Makino A77, Pro3, with custom "Makino side" question...

[gti_jay]

Alright, this is my machine;

Makino A77. Fanuc PRO3 control w/ custom makino frontside.

 

We use the tool detail function on the custom side to store all of our tool data. Then upon toolchange, we use the "M56 H1 D2" to transfer data from the custom side, to the "fanuc" side.

 

My question is this. How do I copy tool data in the opposite direction? i.e. If I enter data in the Fanuc tool offset screen, how can I update the custom side data?

 

Jay

[Rick Henrickson The Boeing Co.]

I do not think it goes both ways, andjustments need to be made in the tool data page not tool offset page.

but is this a standalone or is it in a cell?

[gti_jay]

Cascade,

My machines are in a cell, 3 A77's, 12 pallets.

 

I know it goes both ways...You command an "M53" and that put the machine in TOOL OFFSET DATA REGISTER MODE, then you can set the custom side data.

 

I am have trouble "finding" the data that exists in the fanuc side to update.

 

Does that make sense?

 

P.S. Are you a climber?

[specv]

what are you trying to accomplish with this data you are moving?

[Rick Henrickson The Boeing Co.]

i use to climb all the time, rock, and alpine.

 

so do you use h1 d17 or?

 

I just had the makino guys here last week and they said the only way to update the tool data is from the cell control.

I beleive though in the m6 macro the m53 is built in so every time it tool changes i think it updates the cell control.

 

you are trying to get your info from the tool offset page (fanuc side) to the tool data page right?

[specv]

offset 1 on the fanuc side is #10001

2 is #10002

3 is #10003

and so on...

 

but in order to write to the custum side you would need to enter the data without decimal points.

 

example:

M53

T1

S12345

S50

M37

Would put 1.2345 in offset 1 length column and .005 in the diameter column.

[gti_jay]

Cascade,

That is exactlly what I want to do. Get tool data into the custom side.

What do you mean "used to climb" haha

 

Specv,

That is exactlly what I am looking to do. How can I specify;

M53

T1

S#10001

M37

 

The above code won't work right cause of the decimal place in #10001

 

Thats where I am having trouble...

[specv]

S[#10001*10000]

should move the decimal place over 4 places.

[Rick Henrickson The Boeing Co.]

just curious? why dont you just put the offset in the tool data (makino side)

 

just not sure why you would adjust the tool offset (fanuc side)?

[specv]

because the machine reads the fanuc side, not the makino side.

[gti_jay]

Cascade...

Here is why.

When we calibrate our Renishaw probe "Z" axis...The way the software compensates for z is to adjust the tool length....WELL, if you don't update the custom side, the next time you do an M6, the adjusted value is gone!

[Rick Henrickson The Boeing Co.]

i know that, but the makino side puts the data in H1 D17 or D whatever your machine is set to.

it doesnt use any of the other offsets

it takes the data from the makino side to the fanuc side on tool change.

[specv]

if you are making an adjustment you can re run a tool without reading the M6 line and forget to change the makino side. Our operators are instructed to change the tool offset in the makino side and start at the M6 line

[gti_jay]

Cascade,

Yup your certainly right...But the probe software does NOT update the makino side. I want to automatically update the makino side with the compensated tool length value.

 

Otherwise you lose the probe z calibration as soon as you do a toolchange.

 

Follow me?

[Rick Henrickson The Boeing Co.]

are you talking about a renishaw tool pre setter

 

or a renishaw probe for measuring?

 

when I calibrate the renishaw probe for measuring we use the speronni tool presetter and then validate it with our gauge ring for x y and z

and adjust if needed in the makino side.

 

but i understand now what you are talking about.

I really dont think you can get the value from the fanuc side to the makino side atleast thats what they told us

[Rick Henrickson The Boeing Co.]

oh here is something else we noticed.

do you have the botsoma?

 

if it alarms out due to chips built up on the tool

you have to go to alarm page and reset it but it has already tool changed to the next tool

 

when you restart at the next tool (the one it tool changed already) it does not have the right comps loaded in the fanuc side. it is like it doesnt update the comps due to the botsoma alarm

 

I had to do T0 M6 then restart at the M6 to get it to update again. Have you seen this?

[gti_jay]

You can do it. I verified what SPECV said and it works just fine.

 

M53

T1

S[#10001*10000]

M37

M30

 

This code will update the Makino side data with the value stored in fanuc tool offset #1

 

Thanks everyone for your very prompt help.

 

JAY

[gti_jay]

Cascade,

I'm sorry...I can't help you with that.

I'm not familiar with that.

 

It might sound silly, But in the past we had an issue with program format..

 

T15M6;

 

M6T15;

 

T15;

M6;

 

All 3 of the above examples yield the same result IN THEORY...

 

However, we discovered that that placing the tool command and the M code on the same line DID NOT ALWAYS UPDATE THE FANUC SIDE. for reasons unknown, it didn't always work causing some severe crashes on proven work.

 

The ONLY format that works all the time is placing the code on 2 separate lines

 

T15;

M6;

 

Maybe this will help?

 

JAY

[Rick Henrickson The Boeing Co.]

Thanks guys I have been wanting to do that but was told you couldnt.

 

Nice job!

[specv]

when we recalibrate our probe it updates the custom side. what software are you using?

[Rick Henrickson The Boeing Co.]

great I will give that a try, I can alarm it out bye hand.

[Rick Henrickson The Boeing Co.]

maybe it does and I didnt give the screen enough time to refresh. I will go try it

[Rick Henrickson The Boeing Co.]

the software is inspection plus for the mp700

[Psychomill]

I suppose you could put the M53 in your calibration program to write to tool detail.

 

For tool change, all of our Makinos are programmed like this:

 

T1M6

 

And the M56 is in the tool change program. Never had it not get the tool offsets to the Fanuc side. With the probe, as soon as you read a M6, it should pull the new tool length over to the Fanuc side.

 

Now if you're calibrating in a part program, then you'll need the added M56 line to read the tool offset. Otherwise, you shouldn't have to. It's no different than someone setting a tool at the spindle on the tool detail, then not reading a M56 or changing the fanuc side.

 

Also, what cell controler are you using? The A2 system doesn't care about tool detail. But with B2 and A3, you might run into some issues if the cell control isn't updated for the ITN.

[Rick Henrickson The Boeing Co.]

the cell controler is mas 5

brand new

psycho thank you i will need to do it in the program in that instance.