Hello Guest it is September 19, 2019, 05:09:08 AM

Author Topic: Where are tool length offsets referenced from?  (Read 3501 times)

0 Members and 1 Guest are viewing this topic.

Where are tool length offsets referenced from?
« on: July 03, 2016, 03:49:53 AM »
I get the basic idea of tool length offsets but I am wondering where they are referenced from. Obviously the actual tool length has little to do with where Mach3 would define the tools zero position in relation to my workpiece.

I have done a lot of research but I have yet to find clear info about the actual reference point...

Am I assuming correctly that if my Z zero position is at the top of the travel, I'm my case 12" above the bed, that Mach3 determines the length offset from that point for each tool?

If someone would be so kind as to offer what I may enter in the tool table for, lets use the example of a tool that is 1.5" and the travel to the touch plate is -10.5" I would greatly appreciate it. This would let me see how the offsets are calculated and what data I actually enter into the tool length offset table.

Additionally, I believe I would prefer positive offsets. Is this possible since my Z operates from 0 to negative 12"?

Lastly, zero to the top of my workpiece - I am willing to alter this to the top of the table but since I have a wood router the table height will constantly change since I surface the spoil board.

Any example would be greatly appreciated.


Thanks in advance,



Gio
Re: Where are tool length offsets referenced from?
« Reply #1 on: July 03, 2016, 09:21:28 AM »
Tool legth offset is just a number, where it is referenced from is up to you. People have a tough time getting there mind around this. I simply pick a reference tool. My preference is a common edge finder permanently installed in a toolholder. It needs a tool number to be assigned. A dab of paint at the joint shows that it has not been moved. This edge finder can be used to pick up the sides or the top of a part.  I like to use a 0.500" pin that is rolled back and forth under the edge finder. I do this because an oops like being in continuous or a large jog step when approaching the part doesn't result in a crash.

So using my reference tool with the correct tool number I can pick up the top of a part, or the table, or top of the vise and zero the Z axis. Then set other tools on that same surface.  So the offset number will simply be plus or minus the length difference between my reference tool and this tool. To test you got it right. Move the reference tool with the correct tool number well clear of table or part and zero the Z axis. Call a tool change for a new tool with the correct tool number. Make a feed move to Z zero. The end of this tool should now be at the same Z level that you set the reference tool at.

Hope this helps, it takes a little practice.
Re: Where are tool length offsets referenced from?
« Reply #2 on: July 03, 2016, 12:34:07 PM »
Gary is giving you the right info regarding the tool offsets. By using the edge finder, you have a reliable Zero Home reference tool that is not going to get busted off in a crash. You have to learn to think about the Machine home, and the Work home. They are not the same thing.

They both exist on the machine, and the "Z Zero at the top of the machine travel" is the Machine Z home.

You don't have to worry about making all the tool offsets "positive."  Mach3 will take care of all the math/arithmetic as far as tool offsets. When the program is running, the Z axis readout shows the program depth of a surface or hole, no matter how much longer or shorter one tool is from the others.





Re: Where are tool length offsets referenced from?
« Reply #3 on: July 03, 2016, 01:27:55 PM »
By the way, unless you have really accurate homing switches, or pick up home from an encoder index mark, using the machine coordinates is pretty much useless except for soft limits.  I only implemented limt switches on all axis to prevent a hard crash against the end stops. Mine are simply wired in series and connected to a hard wired E-stop circuit.
Re: Where are tool length offsets referenced from?
« Reply #4 on: July 03, 2016, 10:32:31 PM »
I thank everyone for the help! This forum is awesome.  I hope one day  I can contribute here they way you all have been so willing to do!

If I am understanding this, Mach uses tool X to determine the offset of the other tools. This leads me to ask what I initially enter for tool x and are the other tools, 2, 3, 4 and so on a plus or minus value from the index tool.

Better stated - If I have in tool position 1 a 2" bit and this is my reference tool would it be zero length in the offset table and if tool 2 was a 1" bit would it be -1" and lastly if tool 3 was a 3" bit would it be +1 in the tool table.

Just to let you know a little about me and the machine I am trying to get this working on, I fabricate CNC routers - well, more precisely I design the machines (the frame, gentry, motor mounts  and other mechanical components) and am know to be one of those engineers that like to run the parts I design So I do run mills, lathes, routers and weld.

