Safety improvement post mod

[Bob W.]

I don't know why I didn't think of this a long time ago but I found a pretty good safety improvement, at least for my shop. I am usually running my machines pegged at 12k rpm and I have inadvertantly spooled up the spindle to 12k with edge finders, dial indicators, co-ax indicators in there. Granted, this is once a year and I am lucky I haven't been seriously injured or worse.

 

With my machines (Haas) the spindle reverts to the last rpm it was running at when one hits the cw or ccw spindle start buttons. If the operator forgets to reset the rpms to an appropriate value it will spool up to whatever it was running at before. I modified my post to add an S50 at the end of my programs right before the M30 so it will reset the spindle rpms to a safe value at the end of every program. This will cut these types of issues by 95% or better and it took all of 5 minutes.

 

I just figured I would throw this out there because it is very simple and at the least it could save a dial indicator.

 

I have just taken on a local high school kid with an interest in machining and I am trying to create a safe environment for him to work in. If anyone can think of similar safety mods like this please post them.

 

Thanks,

Bob

[Chris Rizzo]

That's a great idea Bob. I've exploded a edge finder just like that too, forgetting to hit the spindle speed -10% about 8 or 9 times.

[Guest CNC Apps Guy 1]

On FANUC machines, I've captured the current tool number in the spindle as a MACRO variable in the Tool CHange MACRO. Then as opposed to calling G43 HXX Z1.25, it would actually read G43 H#506 Z1.25

 

NO possibility of using the wrong offset that way.

[Grievous]

You can do even more.. you can configure your Fanuc controler to load the offset automaticaly when it's changing the tool so there is no need of G43 Hxx or Dxx at all. Like on mighty Sinumerik. Only thing is if you're using on some tools, like T cutters, 2 diferent offsets. You'll need to decalre the second offset in conventional way.

[Dave.L]

quote:

---

NO possibility of using the wrong offset that way.

---

James,

 

That's a cool idea except when you use multiple length offsets (we do for t-slot cutters).

 

I have not done it yet, but I wanted to errorproof fat fingering of wear offsets.

 

I am always affraid someone will be careless and enter -1.0 instead of -.001 or something for a length wear value.

 

It would be cool to have a range limit to prevent damage.

[jeff]

quote:

---

I modified my post to add an S50 at the end of my programs right before the M30 so it will reset the spindle rpms to a safe value at the end of every program.

---

I've been doing this for years.

Mainly because on Okumas the spindle is still orientated at the end of the cycle when it changes back to tool 1, and I don't like having it sit there for an hour or so putting all that strain on the motor if I am still programming the next job.

 

I started doing this after we had to replace our first spindle and I noticed that after a while the tool would get hot and you could hear the motor struggle to hold it oriented.

Maybe it's helping, maybe not, but it eases my mind LOL.

[LA CAMmer]

Thanks for the idea, Bob.

 

Talked to guys on the floor about it and they love it.

[YoDoug®]

quote:

---

I am always affraid someone will be careless and enter -1.0 instead of -.001 or something for a length wear value.

---

I wrote 2 macros at my last job that addressed this. They were coded into the posts for our production mills.

 

One was at the end of each tool path. It takes the current H, D, and wear values and writes them to a calculated variable, IE, tool 24 goes to variable #724, 25 to #725, etc.

 

Then there is a macro after the tool change for each tool. It looks at the stored calculated variable from the other macro that goes with the current tool and compares it to the actual H, D, and wear values and if the difference is greater than a predetermined value then it alarms. There is also a block skip to skip this check for first piece set up.

 

We normally kept it at around >.1 difference would alarm.

[Dave.L]

Doug,

 

Yea, that is what I would like to do. If you could share it - that would be great!

[YoDoug®]

Dave unfortunately when they laid me off they only gave a few minutes to pull personal files off my pc. I have been wanting to rewrite it soon, but it depends on free time. If I do I'll share.

[Dave.L]

quote:

---

If I do I'll share

---

Doug, if I beat you to it, I will share too.

 

It's been on my list for a while, but low on the list.

[Acro Engineering]

Anyone get around to writing the offset macro? I decided to do the same thing and looked on the Forum first...

[YoDoug®]

I have not rewritten it as of yet. What kind of control are you looking for this to work in.

[Joe788]

I have Mazaks so I don't need that macro. Offset increment limiting is a parameter.

[YoDoug®]

I have Mazaks so I don't need that macro. Offset increment limiting is a parameter.

 

It is on Okuma also. I think on 31i you can too, I just don't remember for sure. Its been a while since I've worked on one.

 

 

 

[Acro Engineering]

Fanuc 21i.

We always have the true radius of the cutter in the offsets that match the tool number (T1=H1,D1) and use a laser to measure the tools. This way anyone can view the offsets and determine what size cutter is in the machine, we add 100 to the offset to use wear comp so as to reduce operator error (T1=H101,D101) and have logic in the post to check tool number equal offset number if control comp is used and tool number equal offset number plus 100 if wear comp is used.

 

My goal is to create a macro and modify the post:

Check the offsets of the tool in the spindle to confirm the offsets are not zero.

Confirm the tool matches the programmed radius when using computer comp (within .0005).

Confirm radius of cutter is within a percentage (10%) of the programmed tool diameter but not larger than the programmed diameter when using control comp.

Confirm the radius of the cutter is within a percentage (10%) of the programmed tool diameter but not larger than the programmed diameter when using control comp. Do the math to place the correct wear offset in the control in the correct offset based on the measured tool offset. This way the operator does not have to measure for wear but just run the same macro to measure the tools length and radius like he always does.