Negative Tool Lengths?

[nine blue]

Situtation:

New guy hires into shop. Sets up on our Leblond Makino VMC with Fanuc 11M control.He homes the Z axis and sets the distance from the spindle face to the part zero as a positive number in the G54 work coordinate. He sets the tool length from the tip of the tool to part zero as a negative number in the tool length table. Claims this type of set up is crash proof if the programmer leaves out the G43 or the control "misses" the G43.

Says the spindle will merely go home.

Problems:

The tool lengths as you can imagine no where reflect the actual tool length.

I get confused when I have to make edits to his program. He does not use Mastercam. Prefers the conversational Fancuc format which I do not like at all.

Questions:

Are his concerns about "missing" the G43 valid?

Do any of you guys use this method? I've never

seen it before but would be willing to try if it was a proven advantage?

Does anyone program using this method in Mastercam?

If so how do you set up your parameters page for part zero?

 

BTW I'm not exactly sure if I accurately described

his set up method but I know his tool lengths are all negative. And he is a good machinist. No scrap and quick on setups.

[Guest]

quote:

---

if the programmer leaves out the G43 or the control "misses" the G43.

---

I don't agree with this part of his statement, if that's the issue there are "bigger" problems to correct.

 

Gage length programming is a much better way to fly IMO. Especially if you're programming an HMC.

 

His tools should be set as the "gage length" This would be the length of the tool and the holder from the "Gage point" of the holder to the tip of the tool. His program should be NO different only his offsets should reflect this difference. All of this requires a tool length presetter to be used.

 

JM2C

[ToolMan184]

New Guy = Get with our system not us get with his system. M2C

[Thad]

Toolman, what if his system is better?

 

Thad

[Matthew]

quote:

---

Toolman, what if his system is better?

---

He should prove himself first using the current system and once he's been there for a while then he should make some suggestions to improve the process making sure everyone understands and agrees with the new methods. I'm sure this place has been making good parts with minimal crashes before he got there.

[Guest CNC Apps Guy 1]

quote:

---

...Gage length programming is a much better way to fly IMO...

---

+10000

 

Reasons;

1) Tools can be transported from macine to machine and the offsets can be input via G10

2) The same tool can be used across multiple jobs easier.

3) Can be used in conunction with an offline presetter.

 

There are more reasons but these are a couple of the biggies.

 

When I train customers even on VMC's I teach them + Tool Lengths because it's a more versatile system.

 

Crashproof.... that's a silly reason IMHO. Like John says if that's the reasaon then you do have bigger problems.

 

JM2C

[pip]

I agree with Mathew here. Do it the tested and proven, in that company, way. Then when you have proven your worth, make suggestions. Backed up with evidence. You can alianate yourself very quicky in a firm if you try it your own way, and wont adapt to the firms way..

[nine blue]

Wow! Thank you for the quick replies.

Your advice and comments confirm my gut feeling.

I'm making a print out of John's and CNC Apps Guy

replies in case I need some back up to justify using positive tool length offsets.

Thanks again. You guys are the best.

[Guest CNC Apps Guy 1]

Anytime.

 

Welcome to the Forum!

[Dave Ball]

Machines don't "miss" code, usually the problem is in the communication getting the code to the machine, back in the day this was less than perfect and some info was lost from time to time. In 25 years I've never had a machine "miss" a code. This guy is using old skool techniques that just don't have any advantages that apply today.

[ToolMan184]

Matt, that is my exact way of thinking. Prove yourself then we can look at making changes. We make changes very often from folks I have worked with for awhile. When it comes to setting tools the way he describes just seems alot could go wrong.

[Rick Henrickson 65]

this is an old method and many people still use it I bet one of his tools has a zero tool length and he measures the rest relative to that tool you can still crash nothing is crash proof!

 

Gauge line is the best for sure

[MotorCityMinion]

Currently using negative offsets. The shop in general doesn't have a clue as to what a pre-setter is for. Never tried a negative offset without a g43 either.

 

"I don't agree with this part of his statement, if that's the issue there are "bigger" problems to correct."

 

I agree with the disagreement. After seeing code a few hundred times a month, someone all the sudden forgets to add a g43 next to the H callout? Kind of like forgetting to breath , isn't it? In 20 years of machining, I've never seen a controller miss a g43 callout. Is that even possible?

 

No scrap and quick. Work with him for a few. New concepts usually seem awkward at first.

[Thee Dragracer1951]

I think I might ned schoolin here.

I use negative tool offsets. I set tools off the presetter on the table. It's 2.0 inches high. Then set the G54 Z offset from that. That would be a positive number but the actual tool offsets are negative. What the heck are you guys talking about to get positive numbers?????

[Guest CNC Apps Guy 1]

The positive number is the "Gage Length", or the value from the gage line of the tool holder/spindle to the tip of the tool.

 

HTH

[MotorCityMinion]

It's also a fixed value. Has nothing to do with the wpc Z value or the workpiece face. You can actually eyeball it with a scale, tool tip to spindle nose. Tool presetters, stand alone units or machine installed units, measure this value. The better stand alone units come with optical comparators for checking nose radius and angles as well. They also check tool diameters fairly accurately. They are calibrated with a standard that is set to a known length and usually ground at the center for setting the cl.

 

Try this: Take a 123 block and place it on the table top of a vertical machine or the edge of a pallet on a horizontal. Now touch off the spindle nose to block and origin out your Z. (Zero it). Back off the z and put a tool in the spindle. Now touch off the tool to the 123 block. The number will be positive and that is the gage length were talking about here.

 

This is what the stand alone units do , just quicker and out of the machine. In top notch shop with a crib, the crib attendant will set the tools before they get to your machine.

 

Schools out, miller time.