it may save a lot of time.
On my router, I use an auto zero system with two touch plates. One that I place on the workpiece to set Z zero, and a fixed plate away from the work that is set as a reference position. When setting Z zero, Mach3 will touch the plate on the workpiece, then go to the fixed plate, and save it's location relative to Z zero.
When there is a tool change, I change the tool, and my M6 macros send it to the fixed plate, which sets the tool to Z zero.
With this method, you don't need to use the tool table, or use G43 length offsets. You never need to know the length of the tool, as everything is done automatically.
This may not be for everyone. If you do a lot of tool changes, and have your tools pre-measured in holders, then the tool table and G43 may be a lot faster.
-
Thanks for the input