Stupid question of the day - Using Tools not in changer

jonaddis84 · Dec 15, 2015

I know I can set up more than 10 tools in the control even though my changer only holds 10. How do I go about using a tool # >10 in a program? IE: I am using #5 and want to put it back in the tool changer then manually load tool #16. If I just tell it to change to #16 does it automatically know to put the other one back and wait for me to load #16?

Thanks

Matt@RFR · Dec 15, 2015

If I'm understanding correctly, you would:

M6 T16
M0

Hit Reset while at M0 because the tool release button is locked out during any automatic operation. Install T16 manually, then start program again at or just below the M0.

What exactly is T16? A tool too long to have in the tool changer? Too heavy?

jonaddis84 · Dec 15, 2015

Matt@RFR said:
If I'm understanding correctly, you would:

M6 T16
M0

Hit Reset while at M0 because the tool release button is locked out during any automatic operation. Install T16 manually, then start program again at or just below the M0.

What exactly is T16? A tool too long to have in the tool changer? Too heavy?

T16 is hypothetical at this point, but I only have a 10ATC, so Im sure I will end up with more tools than can fit in there. Especially since one is a probe, one is the tool setter calibration "rod", and I also am not sure if say a 3" face mill would end up killing the two spots next to it if it was in the ATC.

Kind of a bummer if thats the way it has to work...

thesidetalker · Dec 15, 2015

Are you wanting to just store extra tool length/dia offsets (and use them later) or use more than 10 tools in a program?

BGL · Dec 15, 2015

What I have done..
Set up one program to run all the tools you can.
Set up another program to run other tools - use different offsets for this set with notations such as:
First program...(Tool set 1 T2_H02)
Second program...(Tools set 2 T2_H12)

Tags or marker on tools, tools set in a rack are big help.

Might be a better idea but this has gotten me through several times.

jonaddis84 · Dec 15, 2015

thesidetalker said:
Are you wanting to just store extra tool length/dia offsets (and use them later) or use more than 10 tools in a program?

I doubt I will use more than 10 in a program. In my line of work, I wont really ever be working on large batches of parts where I can sit and setup the ATC for a specific job. I will probably have 10 tools that Id like to stay in the ATC all the time for the majority of my work so I can fixture up and go. However, there may be odd jobs here and there that I need a tool outside of the ATC, so instead of swapping it out there, I thought there might be an easy way to just call it up and put it in manually.

A good example might be a large diameter slitting saw, where if I had it in the ATC Id lose two other spots, or even just tried to put it in for one job, Id have to actually remove 3 tools in order to put that one tool in.

shawnshop · Dec 15, 2015

You can't put the tool back in the changer and then manually load a tool unless you leave an open slot... If I were to program what your asking I would leave 1 slot open with no tool...we will say tool 10.. At the end of the previous tool program call up

t10 m6. To get to empty slot. Then
T16 M0 tool 16 with a program stop. Hit The hand jog button so tool release button will let you Load t16 using h 16 for your height offset.

Continue with that sequence of t xx m0 for all tools greater than the 10. And put an m0 in the program to stop and unload the t10 slot before you continue to tools in the ATC

You can go between auto and manual without hitting reset as long as it's stopped on an m0. That way for long programs your not finding where you stopped for every tool change where its not in the ATC. I believe you can have up to 99 tools set and stored this way.

It works for me. But just my $.02 worth.

SIM · Dec 16, 2015

Its the simple jobs that eat tool spots...four different drilled and tapped holes with a spot drill is 9 tools, add a reamer and endmill your done.

That said, my 1st CNC was a Bridgeport retrofit without a tool change...you can become very good at figuring ways to sidestep tool changes by multitasking tools and grouping.

jonaddis84 · Dec 16, 2015

shawnshop said:
You can't put the tool back in the changer and then manually load a tool unless you leave an open slot... If I were to program what your asking I would leave 1 slot open with no tool...we will say tool 10.. At the end of the previous tool program call up

t10 m6. To get to empty slot. Then
T16 M0 tool 16 with a program stop. Hit The hand jog button so tool release button will let you Load t16 using h 16 for your height offset.

Continue with that sequence of t xx m0 for all tools greater than the 10. And put an m0 in the program to stop and unload the t10 slot before you continue to tools in the ATC

You can go between auto and manual without hitting reset as long as it's stopped on an m0. That way for long programs your not finding where you stopped for every tool change where its not in the ATC. I believe you can have up to 99 tools set and stored this way.

It works for me. But just my $.02 worth.

This seems like a pretty good workaround, I like it a lot better than resetting the program and having to find where it left off. Im just curious what happens if you call up T16 M6 and you only have a 10ATC? I suppose one other option would be to use the same method you described, but actually have a tool in T10, then remove it and install what I want and change the offset. That way Im not losing a spot.

So, with what you described, you can call up a tool change to say T10 M6, stop the program M0, manually change tools, then the next line would just call up T16 without an M6 and the control will use that offset?

Thanks for all the replies so far.

SIM · Dec 16, 2015

A word of caution...if swapping tools for T10...make sure Pocket 10 is empty when loading new tool into spindle or the next M6 will have spindle and tool colliding with tool in Pocket 10.

Machine kinda does not let you do that...but an E-stop or tool changer reset can screw up the staging.

shawnshop · Dec 16, 2015

You can't use a t #greater than 10 with an m6 or it has an invalid tool number alarm. You can swap out a tool 1-10 as I had stated. Above but you have to have an m0 at the end of each program sequence before the next tool change to ensure you have the proper tool in the slot. So you don't have t5 slot end up with t15 in it or next program cycle you will crash t 5. Because it is the wrong tool in slot 5. Also I forgot to add you need to have a go to position prior to the m0 if not it doesn't go home.. Here is a sample program of what I use on a regular basis.

