HAAS VF-3 programmable coolant

[Bowfisherman]

I recently recieved a haas vf-3 with programmable coolant. Story is, I have a few other VMC's but none have programmable coolant. I am using MCAM X MR1 and would like a little insight as to how I make this programmable coolant thing work and where code needs to go and if MCAM has a macro or setting that turns Programmable coolant on.

 

Thanks,

[Guest CNC Apps Guy 1]

In a nutshell if your machine needs/wants a code to turn something on/off, you can do it in MC.

 

I know nothing about the new Haas Programmable Coolant Nozzles, I know the older ones you set up in the tool table. It may still be that way I don;t know but if yo uput up some code, I'm sure we could point you in the right direction.

[iowajim62]

Programmable Coolant is controlled on the Tool Offset Page. you can't program it by code in the program. You can move it up and down on the Operators Control Panel and it will reflect the position on the Tool Offsets page. You can input a number on the offset page if you like as well.

HTH

[Bowfisherman]

I appreciate that, I will upload code tomm. while at work.

 

Thanks

[Bowfisherman]

Iowajim62,

 

Do you adjust the spigot to tool one of the program and then input tool offsets afterwards?

[iowajim62]

quote:

---

Do you adjust the spigot to tool one of the program and then input tool offsets afterwards

---

No,setup your tools in holders and load in the machine, now when you run/prove out your program you will adjust the coolant as each tool comes in the spindle. On the control panel are coolant up and down buttons to adjust the position for each tool. After you manually adjust the nozzle go to the Tool Offsets page and adjust the number for position which is the first value after the tool number. You can use positive or negative numbers to edit the values that may already be there. For example T1 has a value of 4 and you moved the nozzle down. You go to offset page and it shows the coolant positon to be at 6, move the cursor to T1 coolant value and type 2 and push input. You get a value of 6. Now when you run your program the nozzle will move up and down with each different tool. HTH

[Randy Morton @ Clem Industrial]

Iowa,

 

Not to mince words, but I would disagree with you about the programmable coolant. Would it not be called 'programmable' so that it could be using in conjunction with a G or M code? I am fairly certain when I ran a VF6 years ago that I was throwing in M (maybe G) codes to get it working... I will have to look into it.

[John13]

I set up my programmable coolant at the control. After I get all the tool heights in, I go back and do the coolant. On the Haas control>hand jog> offset> Coolant Position is the column right next to the tool number. Move the cursor to the tool you want to adjust to under the Coolant Position column adjust the coolant up/down and enter the number. Change tools/repeat for all tools.

 

When you go to change programs or whatever, if you do not clear all values, you will need to do math (at least I do) Say your coolant is position 3, next program you adjust it and it is 7, instead of inputting 7, you input 4 and it adds the 3 and 4 and that's where the 7 comes from. Confused me for a while when I first got the machine.

 

HTH, I hope I didn't confuse you any more.

 

 

After further review, I see I almost copied iowajim using different values.

 

Oh well

 

[ 10-16-2007, 08:57 AM: Message edited by: John Kulp@Amphenol InterCon Systems ]

[heavychevy2155]

No, Iowajim is on the money.

[Lars Christensen]

M34 and M35 will make it possible for you to change your position in a program.

[Bowfisherman]

Iowajim,,, it worked!!!!!, I done just as you said and the dog gone thing worked.

 

This is the reason these forums are successful.

Cause of guys like yourselves.

Hope I have something to bring to the table when needed.

Thanks

[Michael Sullivan]

I want programmable coolant for my Super MiniMill

I always had it on the big HAAS'

[Kannon]

quote:

---

When you go to change programs or whatever, if you do not clear all values, you will need to do math (at least I do) Say your coolant is position 3, next program you adjust it and it is 7, instead of inputting 7, you input 4 and it adds the 3 and 4 and that's whee the 7 comes from. Confused me for a while when I first got the machine.

---

just put in 7 and hit F1 and it writes it. otherwise you can do teh math like Keebler.

[John13]

Thanks Kannon, I never knew that.

[Kannon]

quote:

---

Thanks Kannon, I never knew that.

---

your welcome!

[iowajim62]

Randy,

I stand corrected, I learned something new.

Lars,

You are right Sir.

Leonard,

Your Welcome

Look at the code Lars and Randy put up and try that too.

Kannon,

Thanx for the tip bro.

[Surface]

I have a little macro which reads the tool-offset table. At each tool change, I call the macro (G65). The macro reads the tool length and will automaticly adjust the programable coolant if no coolant position is specified. ie position=0

If a value is present to position the coolant, the macro won't automaticly move it.

Not perfect, but it gets it in the ballpark and saves a few keystrokes.

[Bryan Johnson]

this macro sounds like the way to go.