The machine in question is a 60x120 wood/aluminum/plastic flatbed router that, at least according to the equipment we have, is accurate to +/- 0.0006 per 2000mm,  uses C1/C2 grade linear motion components, dual 110mm frame 1.8Kw servos for X, single 110mm 1.3Kw servo for the Y, single 1Kw Z , harmonic gear reduction and very precise proximity sensors. Not bad for a wood router I suppose... I will say I spent a fortune on the drive  and linear motion components on this one and this is my personal machine. Saved a long time to afford this and am excited to have built one from the ground up myself. I never imagined tool offsets would be the death of me - lol.

I recently switched from a different control systems to Mach (I really like Mach better than the commercial over-priced systems) but the ATC is giving me a heck of a time due to tool lengths. The way the systems I am familiar with handle offsets, as far as the end-user is concerned, are very different than Mach (or I am just not as knowledgable in the back-end of how this is done - either way it is different to me).

I am very comfortable with machine coordinate mode vs. work offsets and have a (mostly) functional tool carousel tool changer with a very precise fixed Z touch-off sensor. Additionally, all tools are set with a tool setter  -as garyhlucas has stated, I am one of those that are having "trouble wrapping my mind around" the way mach does it.

What I am having to do now after a tool change is re-zero the Z each time a tool change is called and I should not have to do this if I can figure out tool length offsets.

You all here have given me great information and I will try, using the above, to figure this out. I am kind of understanding how Mach handles the tool lengths I think - If someone would be so kind as to confirm that my example above is the right logic I will give it a go.

Thank you again everyone - I greatly appreciate all the answers; they have been very helpful.

Offline Davek0974

*
  •  2,577 2,577
    • View Profile
    • DD Metal Products Ltd
Re: Where are tool length offsets referenced from?
« Reply #5 on: July 04, 2016, 12:31:52 AM »
Bridgeport Mill, Mach3 V062, CSMIO-IP/A controller, AC Servo Drives
Re: Where are tool length offsets referenced from?
« Reply #6 on: July 04, 2016, 01:37:31 PM »
Once tool length offsets have been entered, and a length offset has been applied for a tool, then ANY tool can be used to pick up Z zero.

What hasn't been mentioned is that after loading a tool you need to call G43 H(offset #) to apply the offset.  Can't remember when it actually gets applied, an immediate Z move or on the next Z move. To cancel the offset use G49. Be careful doing this! Canceling an offset with a long tool still in the spindle can be really bad!

Bit of a funny story about this process. I was hired as a machine designer at a machine shop. A few days later they fired the machinist running a Fadal 4020. They asked me if I could run it as I had a little CNC experience.  Sitting in the machine was a great big valve casting with a flange on top that needed to be milled, drilled, and backfaced too. There was a 1" wide slot already milled into face of the flange. I asked another machinist what the slot was for?  He said "He does that for every job. That's the Z zero finished surface where he sets off all the tools." Oh yeh he understood tool offsets, Not!
Re: Where are tool length offsets referenced from?
« Reply #7 on: July 04, 2016, 02:38:08 PM »
Davek0974 - The youtube link is VERY informative. Thank you!

garyhlucas - Thank you for mentioning G43 and G49! Also it is nice to speak with a fellow designer turned machinist. That is a funny story about the valve casting - you're right; that person had absolutely NO understanding of tool offsets. I have to know - were you able to mill it out?
Re: Where are tool length offsets referenced from?
« Reply #8 on: July 04, 2016, 10:44:35 PM »
No I never did the part. It barely fit in the machine and the flanges were the easy part.  The interior had to be machined too, and down inside at a depth of over 6" was a 6" diameter internal thread and a tapered seat! If we did try to machine it the whole operation from roughing to thread milling would have to be done completely blind. I think they finally realized this was beyond us and sent it to someone with the right equipment.

They hired a new machinist that was very good, and we got a second machine. I continued doing all the programming, until they replaced me because  they said I was too slow. Funny part was I wrote 4 times more programs than we actually ran, because there simply wasn't enough machine hours to do all the work they were sending to us!
Re: Where are tool length offsets referenced from?
« Reply #9 on: July 04, 2016, 10:57:22 PM »
Gary - It is a shame how employers treat people sometimes. Fortunately I work in a very easy-going environment in both my jobs. I work 50% of the time engineering/fabricating and the other time for a defense contractor and they are very laid back - you have to be to do that kind of work. The great part is I get to play with cool equipment at both jobs though!

On the tool offsets; I can't wait until tomorrow to try to get my ATC working properly - thanks to all of you here!

Kind regards,

Go