G90
G80
G40
T3m6
M1
S5000
G00 x. Y. Z.
G43 z1.5 H03 m08
Z
Xy
Xy
Xy
Z
Xy
Xy
Xy. All tool path
M5
M9
G00
G53 z0.
T27M0
S6000M3
G00. X. Y.
G43 z. H27 m08
Z
Xy
X
Y
Xy
X
Y
Xy
Y
X
M9
M5
G53 Z0.
M0 (put previous t3 back in for pocket 3)

yes I put notes in my program so I remember what I was suppose to do.. Then you can continue on. With tools in ATC or keep using the program as stated above. I like trying to put all t# above t10 to the end of my program so they all happen in sequence together that way you only have to remember to put the tool that's number matches the pocket number back in once... It may also be a good idea to have an M0 prior to the tool that has been taken out for the greater tool numbers to be sure you remembered to get the right tool in.

jonaddis84 · Dec 16, 2015

shawnshop said:
You can't use a t #greater than 10 with an m6 or it has an invalid tool number alarm. You can swap out a tool 1-10 as I had stated. Above but you have to have an m0 at the end of each program sequence before the next tool change to ensure you have the proper tool in the slot. So you don't have t5 slot end up with t15 in it or next program cycle you will crash t 5. Because it is the wrong tool in slot 5. Also I forgot to add you need to have a go to position prior to the m0 if not it doesn't go home.. Here is a sample program of what I use on a regular basis.

G90
G80
G40
T3m6
M1
S5000
G00 x. Y. Z.
G43 z1.5 H03 m08
Z
Xy
Xy
Xy
Z
Xy
Xy
Xy. All tool path
M5
M9
G00
G53 z0.
T27M0
S6000M3
G00. X. Y.
G43 z. H27 m08
Z
Xy
X
Y
Xy
X
Y
Xy
Y
X
M9
M5
G53 Z0.
M0 (put previous t3 back in for pocket 3)

yes I put notes in my program so I remember what I was suppose to do.. Then you can continue on. With tools in ATC or keep using the program as stated above. I like trying to put all t# above t10 to the end of my program so they all happen in sequence together that way you only have to remember to put the tool that's number matches the pocket number back in once... It may also be a good idea to have an M0 prior to the tool that has been taken out for the greater tool numbers to be sure you remembered to get the right tool in.

Thanks man, I appreciate you posting that. Seems like the way to go.

shawnshop · Dec 16, 2015

No problem. Even our Haas service /sales people didn't have an answer so it took some trial and error to figure that out... I guess I should put the disclaimer that it works on our machines that are less than 5 years old. Older than that I can't say for sure.

jonaddis84 · Dec 16, 2015

shawnshop said:
No problem. Even our Haas service /sales people didn't have an answer so it took some trial and error to figure that out... I guess I should put the disclaimer that it works on our machines that are less than 5 years old. Older than that I can't say for sure.

Well I guess my question wasnt as stupid as I thought it was going to be after all!

shawnshop · Dec 16, 2015

Now a question. Is there a way to call up a tool and a height based off of your work coordinate system and then use that tool with those conditions to machine... Ex if your pocketing and it misses a little boss in the bottom of the pocket. And you want to manually call up that tool /height/work offset, and manually go clean up that small boss.

I do lots of 1 off parts so I would rather not have to repost a program to clean up a small finish step..

Thanks ...

thesidetalker · Dec 16, 2015

shawnshop said:
Now a question. Is there a way to call up a tool and a height based off of your work coordinate system and then use that tool with those conditions to machine... Ex if your pocketing and it misses a little boss in the bottom of the pocket. And you want to manually call up that tool /height/work offset, and manually go clean up that small boss.

I do lots of 1 off parts so I would rather not have to repost a program to clean up a small finish step..

Thanks ...

Like... MDI? Manual Data Input?

T1M6
G0 G90 G54 G43 H1 XYZ?

shawnshop · Dec 16, 2015

Yes but to from what I have found it looses position after it has moved to that position and you go into hand jog mode... There may be something simple I am missing. But every time I have tried I have never had success... Can you verify if it works. And I am just missing something.... Basically I want to be able to run manually with actual offsets.

I could do it on my old journeyman tree mill. And used it often

beege · Dec 16, 2015

What I might do...
Turn on Setting 36 (program restart)
Find the place in your program where the tool in question will bee on the floor of the feature you need to touch up.
Slow down rapids and feed rate
Press "start" and follow the tool to near where it wants to be, then single block to where it's on the floor.'
reset.
manually clean up what needs cleaning up, while Z is there
Turn off Setting 36.

shawnshop · Dec 16, 2015

Yes that's one way of doing it. But its still not manually running the machine based off of the fixture and tool offsets. I know you can position the tool to say z 1. Above the part at x y with MDI and then enter the height in the operator portion of the position. Tab and then jog from there. Which is the best way I have found... But that's still based on the operator setting not the work and tool length.

jonaddis84 · Jan 13, 2016

So how on earth do I set a tool that is higher than my ATC holds? If I go to offsets, and go to say tool #15 to probe its offsets, it will start the probe cycle and say M6 T15, but then it gives me a H and T values do not match error. The active tool still shows #2 which is what I removed to put #15 in.

Stupid question of the day - Using Tools not in changer

Aluminum

Titanium

Aluminum

Stainless

Hot Rolled

Aluminum

Aluminum

Titanium

Aluminum

Titanium

Aluminum

Aluminum

Aluminum

Aluminum

Aluminum

Stainless

Aluminum

Stainless

Aluminum

Aluminum

Similar threads