Can i have a copy of it?

[htm01]

surface,i'd like to see that too.can you put on FTP?

[Surface]

All of my tools are set from a Renishaw tool-probe. So they are always a constant length. The macro I use is:

 

%

O09005 (M88-COOLANT POSITIONING)

(10-05-06)

(#523 STORES P-COOL POSITION)

(#120 IS FOR VOLITILE USE)

G103 P1

#1= #[ 2000 + #3026 ] (GET TLO VALUE FOR TOOL IN SPDL)

IF [ [ #1 GE 2.000 ] AND [ #1 LT 2.500 ] ] THEN #523= 5

IF [ [ #1 GE 2.500 ] AND [ #1 LT 3.000 ] ] THEN #523= 6

IF [ [ #1 GE 3.000 ] AND [ #1 LT 3.500 ] ] THEN #523= 7

IF [ [ #1 GE 3.500 ] AND [ #1 LT 4.000 ] ] THEN #523= 8

IF [ [ #1 GE 4.000 ] AND [ #1 LT 4.500 ] ] THEN #523= 9

IF [ [ #1 GE 4.500 ] AND [ #1 LT 5.000 ] ] THEN #523= 10

IF [ [ #1 GE 5.000 ] AND [ #1 LT 5.500 ] ] THEN #523= 11

IF [ [ #1 GE 5.500 ] AND [ #1 LT 6.000 ] ] THEN #523= 12

IF [ [ #1 GE 6.000 ] AND [ #1 LT 6.500 ] ] THEN #523= 13

IF [ [ #1 GE 6.500 ] AND [ #1 LT 7.000 ] ] THEN #523= 14

IF [ [ #1 GE 7.000 ] AND [ #1 LT 7.500 ] ] THEN #523= 15

IF [ [ #1 GE 7.500 ] AND [ #1 LT 8.000 ] ] THEN #523= 16

IF [ [ #1 GE 8.000 ] AND [ #1 LT 8.500 ] ] THEN #523= 17

IF [ [ #1 GE 8.500 ] AND [ #1 LT 9.000 ] ] THEN #523= 18

IF [ [ #1 GE 9.000 ] AND [ #1 LT 9.500 ] ] THEN #523= 19

IF [ [ #1 GE 9.500 ] AND [ #1 LT 10.000 ] ] THEN #523= 20

IF [ [ #1 GE 10.000 ] AND [ #1 LT 11.000 ] ] THEN #523= 21

()

()

N10 (HOME P-COOL)

#120= 20.

WH [ #120 GT 0. ] DO1

M35 (MOVE P-COOL UP 1)

#120= #120 - 1.

END1

()

()

N20 (POSITION P-COOL)

#120= 1.

WH [ #120 LT #523 ] DO2

M34 (MOVE P-COOL DOWN)

#120= #120 + 1.

END2

N100

G103

M99

%

 

At each tool change, You need to call the macro. You will need to modify your post so it outputs like this:

 

T1 M6

G0 G90 G54 X1.75 Y-.6252 A0. S5229 M3

G43 H1 Z.75

G65 P9005

M8

G98 G83 Z-.0857 R.65 Q.1 F20.9

 

 

You will probably need to modify the p-cool values above to suit your particular machine, but you can see pretty easily how it was done.

In the machine's tool-table, the p-cool value is set to 0 and it should automaticly adjust.

[kenfromlodi]

If I put this macro in my M6 macro shouldnt it work on each tool when M6 is called instead of having to put it on each tool change?

[Surface]

Ken, now that's a thought... I don't see why it wouldn't work. As an alternitive, I suppose you could associate the Macro with an unused M or G code.

If you are able to modify the M6 macro, would you send a copy. It sounds a little cleaner that what I was able to hack together.

[Randy Morton @ Clem Industrial]

Surface, would another thought to your 'not perfect' option be to reset the values of the tools used to 0 in the coolant setting? If you can change the number I am sure you can zero it... then you dont have to cycle thru all the coolant pre-sets and zero them between jobs...?

 

Just a thought, good idea btw!

 

I am also interested in the M6 macro if you manage to hack it =]

[kenfromlodi]

I have an excellent macro man that is helping me so im sure we will get it and then I will put it up.

we have 7 HAAS mills here and this will be great. most of our macros are on our SH-630's so this will be fun to mess with the HAAS.

[kenfromlodi]

It seems I may have stuck my foot in my mouth (again) by assuming I could edit the M6 macro on our HAAS control. I am having a hard time even getting to see it let alone edit it. I think its a factory installed macro that I cant call up or see without knowing the proper procedure to make it appear.

We have 90+ cnc's here and only 7 HAAS mills so we are not familiar enough with this control to do this (YET!) Anyone know how to call it up, output it or just replace it?